This collaborative work elaborated by professionals confronted daily to the use of FE methods targets young engineers, who recently graduated from university and often studied exclusively the fundamentals of the FE calculations. Its objective is to answer some recurring questions (such as the mesh size, how to smoothen the peaks, …,) to avoid some issues, and to specify what the FE cannot do. The task force favored to name the project Recommendations and Advices rather than Guide because the document aims to share applications and discuss about finite elements and not create an exhaustive guideline.
The content of the website is dynamic and evolving. The task force is open to suggestions and correction propositions. We are especially interested in complementary examples for Part 3. If you have any recommendations, please contact us on the comments page or by email at elements.finis@afgc.asso.fr.
The three parts can be studied independently.
##### The first part discusses the theoretical elements. The following topics will be considered: - Chapter 1 discusses general information about the method. - Chapter 2 explains the different concepts related to FE calculations in structural dynamics. - Chapter 3 describes non-linear static calculations. - Chapter 4 is about the modeling of civil engineering materials and the questions related to considering phasing. - Chapter 5 explains why post-treatment is necessary to transcribe the peculiarity of “composite materials” that constitute reinforced concrete. - Finally, chapter 6 highlights the possible use of the FE method applied to geotechnical problems. The rest of the document has nothing to do with this specific topic. ##### The second part provides elements to incorporate into a structural analysis using the FE method. Two main reasons push the engineer to use iterative methods with various step verifications and specific treatments: - The first reason is that the FE calculation methods are deduced from the Strength of Materials hypotheses and are not consistently compatible with the regulatory calculation methods. It is true for reinforced concrete for which the regulatory deformation diagram is not agreeing with the one represented by the FE. Additionally, the regulation stipulates calculations that not all the software take into consideration (contributing widths, offset of the bending moment diagram in the strut-and-tie method, crack consideration, …) It is also true for steel for which there are discrepancies between the regulatory assembly or instability calculations and the results found using FE methods, which can be very precise. - The second reason is related to the theoretical calculation, which considers homogeneous elements and does not directly handle materials such as reinforced concrete. In this case, data processing is necessary to transcribe the peculiar behavior of concrete and its reinforcement. The focus must be specifically directed towards steel netting (especially for shells) that can create the illusion that the software is performing the regulatory calculation whereas it is not always the case. The second part starts by advising to create a structural analysis using FE. Later, the first chapter presents the objectives of the calculations to perform. Then, the second chapter describes the modeling of the structure. It focuses on detailing the various materials, the treatment of the interfaces, (to complete,) for the different types of calculations from the simplest to the most complex one. The third chapter discusses the treatment of the results. Finally, the two last chapters highlight in detail the verifications that must be conducted to validate the results and the final formatting of the computation report. The latter will attest to the work that was performed, the accurate inclusion of the structure’s use, the objectives related to the construction phases, and of course the project’s compliance with the regulation. For each step, the authors worked on demonstrating, using examples, all the precautions one must take when using simplifications, and the verifications to conduct to ensure the accuracy of the hypotheses. Those will allow to obtain a rigorous model and results that will be as close as possible to the real behavior of the studied structure. --- #### The authors The Recommendations and Advice were written between 2016 and 2019 by the Task Force about Finite Elements of the French Association of Civil Engineers (AFGC.) Thank you to all from the group who participated, editors, and proofreaders. This paper is posted online so that the users can share with the team all their questions, comments, observations, and suggestions. **Main facilitator of the guideline: C. Le Quéré (Egis) and D. Guth (Setec diadès)** **Facilitators of part 1: G. Hervé-Secourgeon (EDF R&D) and P. Bressolette (UCA)** Main authors from the various chapters: - Chapter 1: P. Bressolette (UCA,) L. Adelaide (IFSTTAR,) L. Jouval (ARTELIA) - Chapter 2: G. Hervé-Secourgeon (EDF R&D) - Chapter 3: S. Michel-Ponnelle (EDF R&D) - Chapter 4: J.-J. Brioist (CEREMA,) H. Somja (INSA of Rennes,) M. Scalliet (CERIB) - Chapter 5: G. Hervé-Secourgeon (EDF R&D) - Chapter 6: Leopoldo Tesser (GDS,) S. Burlon (IFSTTAR) **Facilitator of part 2: S. Juster (CPA Experts,) D. Guth (Setec diadès) and C. Le Quéré (Egis)** Main authors of part 2: - Arnaud Bouard (SCE) - Franck Dubois (VINCI Construction France) - Christian Gallois (Areva) - Didier Guth (Setec diadès) - Landry Jouval (Artelia) - Sandrine Juster-Lermitte (CPA Experts) - Claude Le Quéré (Egis) - Emilie Leroux (Tractebel Engineering) - Pascal Mangin (CTICM) - Pierre Mazurelle (Arcadis) - Jean Michalewicz (ETPO) - Gildas Potin (Tractebel Engineering) - Vincent Rousseau (Bouygues TPRF) Proofreading of part 2: - Valentina Bruno (Setec tpi) - Olivier Cheray (A.Aegerter & Dr.O.Bosshardt AG - Ingenieure und Planer) - Yavuz Demir (CTE Strasbourg) - Franck Dubois (VINCI Construction France) - Sylvie Ezran (Setec tpi) - Didier Guth (Arcadis) - Sébastien Miossec (VINCI Construction France)**\*You?** We are looking for volunteers!
Proofreaders of parts 1 and 2: - Fabien Coulon (VINCI Construction Grands Projets) - Thierry Kretz (IFSTTAR) - Michel Marchetti (Formule Informatique) - Stéphane Velin (VINCI Construction Grands Projets) **Facilitator of part 3: Christian Gallois (ex-Areva)** Main authors of part 3: - Valentina Bruno (Setec tpi) - Jacques Combescure (Artès) - Jean-Paul Deveaud (Cerema Centre-Est) - Franck Dubois (VINCI Construction France) - Sylvie Ezran (Setec tpi) - Samy Guezouli (INSA of Rennes) - Didier Guth (Setec diadès) - Pierre Perrin (Dir Est) - Albert Lepeltier (Setec tpi) - Aymeric Perret du Cray (Setec tpi) - Thierry Richard (VINCI Construction France) - Hughes Somja (INSA of Rennes) - Benjamin Tritschler (Arcadis) # Leave us a comment for us to improve the website #### **Leave us a comment for us to improve the website** It could be: - a disagreement, - a proposal for a better phrasing, - a proposal for a bibliography reference, - a link to a relevant internet webpage, - a practical example illustrated or not, - a question. Please leave your comments as shown below:Date | Name | Contact information (optional) |
Part 1 | Chapter A3.3 | My comment |
Part 2 | Chapter Ex | My comment |
Part 3 | Example y | My comment |
Date | Name | Contact information (optional) |
Part 1 | Chapter A3.3 | My comment |
Part 2 | Chapter Ex | My comment |
Part 3 | Example y | My comment |
Date | Name | Contact information (optional) |
Part 1 | Chapter A3.3 | My comment |
Part 2 | Chapter Ex | My comment |
Part 3 | Example y | My comment |
**Structural analysis is a process in which the engineer establishes a simplified representation of the structure that replicates as effectively as possible its mechanical behavior.**
##### **Modeling** According to the Eurocode, structural modeling must imply calculations that are conducted using appropriate computational models including the related variables. It is expected that structural models can predict the structural behavior within an acceptable range of precision. Moreover, the models must be adequate to the considered limit-states throughout all the steps of the project. The structural models used must be based on a theory and an established practice and must be verified experimentally if needed. Modeling is then an approach or even a procedure, that consists of establishing a model. According to its objectives and the means used, modeling can be handled using distinct methods. It is all about representing an object, a real phenomenon, or a phenomenon extracted from its environment and simplifying it using an isolated system that follows a concept or a theory. It is developed starting from the acting physical phenomena, which means that it incorporates physical laws. Thus, the constitutive laws are formulated under mathematical equations compatible with each material and each structural element of the overall structure. This leads to solving complex continuum mechanics systems of equations written as partial differential equations. The main peculiarity of civil engineering calculations compared to other engineering fields is the need to consider all the phases of construction such as the clearance and filling works, the concrete work of the foundations, attaching braces, tensioning, or anchoring cables. Modeling transcribes these events in the static language in various ways: by the continuation of computation with internal constraints (“initial constraints”,) by changing the stiffness of some elements (go from a zero value to a positive one,) by getting rid of or modifying the nature of some supports, by changing the points of application of loads, etc. “Modern structures” in civil engineering (built after the second industrial revolution) present favorable features to their structural analysis: homogeneous geometry, repeated patterns, qualitative construction materials (conformed to the “product standards”.) These structures are however affected by multiple factors that are hardly or cannot be controlled: environmental factors such as the type of soil, the quality of the construction itself, as the structure might be built-in zones of limited access or under unfavorable meteorological conditions (e.g. the sensitivity of wooden elements to humidity, which can impact the dimensions and the mechanical features of the element under normal conditions by creating gaps or shrinkage, or steel elements that expand when subjected to high temperatures…,) and the heterogeneous aging of their various elements. To face the issues related to designing and the equilibrium verification of real structures, the structural analysis relies on creating models, which means creating simplifications of the real structure: design of materials, ideal kinematic assumptions (perfect connections, bilateral, independent from the reaction forces,) and even arbitrary choices about what factors are involved in the equilibrium of the structure (by not considering some elements or by neglecting the involvement of some components on the structural behavior.) These simplifications imply that there is only a contingent relationship with the real structures in their environment. Consequently, the output results from the modeling must always be analyzed critically while keeping in mind the explicit assumptions and the less explicit ones that were made: firstly, isolating the system from its environment, then selecting a mathematical model and a solving method… The exact solutions are extremely rare (only a few textbook cases,) it becomes a necessity to solve real problems using approximated methods: - either analytically: for instance, using Strength of Materials formulations for which geometrical considerations lead to a simplification of the problem from 3D to 2D (average surface of plates and shells) or even 1D (average fiber of beams) … - or numerically: FE methods, finite difference methods... To validate the obtained results, one can compare them to experimental values. It is important to note that different sources of error exist in this comparison such as: - modeling errors: coming from the modification of the real problem into a simplified one, - discretization errors: due to the numerical resolution of the problem, - measurement errors: related to the equipment and the measuring process. The obtained results should, ideally, be compared to the experimental measurements that can also be filled with errors… Moreover, it is possible to combine two families of methods: FE for beams, finite differences for plates…**The simplification should allow to solve the problem to evaluate numerically the effects (efforts, stresses, displacements) of different load cases on the structure. However, it should fit as well as possible the behavior of the real structure.**
**![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/G8Xuz978iXQXNMuu-embedded-image-2tg3tcro.png)** *From the problem to its approximated solution* ##### **Finite Element (FE) Method** The FE method is a modeling tool that allows us to solve numerically problems that are set using partial differential equations. The FE method can be applied to civil engineering design since modern construction materials such as steel or concrete allow to work in the continuous framework, which is the underlying assumption of the FE formulations. Thus, it is implied that before using this method, the engineer had a preliminary reflection about it and is aware of the modeling procedure. The FE method is a general numerical method allowing to handle real-life (“industrial”) problems from various fields (solid mechanics, fluid mechanics, thermodynamics…) in continuous frameworks, static or dynamic, linear or non-linear, as well as coupled problems: thermo-mechanical behaviors (structures subjected to fire,) fluid-structure (vibrations of a tank containing liquids,) chemical-mechanical (considering corrosion of rebars in reinforced concrete)… The surge for the FE method is closely related to the improvement of computer science since the 1980s and led to the creation of numerous software. This guideline covers only the use of the FE method, however, this is not the only structural analysis method: besides some traditional approaches such as the graphical statics, the use of graphs and tables or analog techniques on models (recognized by the structural Eurocodes,) there exist much more tools (spectral methods, Boundary Element Methods (BEM), finite difference, etc..) Some methods are still being researched, but the FE approach is the most general and the most used in the field. Comprehensively, the principle behind the FE method can be summarized as follows: the domain of analysis, originally complex, is divided (discretized) into a wide range of subdomains with simple shapes (**finite elements**) from which points are identified (nodes): the **meshing** is now defined. The approximated solution is calculated only at the nodes (discrete solutions.) The solution at any other point can be recovered by interpolating the values at the nodes. More specifically, the different steps of the FE method are: 1. Discretizing the structure in several nodes linked by elements that have well-known behaviors. Establishing the column displacement vector D containing the N degrees of freedom of the structure. The degrees of freedom are the possible displacements (translations and rotations according to the model) of the structure. There are the unknowns of the problem that belongs to the R^{N} space. 2. Establishing the behavior of the elements. It can be divided into two parts: 1. Determining the displacement forces fed: the forces applied by the nodes linked to the element on this element to inflict its displacements d_{e}. The relation is established in a local coordinate system specific to each element, then transposed to the global coordinate system: F_{ed}=K_{e}.D_{e}. One can now go back to the relation given in 1 p 8, but for an educational purpose, it might be preferable to handle separately the issue of the combined behavior of the elements (which is addressed by picking the solution in some kind of behavioral library.) 2. Determining the constraint forces f_{eb}: the forces applied by the nodes on an element directly loaded, to prevent any displacement. The nodes, in this case, play a virtual support role for the element, and one can calculate the reaction forces in a local coordinate system of the element f_{eb}, then in the global coordinate system F_{eb}. 4. Assembling. Establishing the structure’s stiffness matrix and the forces applied by the nodes onto the elements according to their loading. This process is conducted by summation, in the R^{N} space for vectors and R^{N} x R^{N} space for matrices, of the elementary stiffness matrices and the constraint force matrices: K=∑K_{e} and F_{B}=∑F_{Be}. 5. Writing and solving the equation of displacements, which is the equilibrium equation of the nodes. The nodes are applying forces onto the elements, which leads to a displacement D (KD) and constraint forces, namely reaction forces, as a consequence of the loads directly applied to the elements (F_{B}.) The nodes can be subjected to external forces that would be directly applied to the nodes (F_{N},) such as reaction forces at the support for instance. The general equation writes KD=F (with F=F_{N}-F_{B}.) 6. Solving: displacement calculations: D=K^{-1}F. In practice, one must distinguish the degrees of freedom with known values (the supports) from the others. Let D_{1} denote the unknown degrees of freedom and D_{2} the known degrees of freedom. One then organizes the working space in a way that the unknowns are first. The general equation then reads: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-10/flKgI6Cbb823JqSV-embedded-image-xuzwfpxh.png) In this equation, F_{1} and D_{2} are known. One must then calculate ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-10/Xgbyiz6L8eXQGJM4-embedded-image-fvycpj3n.png) then F2. 7. Knowing the displacements, it is possible to determine the efforts in the elements by using the fundamental behavior equations of each element. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/8ocS6Yri9851zlIT-embedded-image-qoot2dbp.png) *Geometry and meshing (triangular finite elements and nodes.)* This guideline describes the available tools often used in the computational FE software in statics and dynamics. To save space and be as clear as possible, we have chosen not to introduce any problem related to interstitial flow despite their great interest in geotechnical work. Regarding the difficulty of modeling, the geotechnical field (also covered by the FE method) raises challenges, on the one hand, analogous to the issues met in dynamics of structures (choosing the time discretization,) and on the other hand, elastoplastic issues (heterogeneous permeability, boundary between saturated and non-saturated zones, etc.).**The FE method is a tool for numerical calculations. The modelling prior to solving can rely on all the principles of the preexisting structural analysis.**
# PART 1 – THEORETICAL ELEMENTS # Chapter A. Introduction #### **Chapter A. Introduction** When performing a FE calculation of a structure, the modeling assumptions as well as the objectives must be defined. Those goals generally consist of solving: - the displacements caused by a static loading (permanent) quasi-static (without inertial effects) or dynamic (fast-loading,) - internal state, such as stresses, damages inflicted (cracking, etc.) Among the modeling hypotheses, it is preferable to handle chronologically: - the choice of the general formulation, - the dimensionality of the model, - the choice of the elements, - the definition of the interactions with the environment. **A1. A general formulation for linear elastic calculations** [A1. A general formulation for linear elastic calculations](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a1-general-formulation-for-linear-elastic-calculations "A1. General formulation for linear elastic calculations") **A2. The dimensionality of the model** [A2. The dimensionality of the model](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a2-the-dimensionality-of-the-model "A2. The dimensionality of the model") **A3. The choice of the FE** [A3. The choice of the FE](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a3-choosing-the-finite-elements "A3. Choosing the finite elements") **A4. Interaction between the structure and its environment** [A4. Interaction between the structure and its environment](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a4-interaction-between-the-structure-and-its-environment "A4. Interaction between the structure and its environment") **A5. Estimation of the quality of the approximated numerical solution** [A5. Estimation of the quality of the approximated numerical solution](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a5-estimation-of-the-quality-of-the-approximated-numerical-solution "A5. Estimation of the quality of the approximated numerical solution") # A1. General formulation for linear elastic calculations #### **A1. A general formulation for linear elastic calculations** The two main formulations for linear calculations are displacements-based and stress-based. Most of the software nowadays rely on a displacement formulation because it can easily consider the boundary conditions, unlike a stress-based formulation. Mixed formulations, using displacements and stresses also exist. There are other formulations, but they will not be discussed in this chapter. In this document, only the displacement formulation (the most commonly used) is introduced: in this context, the basic unknowns are the displacements at the nodes, typically represented by q, from which all the other values are deduced (strains ε, stresses σ ....) The displacement at any point of an element, represented by u(x,y,z), are obtained by interpolation between the values at the nodes using interpolation functions (known as shape functions) represented by N(x,y,z), which are low order polynomials (generally of degree 1 to 3): **![](https://lh5.googleusercontent.com/V5NmIPbRaSI7SR73_-yvW8Vmjl42vpjoPCl7BXJvaYmtEQ_GUvaSEc9zNqIe7huM0A5ST1x6VFu-V9vCxzEGHBuJeI9IftMRrANh4tjRQ9PdzAQjDdRvMPSaUHeWlqQNiOYPhUbn2jLZmIX6YISXbw)** The strain-displacement relation is obtained by computing the derivative using the differential operator (matrix) D (different according to the situation,) from which the matrix B appears, connecting strains and displacements to the nodes: **![](https://lh6.googleusercontent.com/nasaaovNf7Rsc-9g8PU0Y92XUH4hRUhdrWm-sX8fYGkUvYHfsccIoDa20vrOm-Fs-dfy6QV_CSRs79ntprZMRTeQH75gcGOhaJ31eEKq6SVbRsDBoJ64pVfwZ3D5rGqf6A6i3nJ2FS7T9SbdZnHVXA)** To obtain the stresses, it is essential to introduce the constitutive law of the material. Thus, in linear elasticity, the strain-stress relation is written (H representing Hooke’s matrix): **![](https://lh3.googleusercontent.com/VHlBq6I_KS33P1I1VbIi7GFggBqmB2afOn1S32bp2ReG75JxZu5USL7f5PA12PhCJKYZFWu2vE9Rqm_bbx7TK1HKsGA1XApZgkRsuPjeAz8yacNYlD4UVy9BHn80r5la-2pbugb1WUIri1zxLrxUtg)** One can observe that all the interesting quantities (displacement at any point, strains, stresses) can be obtained from the displacements at the nodes of the mesh.**Note**: as the deformations (and consequently the strains) are obtained by computing the derivative of the displacements at the nodes, there is a loss in accuracy when calculating those values.
For a static calculation in mechanics of structures, identifying the numerical solution of the problem by the Finite Elements Method (FEM) can be summed up **in 4 main steps**: **Step 1. Determining the elementary matrices and vectors of each element of volume V by applying the following equations (with BT representing the transposed of B):** ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/jdA5Nd4X31CiGeDe-embedded-image-52nsi37g.png) elementary stiffness matrix **![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/NA0A3j5uu667Ym1C-embedded-image-pddnlwvw.png)** elementary vector of equivalent loads with f^{V} the volumetric load vector and f^{S} the surface load vector. The vector of equivalent loads allows us to “bring back to the nodes” the loads applied to the elements (in the volume or the surface,) according to the chosen interpolation.Be careful! Usually, it does not correspond to an even distribution at the nodes of the total load applied on an element.
**Step 2: Determining the stiffness matrix K and the force vector F with respect to the global coordinate system by assembling the elementary quantities and introducing the boundary conditions.** **Step 3: Determining the vector of nodal displacements q by solving the linear system (large scale): ![](https://lh6.googleusercontent.com/vejAPNjKYoqede8Rs9BAezAR7Ks3LHFUYMI-NIWR8Z1CR9Rc-hfaIX6VbpdMj1wAv8AkHGVGgsFnfuBgOGZu9yCoPgthGQf3FlsoBbe9quISLrlgkrRG2x2cEiSgLkGZ-YC4Juv57izetPICyYXjhQ)** The vector q gives the node displacements of the mesh, likewise, the vector F contains the values of the equivalent loads. **Step 4: Resolution of the quantities of interest such as strains and stresses by post-processing the vector of nodal displacements q.** Going back to the elements, the displacement, the strain, and the stress values at any point can be deducted from the displacements at the nodes by using the previous equations. As opposed to the displacements, the stresses and the strains are calculated element by element (and these quantities are not always continuous from one element to another.)Note: it is possible to make an analogy between solving, using finite elements, a mechanical problem, and a thermal problem in a linear permanent regime: in this case, the temperatures T at the nodes are obtained by solving a linear system: Λ. T = Φ, with Λ representing the conductivity matrix and Φ the flux vector at the nodes.
The order of the shape functions N(x,y,z), which is deducted for the solid elements (or continuum mechanics – CM) from the number of nodes in the edge of a finite element (2 nodes: linear element, 3 nodes: quadratic element) has an impact on the degree of strains and stresses evaluated using finite elements. For example, if the differential operator D corresponds to the first-order derivative (which is the case in CM,) the strains and stresses will be constant along with the element for linear elements, and linear along with the element for quadratic elements… As a reminder: in Strength of Materials (SM) to compute the strains we make use of the second-order derivatives (bending of beams, plates….) ![](https://lh3.googleusercontent.com/GlzU9IPtuVkGBIXBzoCWF-ZGBYVyHIjpyNYPI_4uLIwtm3LgzYlI5rnlf9agcbYqSvqP_rpUrRWqwwV8PnhwtTJUk9JAuxXydDpFvwL46uTT5eJtK4mxbnXYytIyymnkswTteAeAMrz3Wn-CiPQFEA) *Shape functions – Triangular element with 3 nodes (linear functions)* **![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-10/7MBXCA8SROchTPLk-embedded-image-n2dgzyxd.jpeg)** *Shape functions – Triangular element with 6 nodes (quadratic functions)*Be careful! It is not possible to mix in the same mesh finite element with shape functions of a different order (for example linear and quadratic elements.) Actually, the continuity of strains cannot be ensured at the interface between elements with shape functions of a different order.
In the software, most finite elements are defined with the same parameters (**isoparametric**,) meaning that the different finite elements of a mesh are built as a geometric transformation of a reference element (which is itself expressed in unitary coordinate system ξ,η,χ.) ![](https://lh4.googleusercontent.com/1_tBsDTSJajml9OpYJtsqSjXN0Fx8kz4AOkDkH6grbnET-alnFzsP-TPDD_kMTadjR6C2re-qPItKtVZZEtJdQjCk8psw1Y_ewuzHWZFobRudzsxx7TDJfljpALwnbQau0zKsKqv_GcpY2-QPQR-HA) *Isoparametric element (quadratic): different transformations (2D)* These geometric transformations, which generally rely on the same nodes used for the interpolation of the displacements (hence “isoparametric”, with the same parameters,) are characterized by their Jacobian matrix J (matrix of the geometric transformation’s partial derivatives of the first order.) **![](https://lh3.googleusercontent.com/RWa4CMkgp9o_eeRbbZbevSCNJ1eJt9p6VdA0YTd-bf0_sMSrxYL-YrY_aozDunxkWvx2iIp1m0pOZTrbtMPTAsqwMCxiNy2nQQRx8mQJJhECxHnswwoF0f3W32jqxDdyP85j_G9C8-ONkxW1HR-qlQ)***Isoparametric element (quadratic): local and global coordinate systems (2D)* One of the advantages of this transformation is the possibility of approximating the boundaries of a given domain by using polynomial geometries. However, the main problem is that the calculation of elementary matrices and vectors can become more complex. Their evaluation is made by numerical integration using a quadrature scheme: weighted summation of the values at a certain point located inside the elements (weights ω\_i, points, ξ\_i) particular to the method (Gauss method, Hammer method….) In this case, the calculation of the elementary stiffness matrix and the elementary vector of equivalent loads are written: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-10/VWX0gEgRchgLfABN-embedded-image-r1c6gb2m.png) When the matrices (by applying the B matrix) are evaluated this way, it is obvious that one must calculate the strains and stresses at the same points (also as a function of B.) The software provides these quantities at the integration points (Gauss or Hammer points, according to the integration scheme.) Moreover, talking about the values at the nodes of a mesh for strains and stresses does not make sense because there are as many values in a node as the number of elements connected to it. Be careful, there is not necessarily a continuity between the elements! Wanting at all costs a nodal value (of strain or stress) of the mesh implies some data processing: extrapolating from the values at the integration points and the average values of different elements sharing the node, which will, at the very least, smoothen the results (nonetheless, talking about values at the nodes in a particular element is justified.) When the quantities are obtained by analytical integration (in the case of beam elements for instance,) they can be expressed at the nodes, at the center of gravity… the previous observations about the continuity between elements being still valid. **![](https://lh5.googleusercontent.com/hsTNPdJxg-tBzNI15Q3p0l8oAK4HrFFJfPKBcwQ081OqqAmZgYYthkPsXdr5dW6dcLiCM0g5xSMUHgUdEdCg8BO4RtheHfh9Bjb_mPvz6buMLEvUf2_9ex3bexLfSwOv00oGBVS1YHJ3rx3_R92Q3w)** *Quadratic elements and integration points (Gauss points)* The way to consider the displacements at the boundary conditions (restraint, support…) might lead to different results depending on the adopted numerical technique. There are two ways of considering the displacements at the boundaries: - Penalization method: it is simple to implement but it has the limitation of being sensitive to the order of magnitude of the stiffness matrix terms. - Lagrange multipliers method: it is not affected by the above-mentioned accuracy problems, but slightly increases the size of the system to be solved.Note: in dynamics, the displacements at any point x,y,z at any moment t is obtained, as in statics, by interpolating the values at the nodes: ux,y,z=Nx,y,z.q(t). These nodes verify the equilibrium condition, given at any time t by: ![](https://lh6.googleusercontent.com/kFhsTELNZvyKKTj2UntV4oZ3mMst6S84kfst52LTvjboQhD_X4rUhHkhT7QzkctzCH78d_lEoOIbAqhBIgENrFWdQ11YrZbhZJ2u070AnfRj8XV-bSytItqrGA7fDuuFbi6JWiLsCPsjn-wlScH7Dw) The mass matrix can be obtained by assembling the elementary mass matrices M_{V }(volumetric mass) and C the damping matrix (viscous). To compute the aforementioned matrix, a system of differential equations needs to be solved using adequate numerical methods (see the chapter on dynamics.) ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/jROz6VD6qWCUAFMM-embedded-image-diul21hy.png)
# A2. The dimensionality of the model #### **A2. The dimensionality of the model** It is very important to simplify the full-size problem to model the interaction between the structure and its environment. To do so, there are 2 known techniques: - the first one consists of transforming the full-size problem into a lower-dimensional space by modeling it as an **axisymmetric structure** or a **2D structure** (plane strain or plane stress assumptions). This technique reduces the used space (see section 2.2). - the second one consists of working in a **3D** space while still reducing the model thanks to kinematic hypotheses. For instance, it is possible to adopt simplifications **such as beam, plate, or shell theories** (see section 2.1). Those 2 techniques help reduce the computational cost. However, the user has to be very careful when adopting those simplifications. For instance, the second technique uses hypotheses that are valid only in a limited domain. It is important to make sure that the adopted simplification stays within the domain of the full-size problem to obtain relevant results. ##### **1) Case of finite elements applied to Strength of Materials** From a finite elements method perspective, the main difference between Continuum Mechanics and Strength of Materials relies on the geometry, which is simplified through additional hypotheses: the initial 3D problem is then transformed into a 2D problem (mean surface for plates and shells) or 1D (mean fiber for beams), but still represented in a 3D space (except for 2D problems, as mentioned above). When the FE method is used to solve a Strength of Materials problem, the finite elements have specific characteristics. It is necessary to assign to those elements geometrical properties (the section, the inertia for beams, the thickness for plates and shells). Moreover, they combine the effects of tension/compression (for beams) or membrane effects (for plates and shells) to the bending effects. The traction/compression and membrane effects are treated as they are treated in Continuum Mechanics, while the bending effects are handled separately. For the computation of bending effects, simplifications in the geometry lead to a particular definition of deformations, which results in different expressions of the differential operator D according to the situation. Another consequence is due to the definitions of the unknowns at the nodes: while in Continuum Mechanics the unknowns are the displacement components, in Strength of Materials the unknowns corresponding to the rotations are added. This happens because it is no longer possible to evaluate directly the rotations as a consequence of the simplifications of the geometry. The initial choice of treating the problem in the frame of Continuum Mechanics or Strength of Materials implies choosing between different families of finite elements. It is, in principle, not possible to mix finite elements of different families because at the interfaces between elements of different nature the rotations are not transmitted unless they are adapted to take it into account. Moreover, the calculated stresses inside the element are usually generalized stresses (or Strength of Materials efforts: axial, shear, torsion, bending). To obtain the stresses (in Continuum Mechanics) at a given point, it is necessary to provide additional information (position inside the beam’s cross-section, for example). In this scenario, choosing a finite element brings on an additional difficulty related to the consideration or not of the shear forces (Euler-Bernoulli or Timoshenko beam theories, Love-Kirchoff, or Reissner-Mindlin plate theories). This choice is related to geometric considerations (slenderness of the cross-section or thickness of the plate). Moreover, taking into account the shear forces might lead to numerical errors (shear locking), which renders the use of some finite elements complicated.The Euler-Bernoulli beam finite element allows to represent exactly the bending moments that vary linearly along with the mean fiber of an element (shape functions of order 3 for the bending displacements and the bending moments obtained by taking the second derivative of the displacements): it is therefore not useful to introduce several elements between 2 nodes subjected to point loads (a dense mesh should be used when the loading is distributed between these 2 points).
Finally, for plate and shell elements, the monotonic convergence is not guaranteed depending on the mesh geometry. This behavior is connected to the formulation of the element itself. This kind of behavior is illustrated in the figure below, showing the evolution of the relative error of the deflections ω and Mx as a function of the number of degrees of freedom (in the case of a rectangular plate supported by its four sides submitted to uniform loading): in green, a non-compliant element (COQ3) for which the results are much less precise than for a compliant element (DKT). Also, for a non-compliant element (COQ3) the convergence is not monotonic (for the bending moments Mx in the figure): more elements leads, paradoxically, to results that can be less precise! ![](https://lh6.googleusercontent.com/0X_1c90ka--SZOx85j_fMDx2BrX_Pnl1n1chOav53v4m77LPDKqVGgS3qPfyeRQCaz6Jem8sG4OjJGXJZz-eEpn-uxu8eK6zAvxAVJkwqsHZETmZjuMxEGd05qWtPN4RP8n_g-ID17OAkAt_-Q55ow) *Bending plate: convergence (deflection ω and bending moment Mx) as a function of the number of degrees of freedom* This domain is particularly important to civil engineering, but it presents specific difficulties that will be explored in the next chapters. ##### **2) Two-dimensional calculations** The studied problems are three-dimensional, however, it is faster to calculate two-dimensional problems. In some cases, it is possible to transform a three-dimensional problem into a two-dimensional problem: - if the problem admits a revolution axis (for the geometry, the loading, and the boundary conditions): it is possible to perform an axisymmetric calculation with no additional hypotheses needed. In the case where the loading is not axisymmetric, it is possible to decompose it in the Fourier series and treat the initial problem as a superposition of axisymmetric calculations. ![](https://lh5.googleusercontent.com/TmuUMEdHPlPjJ61i2TtvRnOYdjQGVhkN9KhqzW_1yFPM-Jnx1CAKT-zfVHBIGSZXePDH4Sepgt3WQJ-p2V5RAHsz_1aAIh96UT5sJ5tCSXXgyJGeQKMg92jdwQJQzUj26BD-IwXmWSY5g2nPRVlUWw) *Cylinder under axisymmetric pressure* - if one adopts the hypothesis of neglecting the stresses or the strains that are out of the plane, for cases in which the structure is either very slender or very thick, plane stress or plane strain assumptions can be made. The obtained solution is then an approximation of the three-dimensional problem. It is important to keep in mind that in-plane stress, the strains outside of the plane are equal to zero (similarly, in-plane strains, the stresses outside of the plane are equal to zero). ![](https://lh3.googleusercontent.com/e1GOyHhtJyckNotS4_zYSJlSHeYrvurUUyVupP5JM5wIO8kn7Y5aRlk9MO53UDKAIsCM4wTdiOHwgq1qqORFmbH0xm3KiA6Ol_DpBpjZnavb-H1Kr6o_1K3iL5klbNXgCD6RyCqOvYOZUNjRmGRK7w) *Dam: important thickness of plane strain assumption* *![](https://lh5.googleusercontent.com/Q3Hm2uB0JnXzJLmdxdRjFSx0ZMxeyEYWIvSZOasc0chRS8d4CX99sIBojaGNl3HIglwWUxrytQHAlmsq8R5Tj2DrZHzk782h4E3cZBnoEzRepTLR8bdrX35s2DVsFzN7qV5LGV8878RpgbyD8NA40g)* *Assembly: low thickness/plane stress assumption* ##### **3) Taking into account the symmetries** Some problems present symmetries (axis of symmetry, plane of symmetry…) and it can be interesting to use them to make the finite element calculations faster. Although, it is important to notice that solving symmetric problems will provide only symmetric results (especially when computing eigenmodes). For that matter, it is important to keep in mind that to use those symmetries in the calculations, not only the geometry has to be symmetrical, but also the loading and the boundary conditions as mentioned above. The resolution of this model will not represent the solution of the whole structure unless the symmetry conditions are added to the model. In Continuum Mechanics, one should impose the displacement components perpendicular to the axis/plane of symmetry equal to zero. In Strength of Materials, it is convenient to add no-rotation conditions around the axis/plane of symmetry. Finally, taking into account symmetries might impact the loading: for instance, a punctual load should be applied with half the intensity if applied to an axis of symmetry. # A3. Choosing the finite elements #### **A3. Choosing the finite elements** **Choosing the element** is an important step. The goal is to select the **type** of element (its shape, the order of the shape functions associated), and the **size** of the element. The **type** and **size** of the elements define the form and the precision of the displacement fields, and consequently the stresses and strains. Moreover, besides the shape, the element has an **aspect**. It should be avoided to create **decayed** or **altered** elements (flattened or elongated) because it degrades the precision in the resolution of the problem. Generally, the generated mesh can be **structured** (a regular division of the elements) or unstructured. It is possible to mix structured and **unstructured** parts in the same domain depending on the complexity of the geometry. In the same context, the **size of the element** chosen depends on the **geometry** of the structure to model and the loadings it is subjected to. The zones with high-stress variations (gradients) or high stresses (friction or cracking, for example) determine the parts where the mesh needs to be more refined in comparison with the other parts to properly observe the stresses and the strains. It is important to perform the first simulation with an initial meshing to determine the sensitive zones and then refine the mesh where needed. The person in charge of modeling must analyze the meshing critically considering the geometry of the structure and the important zones to observe. To choose correctly the finite elements construct the mesh, it is imperative to think about the type of calculation desired: - the whole geometry is going to be represented. It is a Continuum Mechanics problem, so the elements are of the “solid” type and the problem must be predefined as three-dimensional or two-dimensional (plane stress, plane strain assumptions, axisymmetry… see chapter 3). If one wishes to use linear or quadratic shape functions, the precision of the calculations improves with a mesh of quadratic elements, but with an important addition in the computational cost. Thus, a compromise has to be made. In any case, the degrees of freedom are the displacement components (u, v in 2D, u, v, w 3D). The main elements are listed below, ![](https://lh5.googleusercontent.com/FZrRwXV9y76x7Nhzop4356QXyL6KAaimIgTXqPY_6tea3fxKbvr859_S9s3rc_5DReP5ROiBHNCzpAgT3chMwmkHFSnmQB9WB1Xv0M10xYa7ZPs2-Y6RWAZE5fZ3fng1mcWa2qirlRsbIjJYqgWz6w) - the geometry is simplified, in which case one has a Strength of Materials problem (or structural analysis, see Chapter 2) and the finite elements are: - bar/beam elements (a bar element can only transmit tension or compression, whilst the beam element is also capable of transmitting bending moments. Be careful, some software use the term “bar element” to designate any 1D element), - plate/shell elements (the difference between plate and shell is related to the curvature of the mean surface and most software do not make any distinction between the two). Besides the displacement degrees of freedom, the Strength of Material elements have also rotational degrees of freedom (θx, θy, θz), allowing to take into account the non-meshed geometry (cross-section for beam elements, thickness for plates and shells). Moreover, one should ask the question if the shear forces should be taken into account or not (Navier-Bernoulli or Timoshenko beam elements, Love-Kirchoff or Mindlin-Reissner shell elements). In the case of shell elements, as mentioned before, the question about the quality of elements comes to mind (compliant or non-compliant elements). It is particularly difficult to choose between plate and shell finite elements, especially because the literature is scarce in this area. It can be helpful to perform a calculation with known results to test the quality of the available elements. The different elements that are commonly found in Strength of Materials are described in the table below. ![](https://lh4.googleusercontent.com/LUJPz4wLjhvuhIIMm98qOyrWn4nyzzRF1snHMUJXEYeaXyriFuxxWojYdJMfdqoPbrKSnXQ6vj41qXdAkKhhulXj-qzFaNx25BDNz_PDq0njdjjbodmgLlegDvEL69cT2xAsIxayI2_YjJPC90S2bw) # A4. Interaction between the structure and its environment #### **A4. Interaction between the structure and its environment** Taking into account the **interactions between the structure and its environment**: this consideration allows us to reduce the number of discrepancies between the model and the real-life structure. The effect of the environment on the structure is determined from the nodal values such as the nodal displacements and nodal efforts. The first ones are connected to the boundary conditions and the second ones to the external loading \[1\]. - the displacement **boundary conditions** (nodal) make it possible to impose displacement values to a node (zero or non-zero). The imposed displacements are often named **kinematic constraints**. They enable to connect the displacements of certain nodes. Initially, it is preferable to determine if the **symmetries** should be taken into account before imposing the boundary conditions. When symmetries are adopted the nodal displacements perpendicular to the plane of symmetry in 3D or the axis of symmetry in 2D should be blocked (figure 3) (see chapter 4). ![](https://lh6.googleusercontent.com/-0wqv1ol9Bc-it6UTmsVbkdPWF5q_R_jVYVTbernSE5bLKVc19zap1niFIYunKoskRxMa_W2hM2d0mZQ8ww7DeKeJsjcoL3g-l0dQeMOBtZwQlkAUL5TKiW9poYDg4a-ScA2VkELfkPQEn_zQgZwgg) *Boundary conditions for a plate with a hole in the center, 2 axes of symmetry, submitted to tension* Afterward, it is essential to eliminate the **rigid body movements**. A correct finite element model has to restrain free rotations. In 3D, the 6 rigid body movements previously introduced should be avoided (in 2D, there are 3 movements, figure 4). ![](https://lh3.googleusercontent.com/Fi1Rn5UyJ1UHAB7sM50XcgS66OFjjkuvz_pvO5UnrSXAs-Hz-l-ouXYhEH6Da0Xx0UUY84jUErLQgpLfBrqPbQ1d54fONMb9uMnz10jlcILhWIlpkmwcLnaNql6JnmjRLU8cnpe2i5oK84sWRHbtbQ) *Possible rigid body movements in 2D: a) possible horizontal translation; b) possible vertical translation; c) rotation around a hinge; d) all rigid body displacements restrained* Once these 2 steps are accomplished, it should be verified that every rigid body movement is correctly restrained and that no rigid body movement was blocked when this mode has already been removed. In the first case, the problem has no solution and in the second case, unexpected strains may appear. - the **loading** corresponds to exterior efforts exerted on certain parts of the mesh. Among the loadings, forces such as gravity and inertia should be taken into account. They are in general modeled as **volumetric forces** represented by nodal forces applied to all the nodes in the domain. There are also **contact forces** such as pressure or any other force that needs contact with the structure. They can be **surface, linear, or punctual forces**. Their application should also be transformed into nodal forces. Special attention should be paid to the transformation of the contact forces when creating a model respecting its validity domain. Using a point load can generate singularities such as stress concentration in the neighborhood of the node where the load was applied. Thus, to avoid this kind of **singularity**, it is necessary to apply the point load as a surface load in the neighborhood of the node. This technique consists of applying a surface load containing a relatively large area around the application point. Then comes the question of **mesh refinement** in this area and its influence on the obtained results. ##### **Connection conditions** There are different types of finite elements, such as volumetric, plates, shells, beams, and bars. Thin plates and shells are elements, which have a thickness smaller than their other 2 dimensions. A plate works only perpendicularly to its plan (3 degrees of freedom (DOF) for a node: 1 translation and 2 rotations), whereas a shell element works along its plan and perpendicularly to it (6 DOF: 3 translations, 3 rotations). The solid elements also have 6 DOF per node. Chapter 2 presents some practical examples. # A5. Estimation of the quality of the approximated numerical solution #### **A5. Estimation of the quality of the approximated numerical solution** The difference between the exact solution of the problem and the approximate one obtained through the finite element method allows us to assess the quality of the solution: this is called “discretization error”. Since in the general case the exact solution is not known, the idea is to estimate this difference by computing an “error estimator”. The error estimators can be categorized as: - global error estimators: to evaluate the quality of the solution on the whole domain (stress smoothing method, equilibrium residuals, constitutive law errors…), - local error estimators: to evaluate the quality of a particular quantity, such as displacement on a certain point or stresses in a particular zone (weighted residuals method…). The “error estimator” tools (available in some software, with different computational costs in each one) can be used for two different purposes: - to improve the quality of the results of a finite element calculation by refining automatically the mesh and or the time discretization, - to obtain an interval of confidence (inferior and superior boundaries) associated with a global error or a particular quantity of interest. It is important to highlight that certain error estimators, such as the stress smoothing method, only estimate the error, while others, such as the weighted residual method, guaranty the numerical results by computing the range of error. # Chapter B. Structural Dynamics #### **Chapter B. Dynamics** For many applications such as seismic calculations, collisions, vibrations… it is necessary to consider the dynamic phenomena. The dynamic charges applied to a civil engineering structure belong to two different categories: - phenomena that can be compared to static events: constant wind flow, swell, rotary machines. - transitory phenomena: collision, explosion, earthquakes. Concerning seismic motions, if they are theoretically considered as transitory, it is admissible to assimilate them as stationary phenomena while in their strong phase. For the cases in which one tries to model the structure with geometric or material non-linearities, stationary assumptions cannot be considered anymore. The means of representing the loading categories can then be distinguished as shown below: - Stationary: \- Complex Fourier Transform (FT), \- Power Spectral Density (PSD), \- Oscillator response spectrum (ORS). - Transitory: \- Load-displacement curve, speed or acceleration expressed as a function of time, \- Efforts or pressures are expressed as a function of time. Two big families of analysis can be considered: - The modal analysis, which enables to identify the natural frequencies and the associated modes of a structure. This data is useful to characterize: \- The stationary loading response applied using a method of spectral response, \- A temporal response using the Duhamel integration of each loading curve corresponding to the modal responses. \- A transfer function convolved to the signal expressed in terms of the frequencies to deliver an FT or PSD response. \- The time-dependent dynamics that enables to compute the structure’s transitory dynamic response to any temporal vibration. The resolution can be conducted using schemes of time integration, which can be explicit or implicit. The explicit schemes dictate the choice of very small-time steps. Thus, they are the most used to solve problems with small periods (like collision/impact problems.) On the contrary, implicit schemes allow us to use greater time steps and are therefore favorable to study problems occurring on wider time ranges. **Examples of applications****Applications** | **Loading** **representation** | **Quantities** **available** | |
**Modal** | Vibrations analysis | FT | FT |
PSD | PSD | ||
Tracking of natural frequencies | ORS | Spectrum extrema of quantities of various interests | |
**Implicit** **transitory** | Seismic Study | Accelerations, velocities, forces, pressures, or displacements as a function of time | Quantities of diverse interests expressed throughout time |
Weakening | |||
**Explicit** **transitory** | Fall of on object | Modeling of projectiles in contact, collisions | Quantities of diverse interests expressed throughout time |
Plane crash | Accelerations, velocities, forces, pressures, or displacements as a function of time |
Be careful! The modes are defined with a precision level of more or less a multiplying constant. Moreover, they are later normalized using various procedures. The most common for FE software being the normalization according to the mass matrix. This procedure is detailed in the following section. The modes can also be normalized using their greatest modal displacement.
The vibration modes are orthogonal to the mass matrix, which implies that: ![Une image contenant objet, horloge Description générée automatiquement](https://lh4.googleusercontent.com/S6rle343JVEgjvoyKBTEHVirM1UR0Bhspgd9JBrTuVLKHFn2V5k7mHKBPx7jVRsDsYWUGwqP6thRd5xyhlBoNsjiI4pdc9vQrsSzT24AkI9OGeytJCTbHGjqOrLqDbhhKrzA0RdNeIXAREzXBdNwqA) When there are no loadings, the modes have no physical meaning. Different methods can then be used to normalize them to make their visualization more comprehensible. Thus, it is common in FE software to: - normalize the vibration modes according to the mass matrix, such that: ![Une image contenant texte Description générée automatiquement](https://lh5.googleusercontent.com/07jv1foge914iTRtmfr4GK2n2-DW7BEY6jpR2Yo7DvoiAoS9Yif1SfdLAEHu7xc2cwEtc0QA_2k0IPeOGjWWdEr8q66oBqCZauM27caYW7M-EthYYck-Ks8DJM4ZJ_UjM824RDkH7ysP-7GzE3L88A) - normalize the vibration modes according to a particular vibration mode. For the cases in which the software does not normalize this value, it can be denoted by the generalized mass term. It can then be written that for the mode i: ![](https://lh4.googleusercontent.com/zUp8nL5odnQiSBufH7wJblH_Kgsnl_DqEHgzPLhyRzc7rVpldPzW3FWXybsBcG3UEWQsii6xF77YJ3TsZ6bi5WxXPW0yYLrPX-spm18fsvjjWJs-VbLkybYaZRHfrmEnzabmg3sn1FVs6K7KVlOojQ) The objective of this document is to explain case studies for which FE methods were applied, so it is important to remember that the vibration modes are normalized according to the mass matrix, and thus the generalized mass is always equal to 1. The physical value called modal mass is also created, which will allow identifying the structure’s mass quantity that is dragged by a mode in a given direction Δ_{k}: ![Une image contenant texte Description générée automatiquement](https://lh3.googleusercontent.com/1whwVYE93mvwyG56PjIEIYCGurWI-_K0D6enAU24Y0uDhjL4G6bU8DOJTUDIsAuNPVWIyXVTPDxy0J5Sap-lkm3KtJ6QOr-DWXFi81H49pkktuUW8Ssa4XdexaHumF7cvqffKlM9h2v556jHDviXqg)**Please note: modal mass is a very different quantity from generalized mass, as the above equation shows.**
##### **Use of the modal basis** **Time-dependent response by projection onto the modal basis:** A particular solution to the global equation: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/m4YshSWDXwhghyEx-embedded-image-ke7prmx8.png) can be broken down on the bases of orthogonal modal shape vectors into N independent problems that are describing the response r_{i}(t) of a simple oscillator: In the case of earthquakes, the loading f(t) is an inertial loading applied to the entire structure: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/XE4pXZvbJmhSX8CB-embedded-image-46bllxmu.png) **Harmonic Analysis:** For this type of analysis, the goal is to construct a function describing the response of the structure according to the frequencies at different nodes of the model. This response can be a quantity of arbitrary interest (displacement, velocity, acceleration – absolute or relative -, efforts…) as a function of a variety of input harmonic loadings that can also be described in various ways similar to the output quantity of interest. In this case, the imposed loading on an arbitrary set of nodes are of the harmonic type: ![](https://lh4.googleusercontent.com/9z44vZnrznD6xUbBkDsxg_wLVvrKU6Irr_swEO7539OSsMaGnrUguAzS3jH4H6IhE3CCbGlyZ9B7G-Q7b6gnLkSvKz25rajIN_cyBt6gV744-aEqh8eOz1iBOaIJ_INyZpjTzSDfHn-XNmlDRLYFdg) The result of the analysis at all nodes of the structure is a complex transfer function whose norm (amplitude) and argument (phase) are the most generally used. They enable us to identify the resonant frequencies of a structure of equipment and to know the amplitude of its response according to different harmonic loadings. **Modal basis truncation – General case** Usually, because it is not possible to extract all the modes using calculations (too computationally costly, even numerically impossible in some cases), one must focus on those that are most likely to respond to the loading of the structure. If the representative loading frequency saved is f_{c} (Hz), one must extract the modes up to 2f_{c}. It is also important to make sure the modes inclined to contribute locally are well represented. A search for vibration modes must not be accompanied by interpreting the frequency, but by analyzing the modal shapes. # B2. Analysis based on a direct temporal integration #### **B2. Analysis based on a direct temporal integration** **Schemes of integration** **Main Principles:** The principle of the different direct integration methods is to divide the studied interval into n smaller intervals of length ∆t = T/n and to verify the equilibrium at the discrete times Ti = i ∆t = i T/n. The differences between the methods (centered differences, Wilson, Newmark…) rely on the hypothesis that is considered about the variation of the kinematic values on the interval ∆t. **Explicit scheme:** If the displacement value can be calculated directly from the value (or values) of the previous step, the method is said explicit. In this case, the equilibrium is considered at the beginning of the increment. **Implicit scheme:** The implicit methods must consider the equilibrium at the end of the interval, which requires the resolution of a linear system. As stated earlier, there exist many schemes of integration. The objective here is not to make an exhaustive description of all of them (see the specialized publications for that). Only two schemes will be presented in this guideline, the centered differences method: an explicit and conditionally stable method, and the Newmark method: unconditionally stable (for linear problems). A scheme is *unconditionally stable* if, for any initial condition and time step ∆t, the solution is bounded, particularly when ∆t/T is large. On the contrary, a scheme is conditionally stable if the obtained solution is bounded only if ∆t is smaller than a critical value ∆t_{crit}. Precision is a concept that is different from stability and it is extremely important for unconditionally stable schemes. Besides the inevitable rounding errors, the precision has an impact on two sources of approximations: an (artificial) increase of the period and a decrease of the amplitude. The influence of these two phenomena gains importance with the increase of ∆t, but independently. **Centered Differences Method:** It is a scheme resembling finite differences. It relies on the approximation of the acceleration (Taylor series of the second order): ![](https://lh5.googleusercontent.com/TJh8pIVR9wPsQmLK-S-wcYBLg9ruNse4ZVZq9nZAWIC1zEDW8r45ZDOs3wfkZsWovPQOtBgNPxDsUpZKdAgGbOdQtFD0K43V6PPRNniC25HOf9H_SgdDxjOf9t5aBUn-MMwoePtcmbp2eljvnXqxog) To obtain the same order of error for the velocity, one uses: ![](https://lh6.googleusercontent.com/Gdi4GseUWGeM3XtjPmsEhSWTg-S3qqH0GPIoIDysRktlsFsfrMyTcTdhR2cAJvjGTb-Xevmg9TTngSmVt2HiLJnsJ3yds_2iTWvC5Di9h-MVD10idl9lq1c_Un7LmeHnUgh7jVCcX5Yq6ISovusMzA) The displacements at t+∆t are obtained considering the equilibrium at t: ![](https://lh6.googleusercontent.com/5R6KCcdlOEIp0fQV4GHfTOMXdg39cKdlxu4xUJdnBgnhzRVz5wYwQvYCVX8n2X675AuHUNKwKF6zeB7BK7tPjpjagFSsuzaX_QOqWOaHs0-vzwbAp4bGooUfOMYrHMSNs1JH5CAXEp0B9IX6F8VYOQ) Thus, introducing the approximations of the acceleration and the velocity: ![](https://lh4.googleusercontent.com/VdBXTwxAQe2i6s32Z6W_IrB2vewp1EtdCNYpAUK8PG3-OBx8F8q-BvHU-ZWl8BaYOaABGQTYs44uQ4KWKBuNrCmFoqAK_AxCNFdDy8fpzHbT-BJ8QGM4GE5icoQLmd-Ow_rDEiiE6Je0WK1dEsoBoQ) Of the form: ![](https://lh3.googleusercontent.com/Zk24DcTzCNtQmsTx0jLdYL4q1vK0h9L_g1yMrkKmRN0Ro5zeVVsHFw4P5SJViQ7l-FrFs_sKIgb7jcse0nyUGx0BM95HKoQKWuz6sBj4hgu4a3YRb3Lbn9tkt02c3zjH0JIk3wQtue8ydCVVuCZsZg) This method requires a starting procedure to calculate q(-∆t) (from the equilibrium at t=0). The damping introduced by the scheme is equal to zero (no decrease in amplitude). **Newmark method:** The scheme is based on the following approximations of the velocity and the displacement at the end of the intervals: ![](https://lh4.googleusercontent.com/32ZgSuhXTb14RWLmPPTbo3bWnnrp1Tt1wDejXNZtcQCI1O-5eiMcYROWH3IOnD7s-KJl3Up1JkbhDDPUFyEtPjE9Uwe-IZ8Nh90xbZgrcfxCKps-aCnmIDfZlXkxEvyWjDRJV6BZ50jXWGzwaBmuiQ) From the values of both parameters α and δ (ranging between 0 and 1) depends on the precision and the stability of the method: the values (δ = 1/2 and α = 1/4) lead to an unconditionally stable scheme named the Newmark method: it corresponds to considering the mean constant acceleration. Considering the equilibrium at the end of the studied interval (at t+Δt), one obtains: ![](https://lh5.googleusercontent.com/huCbHPlEAt1JpsuxErgoO9jbpJfrPqK26rlu9HZj7f6l-1feVs3PZJcDHb7FWWDh5xjtCbZIp1AHOZcMT0D4q8favEROtCckNl13hvfsxuFAflsnVTz0Uszl2rkDxk9xHO0kR2aqK4DzJma481gEBA) with ![](https://lh4.googleusercontent.com/h_ptzdOTeqhN_n8_x40VMdCgsREkbdtiZYYcfJFrIbB2DX9mRPKIgyLBSao_FD1vh0YzkBdM9KO0zvnG5SJpf4pbo-mFm0P5O3j21I2ys2W6mpXDDLbZQq5gqFsbt-I7JnaWJyngE1YT5u1z0Qr0SQ) and ![](https://lh6.googleusercontent.com/qrhecItnqT9hpAc50uy9NcRL6p1jqcFYbn1w_h2f9SBP-NrcfEYa1-MhPGCa_vp9Dn1USmNjVMdOE2CVCTFYiQDO_i6NCK84pZt1b5LCSabu9oq3cM_tja26q-dSRbDKA7fGN0HLCvpGl2ylPmlLkw) the coefficients being defined as follows: ![](https://lh4.googleusercontent.com/OoJ_MIy-YknCRnHbNM7xO3_jql43j8JXswvAdpcL3daif4MjIfkeLSJQVDAysgKTKk6KGQM_hKWTrqehbuPOXLp6-RVRxNDdx1r2FH9TKD46l9R9_AqqAQISTEYPNIMLo9pq9DEd9JULLPghU-DaEQ) The scheme also requires a starting procedure: the value of q¨(0) is obtained considering the equilibrium at t=0. Alike the centered differences method, the Newmark scheme with basis (δ = 1/2 and α = 1/4) does not introduce numerical damping. The values (α = 0, δ = ½) enable to get back to the centered differences method. **Choice of the spatial and temporal discretization** **Criteria about the element's sizes that satisfy the wavelengths** Different criteria can intervene. They are related to the precision of the expected results and the type of calculations used. For the transitory analysis, the general recommendation is to have a range of 8 to 10 elements per wavelength. The stationary waves being composed of a sum of propagation waves, the stationary dynamics analysis (in the case of earthquakes typically) will be using the same type of criteria. As a reminder, the general equation relating wavelength λ, frequency f, wave celerity c, and natural frequency ω is: ![](https://lh5.googleusercontent.com/4BnP2Hmq3qRgBh-axDU3HS_bHF6W4quMky5MoHhaOiGvaBNAEhwKYxejNTl-yEGel-FN5fZPcHATdf1Lb4xBSI37YaCQBplKJiBf-nDDj6rqTLA2BFhBibmafpSB5bt34PwlzptMGfuhlMirdFlNrg) According to the type of elements used and the type of waves of interest, the following formulations are to be remembered: Volumetric elements in an isotropic environment (typical case of the modeling of an elastic soil od with Young’s modulus E, Poisson’s ratio , and density ρ): ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/8Cw96quNiW320cPM-embedded-image-ohqvsryg.png) Shell isotropic elements: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/MRInmyh8evfcOKg4-embedded-image-t0os4c61.png) These formulations can be written in a more general form for anisotropic media with 2 principal directions 1 and 2: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/I0Yw2hLUqrzcEYQz-embedded-image-qrk6qqqs.png) One can find the size required to target a cutoff frequency of 40Hz for shells, plates, and volumetric elements. The size required is given by the numbers below / λ for 10 elements.**Types of modeling** | **Target Frequency \[Hz\]** | **Thickness \[m\]** | **Type of wave** | **Size coeff. of the element** |
Shells and blocks – GC Concrete | 40 | 0.2 | Flexural | 0.59 |
40 | 0.25 | Flexion | 0.66 | |
40 | 0.5 | Flexion | 0.93 | |
40 | 1 | Flexion | 1.32 | |
40 | 1.5 | Flexion | 1.61 | |
40 | - | Shear | 6.04 | |
40 | - | Compression | 6.75 | |
Shells and blocks – Meca Steel | 40 | 0.01 | Flexion | 0.16 |
40 | 0.02 | Flexion | 0.22 | |
40 | 0.1 | Flexion | 0.50 | |
40 | - | Shear | 8.02 | |
40 | - | Compression | 9.58 |
Note: for rapid dynamic calculations (milliseconds), the damping component is often neglected because its order of magnitude is much smaller than the one of inertial local stiffness terms during the period of analysis
For the more “classic” cases, the damping matrix is generally constructed from the critical damping ratios defined for materials and a linear combination of the M and K matrices that were previously calculated by the FE computational model. This process enables us to considerably simplify the stages of calculation. This approach is related to the “Basile” hypothesis for modal analysis. This hypothesis was formulated to identify the structural damping (mainly in aeronautics), and is explained as follows: “Even when modal damping coupling is present, the modal equations of motion are dynamically decoupled, for structures with a low damping ratio, if the separation of the modes in frequencies is satisfied”.Be careful! Considering the Basile hypothesis leads to an underestimation of the dynamic response elsewhere than at the edge of the materials or at the supports, which are subjected to a high damping ratio compared to a time-dependent calculation by means of direct integration, or using more complex methods such as the complex modes method. This justifies the need for direct integration calculations of the motion equations, or complex modes.
Most of the time, the Basile hypothesis is considered and the matrix is constructed starting from the Rayleigh method: ![](https://lh5.googleusercontent.com/j9bn5e4sVZ0XMI2cDoUdRBU7Eb0Yp5SSMvC7MLaP3ibZZ5IJgb5yi4_JIXodb3QcyWWZzx1gjgQsebC7LjRK87HoyNdelJxXE5BXN-cG7Pq1w5n1D5U1DjszJlzT4iQsZoDRtwGvXbneFMWGPQJu1g) The terms α and β must be introduced. To be pragmatic, the following steps must be considered: ![Une image contenant texte Description générée automatiquement](https://lh4.googleusercontent.com/WnnUlrSGbyfPDFqubVw1TsOOWXVXpwP36wwvdHy0KD-L-fjkDGKuRhW4N4eLX8WLoaShlAcMvd4AQTXeFhErVszfwlk9Jxxh5EzxxVYpGMu6A2pQfmLpseVSnp7MmC5iY_mLWkHNSlHFV9Q2IGp5SA) ![Une image contenant texte Description générée automatiquement](https://lh3.googleusercontent.com/u4C0jQUtmQQoXORoVcgVddUJjyVBw54XZPfqyp3IiH_cbIHoEY_o0y64MqO9KltQOGS8wbzheRgvNpaQmB6vmLPCgZ2RQ0E55vVHYqH8aDhTrf_IGRXaoZ-AmZPPtIsJLXecYNHx7PKDe5tScQkdYg) f_{1} is a lower bound of the first significant vibration mode of the structure, f_{n}, and the first mode encountered after the cut-off of the elastic response spectrum characterizing the applied temporal signal. The value of the reduced damping is calculated for all values of ω, applying the following formula: ![](https://lh4.googleusercontent.com/WO0zlHZggrrdqd6Aw0XtMXhstvw3EV-Hbu-mvMdarut2IxayRReKRdenUf6zliMq4zaf5_Oy9ghuNHCiM457Y9HV3u9nZ-5PqqkzyzWZIFj8cBtdnJ4VtSC3yGFlxsQ_EHGiC8p_ziGpnsDtXwTN_w)Be careful! Since the damping is largely overestimated after the 2 frequencies of interest, it is necessary to master these two values. If fn is chosen adequately, the overestimation of the damping has no consequences because rigid body motions are found on these ranges of frequencies, which will be excited in the response, and the modes with frequencies greater than the critical frequency are insensitive to damping. However, one must be certain that there are no local vibration modes with frequencies worth considering. The impact of an error in the choice of the first frequency can have the worst consequences if a significant mode was forgotten because its response will then be neglected. It is important to note that in between the two frequencies, the damping is underestimated. The evaluation of the response of the structure is therefore conservative.
# B4. Specificities of the seismic analysis #### **B4. Specificities of the seismic analysis** **Spectral response – Specific case of earthquakes** The principle of the method is, for a given seismic direction, to construct the maximum responses from the loading spectrum at all points, mode by mode, then, to accumulate all of them using various methods. When the seismic response is obtained for a given direction, the seismic directions are combined to get the global response. Let us be in a case where the modal vectors are normalized according to the mass matrix, which is the case for most of the FE computational models. One can write the expression for a degree of freedom in a canonical form: ![](https://lh3.googleusercontent.com/ySpvy_CPTUfA2qFlJiFuhYZViaqFtvT8KU8BZuw8vsiG6U24xQKNGZi-vKXg9mHr7LS2t_kT_K2gqODASDApEyJFvV4EJdcPNLSqtcLN-rC1v0NgC7I__RAJXO6vD9B4GCzhQn66QgsgPY8vTjpYwA) The term p_{ik} is called the weighting coefficient. It is an important concept in the case of seismic analysis because it restores the physical contribution of excitation in a given direction k. It is determined for the cases in which the modal shape vectors are normalized according to the mass matrix: ![](https://lh4.googleusercontent.com/W_v_7tyKN9T6Z_vs7ZPCSvEbZJfvraR__eDhFzfrF6c7tbptOuPqm3AvgaTpbruF0KYai5J59AAdKr5utphJj9lz7ddeupNda1Cy5br7TbOlyJo5nGDPRwwJ7QrslPUWSn3DmQ6ybNFeRuAJEizLqw) Moreover, for a seismic motion q¨_{s}(t) in a given direction Delta_{k}, the mean solutions greater than the maximum values of r¨_{ik}(t), r°_{ik}(t), and r_{ik}(t) in terms of pseudo-accelerations, pseudo-velocities, and displacements via the respective spectra of this motion, are known: ![](https://lh6.googleusercontent.com/kI7mgA2AoctFpvBscgkXCeQHaefcDRWCJMftAX7q5QCH19Q-O9FkQo4mkURtvMTl4Dp0RAi4WfoDMAVYSTGX_4KnZ3jjQLnTWoThztN7CXaByAG0pp1CTVgg7dZ7OSU1_tnyZJSHAZtcFkcqMyPGdQ) This response is constructed for a modal damping ξ_{i} that can be evaluated as a proportion of the modal strain energy (see §1.2.1 of Génie parasismique Tome 3, J. Betbeder-Matibet). ![](https://lh6.googleusercontent.com/GXht8h8HUwH1Vf52Ye-3DxojMMsgR-1lHJ8ipt9xkJLl2ihEJaUVvSfmJzkjyMEnB9mJOPzvjiZ_Ap730RMIvUMWsexJtkthsB6Hb10HAis8DQTtcpjG6qYonUIN-SYRr1HSL7vjWRWCbdKe08466A) with: - E_{iT} is the total strain energy of the structure for mode i such that: E_{iT}=1/2 φ_{i}^{T}K φ_{i} - E_{i material j} is the internal strain energy of the structure with the damping of the material being ξ_{j}. Then, from the simple oscillator response, one can construct the response in the structure for each mode, for the acceleration, the velocity, and the displacement respectively: ![](https://lh6.googleusercontent.com/pCExLBB9O82GAICNFIJtumeERY9_62drsfuaTY_LIpI2EWJXgJXVhiieMoWBNgd3172LmAwyYTEyQch9KjlBB26NG4OxxhXivzJIML4J-qKJTMTePLG--TZLDDQCFPoMpi8MhV7qfnSlkC2-8nEW8g) These modal values must then be combined for a given loading direction to obtain the global response of the structure. There exist several cumulation methods (from now on, a_{k,p}, for the sake of example, denotes the component p of the a_{i,k} vector, such as φ_{i,p} with φ_{i}) as shown below: - The “Square Root of the Sum of the Square” (SRSS) – At all nodes p: ![](https://lh5.googleusercontent.com/t05Yj-w-y-ZnXidU1qvBorv21k20NLG4h1uVGwaisesb1zD7TCUU5xRt7VNNh0noXPCqWv1B3uFtiCHhGc_Xjtk-91RjgzKbB-jE9r3qhsKG01Y_e31awVHHQ7GXB76d3Okh23tgU4por-QxYDIxjA) - The Total Quadratic Cumulation (TQC) – At all nodes p: ![](https://lh6.googleusercontent.com/hyUTliwZW4fqC4RRQ4q8afvfwlniQJcEAwf8ZomVJPfp9SeNu76xQJQJp3ukYOZCGN-UnzqFYzwyFkUgNXNL3f9CQKbpOXL3zu9p0WZnbwa0VG1KlOKeYMmHXnl170Zi1z53XeCtHrzFyPu0ucRq4g) with P_{ij} denoting the quadratic coupling coefficient of the modes i and j, such that: ![](https://lh3.googleusercontent.com/H83s-sw6CssXZO91KzBeMW40mpDquMVM4sSj09NvTGn7CpCxlUFUzlFapaGfDAdObXreVTjLcRspL1AvNR3_RYqo6ny-kw4N0NeRjDek7Owb9mSf3xFImIp6QEjdcLzLaYh6fA2iqG0H8ksduHbb5A) It is important to note that, in this case, it concerns a cumulation of algebraic terms, but the signs are all positive, placing it under the square root don’t cause any problem. Let us consider the modal damping values ξ_{i} and ξ_{j} equal to a variable such that x = {0.2, 4, 7, 20 et and 30%}, one can graph, for the natural frequency ratios ω_{i}/ω_{j}, the curve (figure 3) that highlights the cumulation of the neighboring modes. The cumulation coefficient decreases rapidly when the frequency ratio increases, and even more when the damping ratio is low. ![](https://lh3.googleusercontent.com/s6Vk7pjbfuzFmuRukyr3db3RXRI1Z2YaDORCMbp1Ek_1VCnwXMw3q-Rp2EKsaBSOKbLiinpxGxsHRJf2WC1tbwPuBIg2LNelzZYdjO0dDXSu_2Xhl8q0rqZLimfl7SnLV27lMlSyQh26cFAZuJiKCw) Graphic of the coupling coefficient for different damping ratios varying as a function of the natural frequency ratios. This last observation shows that the TQC method is more appropriate than the SRSS because the latter does not consider the cumulation of modes close to one another. On the contrary, there are no advantages of using the TQC method as a comparison to the SRSS method when the nodes are far from one another.Be careful! The cumulated modal responses must not be used to calculate other quantities of interest. For instance, the efforts deduced from the total quadratic cumulation method cannot be calculated using: ![](https://lh3.googleusercontent.com/OATPF3dtU83KdHRRd0eY2sLOg2zLTZNh6q0_CoV6Y5EmYdhM2slW5P_fKKYR3gT2qBNePw3bgtUsKcwtNSefRv_UUcH2EUQPE15CB-uY7weza7Z55SQUxWNhELT5yaC3Hsd0YHUPekMOvg_LS7JFZg): this calculation is incorrect in comparison to the evaluation by the cumulation of the modal efforts. One must, therefore, for this special case, calculate as follows: 1. ![](https://lh4.googleusercontent.com/crvdWqD3tpIuBdQ55lT8Px37yBEwkdkw_kbzYy80JREBdjUVIXxjgfx3jYFhGmUSYPsNXOnjO-QxLtyxyPi4K-jgtbX8CjxumEzaXIjx2L8JQD6btFhSkHnoSRiORc0Dj2IJj-ogF9qLaNYumAZm7Q) 2. For each term p of the fk vector, it can be stated that: ![](https://lh4.googleusercontent.com/9GbXRz5pFFFWtymLy-A-kNzAFLSMJN5drHrYjfEwy7boRIyf8mEWDxDRMZ5pU4jV4k2y6vYUxt2kknsgVM3Bb79kiNMQt7g61koZtTn8qA2UNAzYEZAdXYMznF297-5iIL4GjdstoK4cGlEEMiur1Q) It is also important to keep in mind that criteria allowing to evaluate the state of cracks based on the invariants of the stress tensor, and thus, of the principal stresses, (cf. for instance the criterion proposed in the annex LL of the EN1992-2) cannot be considered after using a quadratic cumulation of any kind.
The spectral responses of each mode, after being cumulated for one seismic direction, must be combined to obtain the global response. In this case, it is called spatial cumulation. The spatial cumulations can be handled using different methods: - By square root of the sum of the squares of the responses obtained in each direction. This method gets rid of the sign and all logical relations between solicitations. It provides only one scalar quantity for each quantity of interest: ![](https://lh4.googleusercontent.com/x8bencX3d5NvY48_qiB3wx0xsuJ2n9yV28N5IV1PU4F8TUfYtIEEkiUyD3e0YLOBPnOAwNZGEQbLDIEmmxJA9kLTKIAS5f_xS7TUh3TCa--gQDsZ2JV5mTf5Jx9uALrEV2-XoMwyOWnEczZ_l9sO2w) - By algebraic cumulation of “Newmark” type. This approach relies on the hypothesis of independence of all the spatial responses. It introduces a weighting coefficient μ, with values ranging according to the different standards, which considers the two other unfavorable responses compared to the preferred direction. It takes into account the sign variability of all the quantities of interest. Thus, it leads to not one accumulated response, but a total of 24 as demonstrated in the following equations: ![](https://lh6.googleusercontent.com/aQMOfljli4SBi04Kzz5a_r2R7iFj0fPPGE4bPKbK6wyJyGwXY4u1Wtm7LdseaHxOtt8RSD7wygbGTqTaxr6rCTGVm0PdWWZCIuZ0Uz9qjhTN_n9fXfAaJkJ_MB1JWUCwkgbq24GR9hGSBnA5hIvc-g) **Truncation of modal bases – Seismic case** For the specific case of earthquakes, and normalizing the modes according to the mass matrix: ![](https://lh3.googleusercontent.com/7jQtttZ2NrVRy7PGQvGXFgl6ExzK4elaaZwbLzu3sS_bmeDGHb9UoN3gypkdqh01dIOrvwrOoGaKN3BQElmPaN_3IMgbeGR2UYcQGhluWeMw-DWHmwGs8wCF9n1BpjBtBvY8rS1-Bt8Zdyj4ttG82g) It corresponds to the mass driven by the mode i in the direction k. This mass is therefore related to a specific direction. For a mode i, there will be 3 modal masses as a function of the different loading directions (if we are in a 3D space, 2 if we are in 2D, and only one for a 1D problem). Figure 4 highlights a 2D example for a frame.The modal displacements multiplied by the weighting coefficient represent the deformation of the structure whose product at all points with the response of a simple oscillator gives the time-dependent response of a given model. This concept is detailed in the following chapter.
![](https://lh4.googleusercontent.com/0f54RdoOYXn16BjCUov732DeWDpqqp0-R-JSIDjKRqLWHyUxrb7PNnykSzXMfl57WWJtBglbi2bDHWDAHv5dB3ViiaeMLTyYPXHG-dAA2consgl64_HS6HThZFAddUWp_9hPei43AIBwRWKhk0AN8Q) ***Mode 1 and displacement in the ey direction* *Mode 1 and displacement in the ex direction*** *Illustration of the mass displacements for the same nodes in 2 different directions* As explained earlier if the model contains N degrees of freedom, there will be at most N natural modes of vibration. However, since the search for natural frequencies and vibration modes is conducted numerically, not all the modes are extracted. In theory, one must have: ![](https://lh3.googleusercontent.com/-ZimdyK1f9lTZ_Fayk2vWprz0fIbvLW489rwEvkSQhey-eJjzTdOxetBJNr9bqdDBCWXDcoNyoHGVgnQ7Y19eLlBiQgXlLFOnCIpKUSI5Xc3oqYC1UR8wTMUPHmth1pct9_B4g4pTR90cOvnzSHlWA) In practice, the algorithm will stop running after a threshold value of the frequency fixed by the user is reached. Then, the user must verify that there are enough modes to restore the percentage of mass required by the engineering rules followed. Usually, the criterion is to restore 90% of the mass.Be careful! If at the threshold frequency, the percentage of mass targeted is not reached, it might be necessary to include a pseudo-mode. Conversely, if a significant percentage of mass is reached at a low frequency, way below the threshold frequency, it is necessary to incorporate a pseudo-mode or to complete the modal base. Indeed, the participating mass of a floor for a local flexural mode inside a sizable structure represents a very small percentage of the total mass. One should also be careful concerning the antisymmetric modes with a modal mass that can be equal to zero because the masses displaced around one axis of the structure will balance one another.
**Pseudo-mode or static correction** As formulated before, the selection criterion of the natural modes concerning the cumulation of the mass is equal to 90% for a frequency of the same order of magnitude as the seismic response’s threshold frequency i.e. 40Hz maximum. Whenever this value cannot be reached, the lowest percentage withheld will be completed with an additional mass associated with a “pseudo-mode” of vibration. Let us remember that for a seismic direction k, there is an accumulated response on n modes such that: ![](https://lh4.googleusercontent.com/5mMrDbbZEL3O-1cm6EqJqdGVIUJLgZzi2UEZlEuzuWaP9oSQCIs3sz2NxDiAoa0K1ygMji_UboKBfJdDJtumfcaDo5iVpVF5LE9OeRgHj9upsRkNMTM-vgbYvve6dn3hYqEXYzjojDLgTHg38UWI7g) To be rigorous, if there are N degrees of freedom, the formulation becomes: ![](https://lh6.googleusercontent.com/Tnve8swlixFANftBlwfkrdyzqiLHjh7I6mE79PfS7-OaEauVYS934GWAxjoNadYc4_9PKPiDwU7Jn0jRPuXuf2YkYzHuaMCrrdOTvm0C-4uy3A12XklosE2x8HhfP2aOozncs6WcPjr3iknbO8qQFA) As seen previously, the modes after the threshold frequency are rigid body motion modes. The structure reacts in phase with the seismic loading that it is subjected to with a relative displacement equal to zero. To complete the modal base, one can construct the pseudo-modes considering that the total response is the sum of the “dynamic” response, taking into account the modal base of the n first modes withheld, and the term proportional to the seismic acceleration of the support q̈s(t). Let us remember the following equation: ![](https://lh4.googleusercontent.com/X_pr91s-Gm18NR1mMn8YK69heWDN2CPqdeASvXHG10iI9i8oJ-NSIwS4YtOSsQRMspYxTl4o_Dfp8HqJs_B10S3AE0b0Hj_dbbiaogMNqJm7a6NJXHToSzva2dvHKfLlPGTubmC2120xct9EC1OReg) with P_{k} the displacement of the structure in the direction k subjected to the static loading equivalent to the mass of the accelerated structure at the acceleration of the last mode n extracted from the natural frequency: ![](https://lh3.googleusercontent.com/IEG_ND1vJ55CvmNnT1s5iynpYvaNgNDHIHuAy5Q6o4qQU615YMJ8c0ARv24msSyf0Oq9ioIvkfL4Tm4aslKmIv-N7P_OfZGF5iIltRnT0cFd_txLVd-3BbXaNaXf9PeF7roq0j_gjBO1B3cjLMj60g) Since the relative acceleration response for the structure is equal to zero after the threshold frequency, one can simply write: ![](https://lh4.googleusercontent.com/4W0OtvHLsK7KW9gk8Bh32gQOEuZuQ1zuXbDtkcszZ8hhbFJNn2Ad_OvX684_OQ_b9bGxvdCqiBjVfWAQQWZ5Dj72l791f1AoVOfFDsnXxun6gZqimDuyg6cxLvv5EMxxqRkIDTn3S2407IArgnPwXQ) Reformulating the previous equation as a function of ![](https://lh6.googleusercontent.com/InE32mSmvte-ddTu1-FG-dPQ6Y8Ip7cyE-2LVXiuBe7YnXHlVF6OXPcyYCjevXRYGIYGa99J1Vkcd2m3h_1NHEn58YvnH60Nm3hf4-sIVWoz5S7tgWRGlm_e97HoRGaDjzzBKpYKKzFyjdGA4xkT0Q), it will be easier to link the pseudo-accelerations spectrum, considering the frame of spectrum analysis: ![](https://lh4.googleusercontent.com/_hLBwOtKgyCiXzwUOnsIZQUPF4DXx6oUWXrhAqz9wEhsOi7pkW4NzYgRddBrbPmOjjWMbSmpAED0I5ks6jpG3-rmvXMf3_YuROzNRrE9epO7UJTpwYW6-S8mwsKFD0WA1PMyp8aV3JchVcLkCgaNTg) Thus, the following formulation can also be considered: ![](https://lh4.googleusercontent.com/fnxQKPnQMZSzg_SBbdkjKzkN0kWZx8uBwz5N_VmFNFtfyBd4ioeIlPptAWP-7e8xR-UEggiQLdPnblu0fPmFmgbWLDJOViA_MgJmRCCxAEm-r325S75aPUueZdfQIxYTgtvIyW24S6ekbWwBEvOx_g) After evaluating these vectors, they must be cumulated. Indeed, the temporal solution for a seismic direction is given using the summation of the components on the modal base: ![](https://lh3.googleusercontent.com/l8TXWogV0O1eb33bGxh3Td-Qe7FMwei9L4AlqjEr4wIJxSJbzGo9zErAoxEpN_Ayhrfs1225vUy57Fk65PB5a0Z0pzhxK_oILjofCpK_ufP3LAV98sWwYlr_5KBST1oyXlOQ2iZjgCpK0YmQCkGanQ) However, this combination cannot be applied to the maximum values that were just calculated previously. # Chapter C. Static non-linear calculations #### **Chapter C. Nonlinear Static calculations** Nonlinear calculations are generally time-demanding: a finite element software solves a nonlinear problem as a series of linear problems (incremental process). To prepare this type of calculation the user has to make decisions such as defining the increments, choosing the algorithm, etc. Therefore, the process requires a certain amount of experience from the user. Most of the nonlinear computational models can, in principle, run until one or multiple conditions are satisfied, or in the case of contact problems, until a specified minimum number of connections (or supports) disappear. Therefore, before starting a nonlinear calculation, it is important to make a preliminary estimation, which will enable us to know when to stop the calculations. **C.1 Nonlinear mechanical problems** [C.1 Nonlinear mechanical problems](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c1-mechanical-non-linear-problems "C1. Mechanical non-linear problems") **C.2 Why performing nonlinear calculations?** [C.2 Why performing nonlinear calculations?](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c2-why-performing-non-linear-calculations "C2. Why performing non-linear calculations") **C.3 Implementation** [C.3 Implementation](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c3-implementation "C3. Implementation") **C.4 Convergence problems? Symptoms and solutions** [C.4 Convergence problems? Symptoms and solutions](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c4-convergence-issues-symptoms-and-solutions "C4. Convergence issues? Symptoms and solutions") # C1. Mechanical non-linear problems #### **C1. Mechanical non-linear problems** 1. **Description of possible non-linearities** The non-linearity of a mechanical problem comes from the fact that the coefficients of the equilibrium equation depend on the displacements of the solid itself in equilibrium. In other words, the equilibrium equation is generally implicit. There are several non-linearity categories for mechanical static problems: - **Material non-linearities**: in cases where the constitutive law is not linear or that the response of the material depends on the loading history. In other words, stress is not a linear function of strains. The most common case in civil engineering is one of the material loaded beyond their elastic capacity, which then develops elasto-plastic behaviors. This behavior is characterized by a dependency between the stiffness of the material and its stress state. - **Geometric nonlinearities**: for cases where the structure is submitted to big displacements or big strains. In the first case, one can no longer write the problem neglecting the changes in the geometry of the structure. In the second case, one can no longer approach the strains simply as the gradient of the displacements. - **Boundary condition non-linearities**: in cases where a structure is progressively loaded and there is potential contact between two bodies with follower forces. These types of non-linearities also appear when the construction phasing or the assembly of a bridge’s deck are simulated, when digging a gallery, constructing an embankment, etc. All the above non-linearities can be coupled if the algorithm allows it, but the resolution of the problem becomes more complex. 2. **Principle of resolution of a non-linear problem: Newton method** When solving a finite element problem, one looks for the displacement field u, such that the inner forces L_{int} are equal to the external forces L_{ext}: ![](https://lh5.googleusercontent.com/scOqYTytSlhGTvwP8rCqlc8c12L8lDN4zv-zfapzL7S1RAqOHnRnuN97DQCt4N6sPn3WE1OX6n7m0P5939IIhDGejAq9bYUtTmHkW1fxCLTcKK9IiFM_ppTIzt_FDbK_Gqy0jR8sr_FXprIlTXHbdg) , which is a non-linear problem as a function of u. Generally, to solve the non-linear static problem, an incremental algorithm is used. For that matter, the problem is parameterized in terms of t (with t representing a pseudo-time, unlike the t parameter used in dynamics). This parameter is used to index the successive load-steps applied on the structure. More precisely, it consists of searching for the equilibrium state corresponding to the successive load-steps F_{1}, F_{2}, … This separation leads to solving a series of quasi-linear problems as shown in the figure below and to determine the state of the structure at the time-step t (displacements, strains, stresses) knowing the solution at the state t-1. The greater the number of load-steps, the better the precision. ![](https://lh4.googleusercontent.com/aCwhkJYQjkY8pgl51o172phYFFthTrXq17PESWqB86j_ZvSU2KkFoJ4b7YrU38xSX7Gykfm8RhivTu1MkVLha_9U4VkZrKrNy_07TTsEEEGsJGTzg_U5BOywF4OpeKXyZemTaHH3hJm6PK0CQAEAJA) *time* *increment*. ![](https://lh4.googleusercontent.com/L7VWeIQtx-1vAuun2My3Tv5GyZKKT8z983zhkbi8ghn9s8baoCodFT5t-DLEPtEeRZJRgwtqUJLRLh4IAreUFr4tm-u0A0-6LkF6quhT869ydMyXZM5oIOg9HRdGYJc0Soso6WBUOUf8EpcEtp9SQw) *Principle of parametrisation in function of t* At each increment t_{i} the discrete problem is K_{i} x q_{i} = F_{i} where q_{i} is the unknown displacement vector under the applied imposed loading F_{i}. While in the linear case seen in chapter 1 the K matrix was explicit, when the problem is non-linear, K_{i} is a matrix with its terms depending implicitly on the value of q_{i}. So, q_{i} cannot be determined directly by computing the inverse of the matrix K. The most used method to solve this non-linear equation is to use a Newton-type algorithm. The idea is to build a good approximation for the equation’s solution ![](https://lh5.googleusercontent.com/lF4wnpwOFH7J2t1JGLuZtJGYoM7y4BnuYw8QvrywECtbW2-EcXqSv5eWdkVEk7Z95FmxXAI2FKBlKu1N8KbDS0gK7i91oTxoUb8f_F9Wc3s6Ssez3Df0jqhHv19u2RpQg27NOshCqKcBdtIAdAvnGw) considering its first-order Taylor expansion ![](https://lh3.googleusercontent.com/OysEV6yjIIMizt-C-UvAL_1vMqIR0B-UnhZ75p50yqDu6DmX5jVCxBFgreGUAIDQfVE2obt4fQTkD5D5191xY8f52ywA3rBtrB5Af6Hb13qYCLmPn1hgcYVYnyP2mX9uHqz9rmD00BSkp6H0Q8aXBA) One must start from an initial point (close enough to the solution) and then compute by iterations ![](https://lh5.googleusercontent.com/brdsJo6bVieDmBg2Ggzhundc5OYEkqLuQ-_kVtdn9AalDXIXJTIUWuYQkkbkHK7r08VudFFzEm2icIyAdwzx5jMrhvwwG6UpIIR6q5pu8xr_q7iDiaCzq3vfjR_fSW-_MU0cz4hWajlwBth6lRMvsw) At each iteration, one should evaluate the residual vector F(qk) until it exceeds (in absolute value) the value arbitrarily close to zero. This convergence criterion must be chosen with care, respecting the standard used by the calculation code (see section 3.3 for more details). **Note**: With the Newton method, at each iteration, one should compute the tangent matrix at the considered point:**![](https://lh6.googleusercontent.com/9JiAZ4aDnBVXhprmjueY5D7CqenQNmK9e62UgAjwpnUtw4XG-aGt-0wOHK0L_-0XwvZfRwSe_oXKL6lMBUVihFEEiXKC-eRNoV4zCHiCwgQemloEaMkgFpsWXmzzych0g9yLErtJaGewzcHIrMNOjQ)** The computational cost of this matrix can be time-consuming. If using this matrix allows having a quadratic convergence (so, in fewer iterations), it is not essential to use this matrix. Other strategies can be adopted to estimate this matrix, namely the quasi-Newton methods. It is conceivable to use the tangent matrix without updating it at each iteration, but also to use the elastic matrix (figure b) or the secant matrix in the case of a damage model. An illustration of the successive iterations according to the used matrix is shown below. **![](https://lh6.googleusercontent.com/8-RzuhuCms3fpqjK1EWUv8uCexmpn-Ue4tCfZZ9hO35du4pedFB2cOkFIkrfTpCrgIFJrIurtT0VLA1U0R5pQmR9laDP9GMiPRuS6GWKjSvrioaQfsHPMtDYGTCqgiZRbjyIETjTK-Emg_vG-_PIXw)** *Illustration of the Newton or quasi-Newton method (elastic matrix)* In general, using the tangent matrix allows a faster convergence (in fewer iterations) but the alternatives might be more effective or more robust according to the situation. As the method is iterative, the process should be stopped when the stop criterion is reached, in other words, when it is verified that a given value (or several values) becomes negligible. The global algorithm can be written as follows: **![](https://lh3.googleusercontent.com/_iX96ptsFXVFJ-gqzVqUmB9U59eZCPN_Lyc3jQB6ikUJTaQQJn1gxL8ySPcMipTxk8H-CxeCzzQmAmgodMvFUDzX8i9tHxjurWYTapwHSdf_7oULu2xrJstBDA-GeYhsEfLdkV9ATbCiPrdBaSnUoQ)** by defining the increments, i indexing the Newton iterations and ε being a positive value close to zero. **Note**: The Newton algorithm is used to solve the equilibrium at each time step. It can also be used to find the stresses in each Gauss point (at all iterations of the Newton problem on the global scale) when the constitutive law requires it. # C2. Why performing non-linear calculations #### **C2. Why performing non-linear calculations** As in many areas of physics, it is only reasonable to undertake a non-linear calculation after having a good idea of the "end of the story". In other words, how the structure will evolve until it becomes unstable. Below are presented the good and more questionable reasons for undergoing non-linear calculations. 1. **Good reasons** - To study the **effort redistribution**. When some parts of a structure enter the plastic phase, the stress level “freezes” to a determined value. The work of external forces can only be dissipated by increasing the stress level somewhere else or by making matter flow from other zones that are already in the plastic phase. The goal here is to verify in which order the structural elements “fail”, and to find the final failure mechanism. - To determine **the evolution of support conditions of a structure**, either by a contact computation or by developing internal plastic joints. - Before reaching a state where the efforts are redistributed, **to obtain an equilibrium state** where, in the plastic zones, the stresses are on average close to the yield stress of the material and the stresses are in the elastic domain elsewhere. For **geomaterials**, to obtain an equilibrium state where the stresses are purely compressive, except for some punctual zones (**eliminate tensile stresses**). These procedures are reasonable, because: - Generally, they can be conducted in a small deformation framework, - They allow simplifying the model and the interpretation of the structure’s mechanics: since the plastic zones have no structural purpose anymore, a weakening analysis of the structure via a succession of elastic calculations can be proposed, which will “deactivate” the plastic zones at some stress levels. The analysis of the plastic zones can also suggest a static approach to the plasticization (strut and tie model). 2. **Questionable reasons** - To determine the shape of the structure in response to large deformations (even while “exploding”), eventually using an automatic re-meshing algorithm provided by the software, - To see if it is worth performing calculations with a behavior that seems very complete from a descriptive point of view, or if elastic calculations performed previously give better results. Those motivations often end up leading to non-convergence or “zero-pivot” problems. When the calculation is interrupted at a given stage of the iterative process, the deformation of the structure (given by the deformation of the mesh, or the strain field) is misleading: - The deformations are in general superior to 1%, so at this stage, the mechanical problem is no longer expressed with correct variables, - The calculated deformation depends critically on the meshing. It means that for two different meshes initially close, one can obtain very different local deformation values, - The calculation “follows”, by definition, one instability at a time; however, the large displacement problems are by its nature multi-branched. In other words, in a certain state, there are several possible equilibrium configurations for a given loading… # C3. Implementation #### **C3. Implementation** The correct method consists of always proceeding step by step so that non-linearities are not introduced all at once: - Performing an initial calculation with an elastic constitutive law before using non-linear ones, - Performing a calculation without contact before performing one with it, a calculation with no friction before including it, … **Every step should be verified properly, and it is necessary to make sure that the solution converges when the mesh and the time-step are refined.** Finally, it should be clear that in non-linear cases, the problem to be solved may have no unique solution (instability, bifurcation, etc.). 1. **Choosing the discretization** The discretization must be chosen focusing on the fact that it must be consistent with the loadings that one wishes to apply, especially if those are not monotonic. The more important the non-linearities are, the smaller the load-increments must be. Also, if the behavior of the model is complex, the integral of the constitutive law is not completely implicit: in that case, it should be verified that the increments are sufficiently small for the model to converge. According to the standards, the management of the time-steps can be automated to a certain extend. This allows us to reduce the time-steps if there is a convergence problem, or even to increase it if the non-linearity is weak and the convergence is fast. For the sake of diligence, it is advised to verify that the convergence is reached by performing a second calculation with smaller load increments. 2. **Choosing the boundary conditions** It should be clear that in the case of softening-types constitutive laws or if a limit load exists, the loading with imposed forces might become not admissible, as shown in the figure below. In the first case, the closer the imposed forces get to the limit load, the harder it will be for the model to converge until it becomes impossible. In the second case, it will be impossible to exceed the effort corresponding to the first peak and obtain a solution after that. ![](https://lh6.googleusercontent.com/Au1ydEtcih5L1IVWGrSf1bIH8gh-Q27_NTYgEOiaxvJ9xFuQ2U3dLZxpWcybVZpiIm2OiMntMmQqs6cxONAOC621-GC8KaTA_GmG0J4qvn5nC9Q9CG0zstxuiXjSguBko6Dclkosq31wx1Th0F-YjQ)![](https://lh6.googleusercontent.com/9gs6Ab_XvjjNwV_BYZuRMx9ybHJKfmOy6wCyd6u0erTi9o_RhHnLk0BAin7MoJvOjQ6h3BDFePRfeHNB4T-9KrOmjubctHFzVVYJkXn-LzjaP3WgXhFjQOTq2KADQcZfxdfa5lxtNA_4UU1qCLo-rg) *Examples of response with limit load or loss of stiffness* There are other cases, where there is no unique solution for a given effort or displacement. It happens, for example, in the case of buckling of thin shells or when the problem has bifurcations, for instance, dissipative branch and elastic branch (see figure below). ![](https://lh3.googleusercontent.com/uHnWTJmDLOjcAWQ6DPV97t9a5HfT96kprTGwQUMbTWG8T20n1QoWIaCYxYgNPXHdfXZfvDdoNjuU9N8dEXHBW87X5HVjfz51Q8bbK403ePOjvGKMDKDFRgTS-18VcxMXEPkETTrL76rAhGr0DDbqIg)![](https://lh6.googleusercontent.com/rx4ekh5kCriXc1juU4jmJ3_1MneD1mGH_tdMCT4gwGvCZWblEfbi1Za2AXM_G4uL7HBAxxhUiFwI-MoBFPSZOnZO1VoFb65ySTPgCeSvR_ZiELiluOr8tXSPANvK3TTQjoRmos94_uRviFuzSu_kFQ) *Response (a) with multiple branches (b) non-monotonic loading and displacement* If the model requires imposed forces, the problem can be solved by continuation or arc length methods (see Code\_Aster \[R5.03.80\] documentation for instance). For an algorithm to work effectively, it is then necessary to conceive its model and to prepare its data, so that one looks for a unique solution by introducing multiple restrictions, such as: - The need for equilibrium stability (in a specific way to be explored!) - Equilibrium with a “minimization of plastic deformation energy”, - Equilibrium with a “minimization of average curvature”, - Equilibrium with a “minimization of the difference between reaction forces” 3. **Evaluation of the convergence of the global non-linear algorithm** The stopping criterion for the Newton algorithm must be considered carefully. It is advised to verify what limit criterion is programmed by default in the software. For example, certain algorithms test the convergence using the norm of the residual (in that case, the criterion depends on the unit used for the forces in the calculation, the precision is not the same if the required residual is 1N or 1MN). Other software use a criterion where the norm of the residual relates to the norm of the loading (in this case, the convergence does not depend on the chosen physical unit). Special precautions must be taken when different elements are mixed (solid, structural elements) or when compound elements are used. In general, one must be careful when the convergence criterion is modified from the recommended value to reach certain results. # C4. Convergence issues? Symptoms and solutions #### **C4. Convergence issues? Symptoms and solutions** As opposed to linear elastic calculations, non-linear calculations can perform iterations indefinitely, never verifying the stopping criterion, but they can also be interrupted abruptly at a given load increment (after the first one), with the warning “zero-pivot”. Let us examine the causes of this type of errors. 1. **Non-convergence of iterations** This phenomenon is almost always a direct consequence of the inadequacy of the used iterative method: the problem to be solved certainly does not satisfy the mathematic conditions, which ensure convergence (non-contracting operator, non-positive operator, non-convex operator, insufficient restrictions in the interval in which one looks for the solution, etc.). This phenomenon may be a consequence of accumulated round off numerical errors that can be attributed to the algorithm itself; however, it does not happen often. The evaluation of the residuals over the iterations may provide information about the nature of the problem: - The residuals tend to zero, but more slowly. This behavior indicates that the mesh is not adequate to calculate the equilibrium: it is the case of the localized phenomenon, where the non-linearities are concentrated in certain parts of the structure. In that case, it is better to restart the calculations with a mesh that is better adapted to the structural mechanism. - The residuals become larger and larger. It means characteristic instability: there is no longer, for this structure, a possible equilibrium configuration at this loading level. After a given state, the residuals increase abruptly to a certain value and then start decreasing again, etc. This behavior appears when the algorithm finds multiple possible solutions: it converges to one of them, then “bounces” towards another one. In other words, there are multiple possible equilibrium configurations! 2. **Abrupt stop** The abrupt stop of the algorithm in a non-linear calculation is often reported as a “zero-pivot” warning when solving a linear system. This expression refers to the “pivot” in the Gaussian elimination method, which is the algorithm used (with small variations) to solve linear systems. Most parts of iterative algorithms replace the problem with a linear system. This situation corresponds to the structure becoming unstable; in elastoplasticity or damage, it means that the structure lost its cohesion. For large displacements or contact problems, it reflects the formation of a mechanism, especially, the possibility of rigid body movement: all interface nodes slide, and the restraints are not enough to reach equilibrium. It may also happen that the algorithm stops for reasons not connected to the state of the structure whatsoever: disk space overflow or programming bug. The first one is easy to solve. 3. **When nothing works** If a non-linear calculation does not converge, and one cannot find in the explanations above the reason, it is recommended to ask oneself the following questions: - Is the initial configuration of the structure in elastic equilibrium? - Is the meshing adapted to the problem one wants to solve? Is the mesh sufficiently refined in the zones where the plastic deformations take place? Is the mesh not too deformed? - Does your model mix solid elements with structural elements (beams, plates, shells)? Do the zones with plastic deformation/damage affect the nodes shared with those ‘Strength of Materials’ type elements? - Are the finite elements well-adapted to the problem? Are there stress oscillations? # Chapter D. Civil Engineering #### **Chapter D. Civil Engineering** **D.1 Civil engineering materials** [D.1 Civil engineering materials](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d1-civil-engineering-materials "D1. Civil engineering materials") **D.2 The categories of structural elements** [D.2 The categories of structural elements](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d2-different-categories-of-structural-elements "D2. Different categories of structural elements ") **D.3 The steps of construction** [D.3 The steps of construction](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d3-the-different-construction-phases "D3. The different construction phases ") # D1. Civil engineering materials #### **D1. Civil engineering materials** The objective of this chapter is to highlight the peculiarities of civil engineering materials regarding FE modeling. Among those, there are the particularities of the civil engineering materials themselves (concrete, timber, steel), and their use within the structure. 1. **Concrete** Concrete is a compound material composed of cement paste, and aggregates of various sizes. The cement paste that contains water and additives acts as a binding agent (glue) between all the aggregates. Even though concrete is a heterogeneous material, it revolutionized the world of construction because of its characteristics such as its versatility, adaptability (offering a variety of aspects: form, color, texture), mechanical resistivity, fire resistivity, acoustic insulation, and diversity (high-performance concrete, precast concrete, etc.). However, concrete is subjected to degradation processes. The latter can be due to environmental factors such as humidity, rain, cold, freeze-thaw, heat, wind, drought, aggressions from deicing rock salt, alkali-reactions, internal or external sulfate-reactions, corrosion, mechanical solicitations due to collisions, and load increase. Depending on the degradation phenomenon, the deterioration of the structural element is progressive and initiates as soon as the concrete tensile stresses are applied. Degradation leads to the emergence of small cracks and localized deformations. The increase of the deformation leads to the decrease of the material’s strength, which can then lead to softening behavior and the collapse of the structure. **Constitutive law** – In the FE calculations, generally, only some aspects of the concrete behavior are considered because of its complexity. To express the most relevant constitutive law, it is necessary to well understand the characteristics of concrete. Thus, it is essential to know the behavior of the cement paste, as well as the behavior of the aggregates, both responsible for the stiffness properties of the material. The paste is the cause of the mechanical strength of the concrete and, because of its water content, is also the cause of the deficiencies such as the increase of porosity, the decrease in mechanical strength, the delayed effects (shrinkage, creep), and the transfer of aggressive agents. Concrete is considered as a “quasi-fragile” material because of its complex behavior. Its main characteristics are highlighted in the literature. The most significant one is its fragile behavior in tension and more ductile in compression and when subjected to unilateral forces in a tension/compression cycle. Other properties must be considered such as the shrinkage and creep according to the environment and the loading applied to the concrete. In the literature, the two main approaches to model the behavior of concrete are: - Models relying on a **continuous approach**, meaning that concrete is considered as a continuous media (Bazant, 1979). Using this approach, the calculations of the cracks are deduced from the displacement-force relationship. There exist different models such as the elasto-plastic (Ottosen, Drucker-Prager), damage (Mazars, Laborderie), smeared crack model, of gradient type, or energy type models (fictitious crack model (Hillerborg, 1984), crack band model). In some cases, elasto-plastic models are used, but the user must be very careful, once the elastic phase is overcome, it is possible to obtain deformations that do not reflect the behavior of concrete at all. - Models based on a **discrete approach**. Indeed, concrete cracks generate geometrical discontinuities, which are integrated between the boundaries of the connected elements. There exist discrete models of Ngo, (Ngo, 1967), Bazant (Bazant, 1979), Blaauwendraad (Blaauwendraad, 1999), and other lattice-type models. However, in the literature, the two most used model categories are the ones based on mechanical damage and the ones considering explicit discontinuities. Although the elastic component is not exactly linear (\[Baron\] p.276; \[Sargin 1971\]), the calculations are generally conducted using the isotropic linear elastic assumption (Hooke’s law) to represent the elastic phase of the concrete behavior. The values of Young’s modulus and Poisson’s ratio are computed by characterization of the concrete. In the eventuality that other mechanical characterizations of the concrete cannot be conducted, some properties such as the compressive strength can be deducted using model laws that can be found in model-codes such as Eurocode 2 for instance.Note – Design offices use the model-codes except for study cases when they conduct detailed analyses on a specific structural element on which particular mechanical phenomena occur: cracks, heave, or local heterogeneity. Indeed, there exist finite elements of “cracked element” type, damage models, viscoplastic laws, or even poro-mechanical coupling laws. However, to conduct these studies, data from on-site or sample analyses of the material must be available to orient the engineer towards adequate constitutive laws, for which, coefficients and moduli will have to be determined anyway.
**Elastoplastic model** – For the sake of simplicity, concrete is often modeled as an isotropic homogeneous elastoplastic material, which is acceptable until the concrete experiences cracking. Regarding an elastoplastic law, concrete cracking is not directly modeled: the cracking zones are characterized by important anelastic deformations (>1-2%) and a fixed constraint state between tensile f_{t} and compressive strength f_{c} of concrete. As shown in chapter 3, an elastoplastic constitutive law for concrete is composed of an elastic law and a plastic flow rule associated with a “criterion of plasticity”. However, the post-cracking behavior can be approximated using a stress-strain curve going further than the tensile strength. The latter can cover the effects of tensile softening (representing the necessary work to open the crack) and tensile hardening (concrete contribution in between the cracks, stresses due to reinforcement adherence). If the decreasing behavior of the material leads to a global decreasing behavior, one must pay attention to the eventual local effects: the size of the finite elements will limit the size of the anelastic zones and the solution will depend on the used mesh. Different numerical techniques enable us to solve or limit this issue. **Damage** – A damage law is a law that considers one of the main macroscopic effects of concrete cracking: the loss of material stiffness. The fundamental idea is to renounce following the eventual cracks (their apparition and propagation) and consider that the concrete of a given structure deteriorates by multiplication of cracks in the damaged areas. This type of law allows us to describe the decrease in material stiffness undergoing small cracks. This stiffness loss is measured by an internal variable called damage, denoted D, that evolves from 0 (undamaged material) to 1 (totally damaged material). This variable is generally a scalar value. To best represent the behavior of concrete, the damage laws consider post-peak softening behavior. This enables determining the stresses as follows:![](https://lh5.googleusercontent.com/LVnurX0lvSgEWk9w6PkOR4Bm2mffTRl7n1tM0JaoaBpPcTTvzKibtMMtd91gyHQTEeDEnr9ky3us4CpCKAtdhyAXX77XnRG58EE8kqR8FGhLrGT7VvemfSCOhoNIfRE_C736Zln-gEI5Q2B_2dSIsg) with ![](https://lh4.googleusercontent.com/83MlBC3-r0r487Li3OTdPXtyFn9scSPKdaj8kbGcA49GAfdpUvOqr-JoGuVGh2Ea7wtTYeKCWxUGaMcfM3McgnlO7267FC7pSbcdmYvekeT0rIkVy8fQ9nuycYSaTc6Ra5lk15E8wwg3XQfCA8hvyQ) The advantage of this method is to consider the concrete as a “continuous medium”, for which the FE methods are perfectly adapted. In the case of concrete behavior, the two main damage modeling families are the anisotropic and isotropic ones. The isotropy characterizes the invariance of the physical properties of concrete regardless of the direction. On the other hand, the anisotropy depends on the direction. An anisotropic law presents different responses due to loading according to its orientation. One of the most used damage models in the industrial and research world is the Mazars model \[Mazars, 1984\]. It is certainly the first damage model for concrete that works accurately. The main difficulties raised by the damage models are: - a dependence a priori of the meshing results: note that one should, in principle, demonstrate that the ruin mechanism obtained with this type of model is independent of the refinement of the mesh, at least after a certain threshold. Besides, this dependence led to the development of the regularization method. - the absence of an analytical solution in these simple cases. Several regularization classes exist including the non-local regularization and the regularization by cracking energy \[Hillerborg, 1976\] (that solves the problem only partially). Among those non-local methods, it is possible to cite the integral methods \[Pijaudier et al., 1987\], \[Giry et al., 2011\] or gradient methods (deformation gradient or internal variable gradient \[De Borst et al., 1992\], \[Peerlings et al., 1996\], \[Nedjar, 2005\], \[Lorentz, 2017\]. These methods require the use of relatively thin meshes, which renders the analysis computationally expensive. **Delayed effects of the stress relocation** – When analyzing the behavior of a concrete structure several weeks after pouring, but especially for the long term, it is necessary to consider the delayed effects such as **shrinkage** and **creep**. These phenomena specific to concrete can, in principle, be modeled adopting a visco-elasto-plastic constitutive law (Bingham law), or sometimes only visco-elastic (“scientific” creep, \[Eymard\]): this approach is generally applied by research laboratories to analyze tests on materials. However, in the case of a refined model considering the delayed effects, it is necessary to incorporate phenomena such as drying and cracking in addition to shrinkage and creep. Indeed, all these phenomena interact with one another, so it is important to model them numerically. The deformation caused by the shrinkage is induced by the drying of the concrete due to the environmental effects. The shrinkage leads to a differential deformation, meaning that the stresses are more significant where the concrete dries faster. This phenomenon causes tensile stresses at the surface, which then leads to cracks and compressive stresses inside the body. Concerning creep, its deformation is generally separated into two deformations, one is due to creep itself, and the other one to shrinkage from the drying process. The latter can be explained by the strong dependence between relative humidity and creep. In Eurocode 2, it is possible to determine concrete deformations due to the delayed effects (without external loading). For this purpose, one must compute the deformation due to the endogenous shrinkage (caused by the internal humidity) and the desiccation deformation (caused by the drying process and the size of the structural element). According to the §3.1.9 of the EN1992-1-1, the creep deformation under compressive stresses σc can be written as: ![](https://lh3.googleusercontent.com/cuTTcEIdWmvHNnGggP8O0KhS2g9Akqep341qzYqE7hXJJJQIo2NlD2w9552xv_LvIC6yVDPLLDcjWQ1RldG22fmuInjmZdJs4O1Q2_GJB3-UudDSqKflg8b7fc3ffK4furFUk07bm3fnWEilYvjsMQ) with E_{c} the tangent modulus (equal to 1.05 E_{cm}) and φ the creep coefficient. The Eurocode 2 (EN 1992-1-1) describes a simplified calculation method of φ (∞, t0). Annex B gives a more complete method enabling the estimation of φ(t, t_{0}) as well as the shrinkage evolution (see the annex B of EN 1992-2). Moreover, it is important to remember that the calculation of the delayed deformation is relative to the type of cement paste. 2. **Structural steel** The behavior of steel is much simpler than the behavior of concrete for several reasons: it is an isotropic material with identical strength and moduli in tension and compression. Moreover, it is subjected to industrial quality control to ensure its homogeneity. **Elastic models** – Even though steel behaves essentially as anisotropic elastoplastic material (Eurocode 3, part 1.1, §5.4.3), the typical models for steel structures, or compound containing steel, adopt a linear elastic behavior. One must then check that the elastic constraint threshold fy was not reached. In the case of beam or column type elements, the codes allow, if the sections have a size that guarantees a sufficient local ductility, to exceed in the analysis the elastic strength and consider reaction moments based on the plastic distribution of the stresses. **Elastoplasticity and strain hardening** – The elastoplastic theory was developed from the study of steel alloys, mainly to predict the rolling and forging stresses (\[Hill\], \[Nadai\]). For steel, the usual model is composed of Hooke’s law for the elastic deformation and the plasticity criterion denoted “Von Mises criterion”, as explained in the Eurocode 3 (part 2, §7.3; part 1.5 §10 and part 1.7 §5.2.3.2): for this criterion, only the elastic constraint threshold fy of steel must be provided. Considering the FE calculations, another issue is the strain **hardening** of the material, meaning the hardening in the purely plastic phase. This aspect is notably explained in the annex C6, part 1.5 of the Eurocode 3. Since it is hard to verify the model, it is preferable to conduct a preliminary computational model with no strain hardening: indeed, one can then verify the quality of the obtained results in the plastic zones by observing the eigenvalues of the Von Mises stresses (the plastic zones must be about monochrome). Nevertheless, it is important to note that the use of an elastic perfectly plastic law with no strain hardening can lead to convergence issues of the linear analysis. Indeed, the plastic zones have zero tangent modulus and, therefore, no stiffness. Considering strain hardening can stabilize the numerical resolution. In the case of strain hardening, until a stress fy+X is reached, the possible loading/unloading phases are elastic, with a modulus equal to the initial one. Thus, fy+X becomes the new elastic yield stress of the material. Moreover, the behavior of the steel is close to the kinematic strain hardening model. As a first approach, one can consider a tensile strain hardening up to a certain stress value (fy+X) that will decrease the compressive elastic yield strength to fy-X, and vice versa. The most common steel model is the isotropic strain hardening, which depends on the accumulated plastic deformation: ![](https://lh3.googleusercontent.com/IMxlT44swv9pLVi9SF6x3ZwvWyeIHbb-2N9w9iAuV2cVovHLAM236hBAQ49fKsVzZZLtRXP6_Vo-yn2NHg95RdbUTWS9IODYSWiFqB1slrIw1aR_r8NjCq0gZ-4ABZJdA0XqPTh3WnHc-iCvd818JQ) where ![](https://lh5.googleusercontent.com/cihePpzw0U0SOzhGYyB1B5_aaE3ldXydMfzdqsWhGENAzBJSL6BjUXxVNpr-iWl-dRNtyRawlpSvMb0LYHERe8eFZMi9xMGfb1ENQZCp1gO95-PxjbtnngA1cciIReNnr0aH-ePv8YbD9JejltjkrA) and f_{y} an increasing function. In this case, there is no distinction between tension and compression, so a strain hardening in one direction leads to an increase of the compressive elastic yield stress. This hypothesis is accurate only if the considered loading is monotone and not cyclic. In most numerical computational models, one can retrieve the eigenvalues of the cumulated plastic deformation. Thus, it is possible to verify that the Von Mises constraint is distributed according to this deformation in the plastic zones. In the specific case of stainless steel, the hypothesis of a linear behavior up the limit of elasticity fy corresponding to plastic deformation of 0.2% is not respected, so it is recommended by the Eurocode 3-1-4, § 4.2. to consider the effects of the nonlinear behavior on the force-displacement relationship in the deflection calculations. The material law is of Ramberg-Osgood type and recommendations to implement this model can be found in annex C of this section of the Eurocode. 3. **Pre-stressing steel** Regarding their behavior, steel cables (braces, tension cables) and steel for pre-stressing differ from other structural steel only by an elastic limit about three times greater (from 1680 to 2140MPa in France), which is justified by the serviceability solicitations, generally greater than 1000MPa. One can then, firstly, model the pre-stressing reinforcement as linear elastic elements or elastoplastic of Von Mises type. Steel elements for pre-stressing are all hot-rolled, so the linear isotropic strain hardening law in the plastic phase should be taken into account. The strain hardening coefficient h can be calculated using the characteristics guaranteed by the manufacturer: ![](https://lh6.googleusercontent.com/H_JaqqXu9T4syw1jy-IcZ-YWuYlmhVX1ZDoYZqPqU1hmaKLfiGXP1WVgtEAOPkTEXVIldnGF4c8tY7IEUgAcU8Yzh0A7JX85k-Sc1Ju6YJPh0DyZUfby3F9qUdvf03SACAh0Vvf9u29sDn3lItsyYg) with R_{m} the constraint to failure, f_{p0,1} the usual elastic limit, E the Young modulus, and A_{gt }the elongation at the point of failure. A direct consequence of this high level of stress is the initiation of the relaxation mechanism. Relaxation of steel is a non-elastic delayed effect that depends essentially on the time spent since the loading was applied. It leads to a progressive decrease of the constraint for bars and cables subjected to a constant elongation. This mechanism initiates at ambient temperature only for elongations exceeding about 60% of the elastic limit (≈1000MPa). Relaxation increases slightly with temperature. Alike concrete creep, it is possible to model the relaxation using a linear visco-elastic constitutive law. However, this approach is mostly used in research work. It is not common to model steel for pre-stressing: generally, it is accounted for by introducing a distributed force within the pre-stressed concrete. Nevertheless, for detailed analysis, in which the interaction between the steel cables and the surrounding medium is of interest, relaxation can be considered using an incremental time-dependent calculation with the relaxation losses introduced as initial stress conditions. 4. **Passive steel** **Normal mechanical actions of passive steels** – For FE calculations, passive steel elements are frequently modeled by linear 1D elements of “bar” type. According to the historical reinforced concrete methods, the reinforcement is considered to work only in tension/compression along its own axis, which is exactly what FE models enable. Connecting those bar elements to the nodes in the solid elements representing the concrete makes it possible to avoid mechanisms specific to “bar-only” assemblies. In most computational software, the bar elements are considered by default as elements with a linear elastic behavior. Considering the 1D characteristic of these elements, the law is of the type N = E A u/L, with u the axial displacement, and N the normal stress at the nodes. It must be verified afterward that the axial force N/A stays within ±f_{y}. **Friction** – What was said in the above paragraphs is valid only if there is a continuous friction force acting between the steel reinforcement and the concrete. 5. **Timber** Timber is a material that possesses some inherent peculiarities: it is not homogeneous (this is true at various scales), it is not isotropic, it does not show symmetrical behaviors, and it can be subjected to ductile or fragile failures according to the solicitation and its orientation. Timber is sensitive to humidity, which has a direct impact on its dimensional characteristics, stiffness, and strength. The duration of the loading has an important impact on the strength and the deformation of the wooden elements. The variations in humidity can amplify the deformations (mechano-sorption). Relying on the previous observation, one can imagine a method to implement the FE analysis in this particular case. **Homogenization** – The hypothesis must be validated for the Representative Elementary Volume (REV), or at least, the volume of the smallest finite element. Knowing that according to the different timber species the growth ring can exceed 1cm, it becomes difficult to assume this homogenization hypothesis close to the connections (peaks, pins, bolts…) with a diameter of the same order of magnitude, or smaller. The presence of nodes is rarely considered when modeling structures or structural elements. **Orthotropy** –Timber has a structure and characteristics that are a function of three directions, the lengthwise directions (the axis of the trunk, wood fibers), the radial directions, and the tangential directions perpendicular to the lengthwise direction. The last two constitute a plan, often named the cross-sectional plane of the beams, on which the growth rings can be visible. The orthotropy coordinate system is therefore quasi-cylindrical. On the contrary, the coordinate system in which the elements are inscribed is cartesian. The representation of this orthotropy, when considered, is in most cases limited by an isotropic transverse hypothesis (radial and tangential axes having identical characteristics) in a cartesian frame. The slope of fibers associated with the presence of nodes is generally not considered in the FE calculations. Rather, it is modeled in the assembly calculation especially for the assemblies by contact. The flexibility matrix (inverse of the stiffness matrix) can be defined as follows for an orthotropic plan: ![](https://lh4.googleusercontent.com/NqE1hFGF-sEKkOsDU_B9ar4LjTIBj0p4nj_i5OOQDEekWyugj8_D7eSmCg9T5PD2LyJo_a4mdQLZwnncox5VgMVReQUMObEbeM8s4al-Dg8EPhdDoWvlA0t_Tj6SBsod-48oEiwO2mg0jB7769WvWg) **Note**: the orthotropy and symmetry hypotheses of Sij reduce the number of independent terms from 36 (most general 3D case) to 9 terms. ![](https://lh5.googleusercontent.com/hhy9gvf1RIc6_krbAlJmgOdoC-WU9PvrzIFY2KFeo7xx3zE8MFKWndA14CVYhsLz_WhXvjWhWPE7JuTgvFCQbh00XauHkLzG3ObhN7dTDcwH5oRFIZcQl6FTbeJ0Tmyo1MgdTG36BUfTBs0NBNnJaQ) *Timber – orthotropy hypothesis* **Elastic modeling** – One must simply know the isotropic transverse matrix of behavior for a 2D or 3D model. The moduli between the lengthwise/longitudinal, radial, and tangential directions can present ratios of the order of 20. They evolve as a function of the loading period (creep), timber humidity when constructing, and during its lifetime (environment). The representation of the FE method will depend on the pertinence of the parameters considered. **Plastic modeling, failure criterion** – For an isotropic transverse non-symmetric material, the Hill, Tsai… criterion can be used knowing that it will be necessary to describe the perpendicular tensile and shear fragile failures. The significant strength variability makes it harder to fix the criteria parameters. The sequence of growth rings or assembled layers with different mechanical characteristics can render a homogeneous model difficult to fix in terms of strength. Indeed, the strength and stiffness are highly correlated for timbers and “systemic” effects appear quickly in terms of element strength. Consequently, there are strength limits in axial tension, axial compression, bending…. Finally, timber structures are particularly sensitive to the behavior of their assembly. Thus, the elements do not need to be modeled in detail, only the assembly zones do. Nevertheless, problems can arise because of the contact zones, the multitude of materials, some of them entering plasticity, the fragile failure of others, and the homogenization limits reminded earlier. It is clear that the modeling effort is related to the scale of the investigation or the advancement of the project. Provided the above singularities are considered, the modeling of timber inside of a structure can be conducted like any other material. **Modeling of the delayed effects and the interaction with the hydric/water phenomena** – Timber is a hygroscopic material sensitive to the relative variation of humidity of the air. Moreover, it is subjected to creep under loading. If one wants to model these phenomena, a rheological viscoelastic model in a variable environment and respecting the thermodynamic principles can be adopted. The generalized viscoelastic behavior of Kelvin-Voigt type, characterized by rheologic parameters and dependent on the level and history of humidity can be associated with the Ranta-Maunus non-viscoelastic behavior to characterize the shrinkage-swelling and the mechano-sorption. # D2. Different categories of structural elements #### **D2. Different categories of structural elements** Here are presented the peculiarities of these elements regarding FE calculations. 1. **Reinforced concrete elements** **Considering the delayed phenomena** – Usually, the project engineer is interested in the redistribution of stresses and the delayed deformations that accompany the aging of the materials. To achieve this, the static calculation by time increments is particularly well adapted and largely sufficient. The shrinkage and the creep of concrete for instance depend only on the time that has elapsed since the pouring phase. Using the incremental calculation, they will be introduced as imposed deformations at each node of the mesh. It is possible to compute beforehand, for each time increment the shrinkage and creep related deformation map: the FE software incorporates the initial state seeking an equilibrium of the elastoplastic material. Nevertheless, attention should be paid to the interaction between the delayed effects and the construction phases, as it will be explained later. **Consideration of cracking** - When concrete cracks in tension, cracks develop towards the nearest face, as well as along the steel-concrete interface (\[Goto\], figure below). ![](https://lh3.googleusercontent.com/px5SUN7ztGzrRzAeLJhR6filpe666G18-EwVr34QpKV-tAs45do9Cq3EkeBr21Agw2Lb-5bRaTI5TGqdFdJ0cRiWcFgyDyY-r8nMIgkHk96HYk7eMXQjPtiXsdCpCaiZJgtXW2DogdVQMEHQIZvuyA) *Internal cracking of the reinforced concrete* When considering a tensioned connecting rod of cracked reinforced concrete as a homogenized continuous medium, the behavior law N(ε) (with N the normal tensile stress) follows the trend of the figure below. ![](https://lh5.googleusercontent.com/WggLg43yJqTRKVXrPexfvrxgheUTtrzGRwEZXzjmimiTpxHeQFk_joS7PlPh7a490SzZmmTCkbBKGH-NEte8fEsOBVM9VqdSfM7XpwtLeRKNwkoeUbSSDKmyd75siDxUkUwoj81CudJt4KO9acy1Ng) *Model of the tension stiffening effect* The Model Code 1990 of the CEB-FIP expresses an analytical formulation. This relationship can be used by modeling the section of cracked concrete as a bar element whose stiffness would be updated in increments (depending on the value of normal stress or elongation, since the relationship is invertible). It can also be used as a law for the behavior of a fiber of a multi-fiber element. **Cast Concrete** - For cast concrete areas (e.g. by passive reinforcement), it is possible to take into account the residual post-crush strength, as indicated in EN1992-1, using Sargin's law: ![](https://lh5.googleusercontent.com/_woZLiqrRwau24vacnjOWpcP9hAIAdKqqPnorNZxAG7uivUr5o95ZTIaObMSUkyWUkCnhWIgpKeGlbTEhl4MeF1u-jwEoZ5X0no04cJC-NTZDf2fxZRLUixUsy_I0FnSHxUK-ECWiK3fFoVA9oXRWw) ![](https://lh6.googleusercontent.com/eFiUL6PuaYT6Pu29RlU5NVHEjCguummjIlUJsBGVqPf5SWoiHGJg0TaG-un8SKOIOPILnpLyyWlbCMkTnRAN40dR3tLXxI1f7Gr3fJIBZjI3L6Grk-ivIjjfaVxDMqnleUCp08tFPKkj828NIKOSTQ) with εc1 the peak value such that ![](https://lh5.googleusercontent.com/Ls8sAmno0JijW1BW4nupXVWqF5v_tVci98xlLg86oHtECrd1SD3-t7hfBBAFh-4S-rfT4NWthg1Hgws7-uzas_h62Xu6DQDcaOHTzPC-asF1S6HmQzCzTxBbAhmas9CDTc67hR_-rYe38JRdpBCdsg) ![](https://lh6.googleusercontent.com/TinIRg69yfRtkcvLMHnYeo6h4EASlz8ebaDQR5k-AsXgo_CzWE8BYwI6pdTm1BgfCAWzxF3a0u1caOLbGl8OFYuBOj-FPzXQrUkfm4EMVQX0wL6em2KqHzNO73BC0YpBaUp8Sk46B19Z4C4PIevf9Q) with ![](https://lh5.googleusercontent.com/fKPv11FDazD-fTFdtojYh_--enCDIAXoRlBTKXYt0cNCYGNV0Ih_lTp4nG1Xy5AinS19W3jc2RAJrwLLWrgKSTkE4Ay1E1B_7KuZn6GrmhrJGNgp3giFiaoZ4oFNuKxTFWomv9PEPxw6NwohcQ2tvw) For ![](https://lh6.googleusercontent.com/DGk8eoTFCTNuCZodicj4qD5JFSb93o3xCyZPMp1NUxanpk3LY5fjUDY4AjflapHI8IMFSEV2nTj8E8Cr8Pq5p8YxH42bu6UC9INu6qTqgzbgbP574J9BbRj_AKuO_u7lUAxMQR_PZZbJwbj15NKLHA) The EN1992-1 §3.1.9 also suggests an increment of strength and deformation of concrete when it is subjected to a confinement stress of σ2=σ3 such that: ![Une image contenant texte Description générée automatiquement](https://lh3.googleusercontent.com/E1-1Z10ae8uzx1T6dHkPKNsY76Z2ssS5BYz069baiCfXUQ2m2dzB1U93dbme_De62LbZgkP9-OHNlhSHWgPvd9uDHoRmkLtt9LGMCnovL-NETJy_Demh9mcy0CvEtw2KHPmidZxYiv84xfO5qVbQJg) However, this law is only one-dimensional and is only valid under monotonic loading. Therefore, it can only be used with the finite element method when modeling concrete confined by a bar element (so the modulus would be incrementally modified), or as a constitutive law of a fiber of a multi-fiber beam element. 2. **Pre-stressed Concrete Elements in Pre-tensioning** Prestressing by pre-tensioning, which is characteristic of industrially prefabricated concrete products (beams, pre-slabs, honeycomb slabs, girder, etc.), consists of tensioning cables (wires, strands or bars) on manufacturing benches, then pouring the concrete before slackening the cables when a minimum concrete strength is reached (called concrete sag resistance). The amount tension in the cable (which must not exceed the maximum prestressing force allowed by design codes), the number of cables, and the strength of the concrete are adjusted according to the loads that the prestressed floor or element must resist. When the cables are loosened, instantaneous losses, of the order of 8% for a prestressed pre-slab for example, must be taken into account (losses due to the entry of anchors, to the relaxation of the prestressing reinforcement during the period between the tensioning of the cables and the transfer of the constraint, to the elastic shortening of the concrete under the compressive stress imposed by the constraint) when designing in the provisional phase of construction with a prestressing transmission length to be considered starting from the end of the precast concrete element. In the longer term, delayed losses due to shrinkage of the concrete, relaxation of the steel, or creep of the concrete, which will finally reach a total loss of 20% for a prestressed pre-slab, must also be considered. In many FE computational software, prestressing can be incorporated in beam-type finite elements representing the cables connected to volumetric finite elements representing the concrete. Depending on the study area, it may be necessary to consider the transmission length of the prestresses in the cables, for example in the end zones. The distribution of the actual prestressing force (considering the instantaneous or delayed losses as a function of the moment in the service life of the product where the calculation/verification is to be performed) is then variable along this transfer length. A linear distribution of this prestressing force is allowed in most computational software and remains safe for dimensioning purposes compared to the more realistic parabolic distribution. For reasons of complexity and need (designs limited to elastic deformations), the modeling of these elements is generally carried out with linear assumptions (constitutive laws of concrete and linear elastic steel, perfect contact between concrete and steel...). However, for refined studies, non-linear hypotheses can be followed according to the need such as damage type constitutive laws for concrete, elasto-plastic type constitutive laws for steel, and the introduction of steel-concrete interface elements. 3. **Pre-stressed Concrete Elements in Post-tensioning** **Elastic losses** - Post-tensioning of the prestressing cables is accompanied by instantaneous losses: friction, anchor recoil, and loss due to elastic elongation. **Delayed effects: creep, shrinkage, and relaxation** - Delayed effects are considered using an incremental calculation. Creep and shrinkage can be introduced as incremental volume deformations given at each node of the mesh. 4. **Steel Structures** Choosing the type of analysis Due to their high slenderness, steel structures are very deformable. As a result, the traditional assumption of reaching stress equilibrium in the initial configuration is not always valid. It is then necessary to establish the internal stress distribution in the deformed configuration. The sensitivity to these non-linear effects, sometimes called second-order effects, is expressed through the critical multiplier αcr: the load multiplier leading to the Eulerian instability of the structure. In the current version of Eurocode 3: - if α_{cr} > 10, non-linear effects can be neglected. If the global structural analysis incorporates the plasticity of the elements the limit value of αcr is increased up to 15, - if 4 < α_{cr} < 10, they must be taken into account. This can however be done with a classical linear elastic analysis by amplifying the transverse forces, - if α_{cr} < 4, the non-linear analysis is mandatory. In the last two cases, if the global geometrical irregularities (or imprecisions) and the element irregularities influence the global behavior, they must be considered. Element irregularities include: - geometrical irregularities: transverse and torsional, - material irregularities: rolled elements or welded elements have self-balanced residual stress distributions created by their manufacturing process. The latter can be represented by an equivalent geometric irregularity, whose value can be found in the current standards. These irregularities must be included in any analysis of a structural member incorporating non-linear effects. In principle, structural or Strength of materials models (bars, beams, plates, and shells) are ideally suited for structural steel calculations. **Wireframe structures** *Elastic analysis* For modeling purposes, it is necessary to analyze precisely: - the nature of the connections between the different structural elements, - the load propagation from each part to the others. *Plastic analysis* When the elementary ductility and/or the assembly ductility is ensured, it is possible to carry out structural analyses incorporating plasticity. Different methods can be used (EC3, §5.4.3): - elasto-plastic analysis, where the plasticized areas are modeled as plastic hinges, - non-linear plastic analysis, taking into account the partial plasticization of the bars along the plastic zones, - rigid-plastic analysis, in which the elastic behavior of the bars between hinges is neglected. *Torsion* Steel elements are rarely massive, they are composed of thin layers to form profiles, open or closed. Especially in the first case, the response to torsional stresses is both in uniform torsion, known as Saint Venant torsion, and in non-uniform torsion, leading to the buckling of the section. The latter phenomenon is usually not considered in commercial software, even though it can have a significant effect on the response of structures. In this case, two solutions are possible: - surface modeling of the element: this solution is not applicable if the analysis is performed on a structure with more than a few elements, - if the situation is similar to that of an I-beam, where the non-uniform torsion can be represented by the alternating bending of the flanges (sometimes called biflexion, Figure), one can proceed to bifilar modeling of the element where the two footings are represented by two distinct elements, connected by transverse elements representing the web. As a result, the specific bending of each flange, and thus the non-uniform torsion, is represented. For instance, this is the case for double girder composite bridges. An application is presented in chapter 3. ![](https://lh3.googleusercontent.com/n-KSBBKkaUYy1ZPoJu0I_Ypw34I8z8KqtnTbYh0rU31ivwXn1AIW53y1zWWd_8wG5j6MAXfRHl-J1iBsv5BV8wTjSqTDEXN9FBg2F-c0LHG4gNH2X6ffhgqyuT3f-2VZcdEXBZEz3IKT7kk7AkYQSg) *Decomposition of torsion into uniform and non-uniform parts: simplified biflexion hypothesis* **2D or 3D elements** The linear elastic analysis of two- or three-dimensional steel elements does not present any specific problems, so the general rules apply. On the other hand, a non-linear analysis may be required to study instability phenomena. Indeed, structures composed of steel plates, whether flat or curved, are subject to buckling phenomena. In the case of flat elements, called plates, buckling is a relatively stable phenomenon: the initiation of buckling of the plate does not lead to failure, the maximum load is reached after buckling. This is called post-critical behavior. In the case of curved elements (shells), instability leads to the immediate and often brutal failure of the structure. From a numerical point of view, in the non-linear static analysis, this leads to a rapid decrease of the load beyond the maximum. In both cases, the maximum load is strongly dependent on the initial deformation applied, in amplitude and shape. The amplitude is fixed by standards. The shape is usually chosen affine to the first mode of instability. However, this choice is not necessarily the most detrimental. It is advised to supplement it with local modes when the structure presents panels of strongly different dimensions. For example, in the case of an orthotropic deck, the deformation affine to the global buckling mode must be supplemented by deformations affine to the buckling of the under panels. In the case of shell-type structures, the problem is even more critical. It is advised, once a first calculation has been performed according to the above assumptions, to adopt in a second calculation a shape of initial deformation affine to the deformation obtained at failure. 5. **Compound structures: steel-concrete** The alternative of a compound steel-concrete construction is sometimes preferred for certain types of industrial buildings and bridges with small to medium spans (midspan < 100 m). The combination of these two materials by making them "work" in their strength domains (concrete in compression and steel in tension) can result in a strong and lightweight design. To achieve this result, the connection between these two materials must be correctly designed. A distinction is made between: - mixed slabs: solid slab + reinforcement, - mixed beams: solid or mixed slab + steel profile + connectors, - mixed columns: steel profile + (concrete filling or concrete coating). Overall structural analyses are usually carried out in the elastic domain by homogenizing the section, or by representing the two materials separately. This second way of proceeding can lead to difficulties in the processing of the results. Indeed, it requires recalculating the stresses on the globalized section to apply the current standards. When more detailed analyses are needed, given the diversity of materials involved in this type of combination both geometrically and in terms of non-linear behaviors, 3D finite element models are necessary to conduct local analyses, which include the processing of the various interfaces (using contact finite elements for example). For studies at the scale of the structure or the elements, relatively high-performance 2D models have been developed over the last decade, such as those based on a fiber cross-section cut-out (fiber model) to enable the section stiffness to be estimated by numerical integration. The assembly of composite bridge girders is another relatively complex detail. Regardless of the assembly solution chosen (butt-strap joint, joist trimmer, or diaphragm), 3D models using solid finite elements are preferred to simplified 2D models, but they are more computationally expensive. **Cracking** - Composite girders are usually made of a steel section that is connected to a reinforced concrete floor or deck by means of connectors. As a result, in areas undergoing a positive moment, where the slab is compressed, strength and stiffness are particularly consequential, whereas in areas undergoing a negative moment, cracking results in significantly lower mechanical characteristics. This cannot be neglected in the overall structural analysis. Different levels of modeling are allowed in the codes: - Flat-rate approaches: for example, Eurocode 4 recommends considering a crack length equal to 15% of the span, on either side of the supports. It also suggests a flat-rate stiffness for composite columns. Eurocode 8 recommends adopting an average stiffness over the whole length of the beam. These differences in approach are justified by the different shapes of the moment diagrams under classical solicitations, mainly gravitational, and seismic stresses, - Approaches defining a cracking zone by analysis of the stress envelopes: Eurocode 4 recommends to consider as cracked any section where the stress exceeds twice the average tensile strength under the envelope of the characteristic stresses calculated, assuming that the structure is not cracked by adopting a long-term concrete modulus. - It is also possible to use non-linear analyses. **Connection** Except in the case of non-linear analysis, it is not useful to model the connection. Current standards allow us to consider the effect of a partial connection on the strength of the elements. For modeling purposes, beam-type finite elements (2D or 3D) are generally used to model the point connection. If a distributed connection hypothesis is considered, appropriate models are available in the literature. **Collaborative widths** Steel beams are connected to particularly wide members, and shear dragging can result in a non-uniform stress distribution across the width of the slab. In wireframe models, this phenomenon is usually taken into account by modeling a slab of reduced width, at constant stress, since it is required for beam models. Strictly speaking, since shear dragging is related to the transmission of shear forces through the connection to the slab, it is therefore dependent on the shape of the moment diagram. The collaborating width should vary from one combination to another. However, the standards allow a single width to be adopted for all calculations. The variability of collaborative widths will be considered if the slab is modeled using surface type elements. **Delayed effects and shrinkage** Since the delayed effects of concrete influence the stiffnesses and stress distribution throughout the structure, they must be taken into account. It should be noted that the Eurocode adjusts the value of the steel-concrete equivalence coefficient according to the type of loading. The shrinkage solicitation induces a self-balanced stress distribution throughout the section; thus it should also be taken into account. **Non-linear analyses** Non-linear computational models of composite structures assume the material and geometric irregularities hypotheses used when modeling concrete and steel materials separately. As mentioned earlier, the connection must be modeled with its own stiffness. However, it should be noted that its numerical processing remains difficult. Usually, it is assumed that the concrete and steel parts cannot be separated transversally and that only longitudinal sliding is possible. The finite element formulation of such a connection can lead to the "locking" phenomenon when the sliding is blocked by the looseness of the transverse stiffness projection preventing the uplift when the equilibrium is reached in the deformed configuration. Therefore, when this type of element is used, it is advised to verify the consistency of the reaction forces in the connection with the tensile/compressive forces of the steel elements. 6. **Braces, tension cables, and suspension cables** **Introduction to the calculations** - Some cable elements can be modeled as bars of the equivalent section. This is the case for vertical tension cables, or prestressing cables, guided in their duct. The curvature of these cables at equilibrium is practically independent of their linear mass. In other cases, the cables tend to be bent by their own weight: the vertical direction is a specific direction that plays a role in the stiffness of these elements. When, at the scale of the cable's span, its curvature becomes important, it strongly influences the stresses and strains it can transmit to the rest of the structure. As an example, for braces, the stiffness of the cable depends mainly on its deflection and elongation. Deflection affects the stiffness of the cable; thus, the tension/deflection relationship of the cable is inherently non-linear. The cable elements present in most codes are based on the \[Gimsing\] model, which assumes that the cables deform as a parabolic curve, an assumption that is valid if the deflection/span ratio is less than 1/12. This model decouples the elastic elongation from the bending of the rope. **The catenary effect** - When the deflection of a rope is greater than 1/12th of the span, it is no longer possible to decouple the elastic elongation from the bending because the tension lever arm becomes the dominant factor in the expression of the bending moment. Several computational models suggest catenary elements to account for this geometrical effect. These elements connect two nodes of the mesh so that a single element is sufficient to model the wire rope. ![](https://lh6.googleusercontent.com/YYgw5GBTgTuvlltxdL31VgEwY4pstaRllkmJs_IPCCWKHGbAKNmvLZ8vGt9V0fIUkNVNV5_1H1e1GpQ-cBuL9dMxWIs3pW59il8uRnP6kGNMkiJt5d7AeRSU3t9UsDBEB_5OisaXWSIcCbikSqmQ-Q) *Nodal displacements of a catenary element* For this type of element, the nodal unknowns are the vertical displacement (in the direction of gravity) and the horizontal displacement (see figure 4). The associated reactions are the variation of the horizontal component of the cable tension, and the vertical reaction at the anchors. Since the relationship between nodal displacements and these reactions depend on the cable tension, finding the equilibrium becomes a non-linear problem, although the structure is globally elastic. # D3. The different construction phases #### **D3. The different construction phases** Studying the phases of construction has two objectives: - to ensure the stability of the structure in the various transitional states leading to the final state, - to calculate the effects that have the assembly on the force distribution and the deformation of the structure. There are various effects related to assembling. They are due to: - the evolution of the static state during construction. For example, a bridge span built by two cantilevered bridge spans and finally clamped/keyed in its center will present, just after the clamping, a moment diagram under permanent loads that cancels out in the middle of the span, which is quite different from the one that would have been obtained without taking into account the assembly method (Figure 5), - the interaction of the delayed effects with the evolution of the static state. In the above example, after keying, the moment in the middle of the span will increase due to creep, - the evolution of the sections over time. For example, in the case of composite steel-concrete structures, if the structure does not rest on arches when the concrete is poured, the weight of the slab is supported by the steel structure alone, - voluntary adjustments of the structure: support elevations, adjustments of the bracings, keystone actuators, ... Taking these effects into account can be relatively complex and, in the most difficult cases, it may be essential to use software that can model the evolution of the structure step by step. However, it is often possible to proceed by superimposing various linear analyses. ![](https://lh4.googleusercontent.com/Zthwr4eVgvccaL0qSmTk15VbPc_84rM7qNf39_vnBuo7qjDAiALO7kRR3p4sumOC16UaoqecpUgx4viwFCU7lwDnTOzcggbtQFc__iFAKbP_aUbD5xh6HcSY_NVKbmv-L97PAI4tK1Z0qnhY0WyyNQ) *Effect of the construction phases in the case of the keying of a cantilevered bridge span* The main issues are related to the effects of the delayed deformation of concrete. Indeed, how can one evaluate the final state midspan moment in the above example? In the case of a single keying point, it is possible to use the method known as the "coefficients method" (Figure 6). This approach is based on the following arguments: Final state = (E(t_{0}, t_{1})/E(t_{0}, t_{∞})) x Final state not keyed + (1-(E(t_{0}, t_{1})/E(t_{0}, t_{∞}))) x Final state without phasing. with t_{0} the duration of load application, t_{1} the duration of the keying, t_{∞} the time considered for the final state, and E(t_{0}, t_{1}) the concrete modulus for obtaining the deformation of the concrete at time t_{1} for a load applied at t_{0}. This method, in the case of a single keying point, outputs the exact theoretical final state. However, it is difficult to extend it to the case of multiple keying points and can lead to absurd results. **![](https://lh6.googleusercontent.com/_kCDYgXOI9fNgksjLnFpCqfnltbHFtnapsyUfF0J0FW-3g2231DUcfqg3hlMDkhMtsOID0Qppa4_4nkFa4bYYYp6x4s4KT4yMkvtznQrcvwrFWIYCFsDQihv_T9YJ-bw9TxAN91-5i-r5UUEXhUFag)** *The unitary case used for the coefficients method* It is best to externalize the effects of changes in the static state as follows (Figure 7) : - case 1: calculation of the final state, if the keying was not carried out ; - case 2: calculation just before keying, with the adequate concrete modulus; - case 3: calculation of the effect of keying: apply an imposed displacement to the structure at the keying point returning the value of the discontinuity (for this example, in rotation) to the value fixed by the keying process, - the final state is the sum of cases 1 and 3. This technique can be extended more easily to cases where the static configuration of the structures is modified many times. ![](https://lh3.googleusercontent.com/JZQxP9UjYxOrhf2yIy3s4Hy7cU8e10aIOJnmrymwzXdgnmafVjga5Wc35_pswz8i7jlPOj5w7zSWfrEu9-SaypSxNPEurCOf2Rxa5IdjZHgtjL_jQICfwa6-DRehYqrXOMYlzrixz-jDCEiNv5hVNw) *Unitary cases used for the superposition method* It is worth remembering that, under the effects of delayed deformation, concrete reacts with an apparent deformation modulus called relaxation modulus, which is lower than the corresponding creep modulus. If the classical ratio between the moduli of steel and concrete, including creep effects, is about 18, in the case of an imposed displacement, this ratio increases up to 24. This tends to make the adjustments by support elevation and actuators less efficient when the latter leads to imposing a deformation on the structure. From the point of view of FE simulations, the large number of intermediate states that need to be processed multiplies the risk of errors. The verifications must concern: - the respect of the boundary conditions in the intermediate phases; - the respect of the displacements fixed by the construction phases in the structure (for example, discontinuity of slope at the keying point). In construction studies, one must also remember that the actual creep of concrete can deviate strongly from the theoretical formulations. The model must therefore be constructed such that it is easily adaptable to restore the deformations appearing in the first phases, and thus improve the prediction of the following ones. # Chapter E. Typical post-treatment in Civil Engineering #### **Chapter E. Typical post-treatment in Civil Engineering** **Introduction** In civil engineering there is a great variety of quantities of interest because of the numerous subjects that can be studied: - The nature of the construction considered and its functionalities (for example the sealing of dams, water tanks, or nuclear power plants, crack opening, stress state, residual deformations, …) - The limit states considered (ultimate or serviceability, …) - The nature of loading (dynamic, static, delayed, …) - The constituent structural elements (reinforced concrete, prestressed concrete, steel, wood, masonry, …) Moreover, the quantities of interest may be directly or indirectly accessible when performing FE calculations. They can be obtained from primary results later processed to provide a given quantity of interest. The latter is then compared to some criterion or used as data for the next steps (reinforcement area, rebar orientation, …). The Eurocodes enables us to know the quantities that should be analyzed according to the various situations mentioned above. However, the way to obtain these values is not established in the codes and standards. This chapter highlights the maneuvers to access those quantities and the mistakes to avoid. **E.1 Generalities** [E.1 Generalities](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/e1-generalities "E1. Generalities") **E.2 The quantities of interest in dynamics** [E.2 Quantities of interest in dynamics](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/e2-quantities-in-dynamics "E2. Quantities in Dynamics") **E.3 The particularities of reinforced concrete** [E.3 Particularities of the reinforced concrete](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/e3-the-specific-case-of-reinforced-concrete "E3. The specific case of reinforced concrete") # E1. Generalities #### **E1. Generalities** The different post-treated quantities may change significantly according to the objective of the finite element analysis. Usually the studied quantities in the pre-dimensioning phase (a sketch or preliminary draft) are different from those searched in the pre-design and design phases. Other quantities of interest are needed when analyzing existing structures to quantify structural risks. It is tempting to consider: - Pre-dimensioning phases (sketch, preliminary draft, …): quantities such as displacements, deflection relative to the span, … - Dimensioning phase: density of reinforcement for slabs, reinforcement area for beams and columns, crack opening, … - Structural analysis: stress state (principal stresses in concrete: directions, signs, tri-axiality and its values, comparison with criteria such as Ottosen, Rankine, Drucker-Prager if the analysis is elastic), principal strains: directions, signs and its values, damage, stresses in the rebars, plastic strains, … It is important to keep in mind that not all quantities of interest are accessible for every type of element and constitutive models. The type of element determines the nature of the degrees of freedom: the nodes and moments on solid elements are not accessible. Analogously, a model simulating plasticity cannot provide damage results. These details may seem trivial, but they are often forgotten by the users, so it is important to mention it. 1. **Stresses and strains** As exposed in the [“Generalities” chapter](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/e1-generalities "E1. Generalities"), the stress and strain fields are not obtained directly when solving a mechanical problem with a FE solver. They are obtained from the displacements by computing the derivative of the interpolated displacement fields. Using the same notation as in the “Generalities” chapter: ![](https://lh6.googleusercontent.com/ok4J2I7wAXripcRr6mysRsZZV-ykdBBf8T2eTjKC2QedKYY3yUL9c72lgFqPgiEeqGLZi4UUL2FdK8ObQzfgLfNkq9m7Jo4_UhjWTX-uF893iD8mtjVkXgICTTel19iWrKK2QSZujphdsWUdSOKQYQ) In linear-elasticity, the strain-stress relation can be written as (H being Hooke’s matrix): ![](https://lh3.googleusercontent.com/kZTVtzfUWwQTrN1i5Qo_jZWjtxT4ZmRt6MeHSk4aPef58i7eUx4QL36wdKPDPeXLiscSbM5ICdSK9NqG3VAHP8cyKM_rEwCBMYf-sIDB-2APkNk0BDfYAu9Jh-X4J6QUSYVBKcoWHDWgi8NB0kHHpg) In this kind of procedure, the strain and stress fields evolve according to the interpolation functions of degree inferior to one of the displacement functions. For non-linear analyses, the stresses and strains cannot be obtained by simply multiplying Hooke’s matrix by the derivative of the nodal displacements. They are based on the values of the element at the Gauss points, and the shape functions are used to extrapolate the results to the rest of the element and nodes. This procedure allows the stresses to evolve according to the same degree as the interpolation functions and not their derivatives. As an example, on an element with n nodes, n_{pg} Gauss points located at the coordinates ξn_{pg} with shape functions N_{i}, we compute the least-square minimization between the interpolated field evaluated from the nodal values searched and the known Gaussian values. ![](https://lh3.googleusercontent.com/zxFn25nXMTNhjRAvy8JI9qhym780vHb1_FM_0La1EcI_xUSOy_lRQTfzfJBiBk2aF9blAWVgU1Q3uGlhMU7vBTMF9Up5wuyslvYYhvFHvan2tyXFscq6ZtVwFEzP3ikFgISD5QZAyi1zoz8TicM89g) *Building elementary nodal values starting from the values at the Gauss points in 1D* So, either it is a matter of minimizing the function: ![](https://lh5.googleusercontent.com/lzACvLS18o_riMk91boJu2g1cnpE4Wf9ExDt4ySdtjroilwf0_IiR5HrGFiMSzyh5IdnGG4mTSnzUfuWop9YFxSb7PoJJTLNg_kamovHfA9sS67QEwe1ckbijXe1TbXy15T2EMjVGHmJVDHiKoM3eg) Or for each node i among the n nodes of the element: ![](https://lh6.googleusercontent.com/jf7_DM4UxkMNtA45no3EuH9yxLhugAKmCIM904XjusJnHrfABQk2Ri-N3eng18a-QPi_GToVVkFQhtG6TEPvCCTg9jo-GayE9j_NAyzw2iM6DkMtbqUurvtVa3mW9ALvR9NaS_YInwO-pBwvfMyjAA) Which can be expressed in matrix form. The matrices are finally computed for all the isoparametric elements of reference: ![](https://lh3.googleusercontent.com/iFg8awEe2fg0vp-guJpYMrBFmfXNBlxlnaDCUR1qKMo-6__k18vVSVZqtNBOGNTE9YprzXJ6W3Yme28euT8-jsnngzwaodJ27v5IUeDa-gfOoE-CNcDtalLxlXDfs0Dpb5edIassq8K12l4E19xOow) And so, it is possible to directly obtain the nodal stresses: ![](https://lh3.googleusercontent.com/50rDzCJWAOrmEPsZqbQb-x54k8AaCc86q8PV1sQEeTTXbBQqy6WZAkFz9X2GGUP9Xj6MVYSIo6s4UTd_Gwzjq-lH663UIaxZMb0wCNVLSrtZEJK-doNx-fZbx4lyjUua0Ai6wD3XCUwRRiXF8rB7RQ) Thus, it is possible to have several nodal values of strains or stresses for a given node, shared by multiple elements. The other nodal values can be deduced from those values. ![](https://lh4.googleusercontent.com/1PRurebz9Ol2ZREblIxrEdnrslqi5JyuUUhbaWnqwoMzMbc1xP5pGY4hE8_CvKpYeZ-vwyDjRbwWF9YQLcWzwnw4GD6QAxxMlma-Io23vpx6e5eJRSZTCLo62Blk1L8m23VYH1PCfNE92Mr3ceoDuQ) *Discontinuity of the elementary nodal values in 1D* Several methods can be used to recover the continuity of strains or stresses (if the material is the same in the 2 adjacent elements) to have a single nodal value of strain (or stress). Those methods consist of smoothening the stress and strain fields by using certain algorithms on the totality of the structure (by least-square minimization). It can also be done by computing the average of the values on a given node shared by multiple elements as shown in the figure below. ![](https://lh3.googleusercontent.com/Ce0a3XSY7OowRI_M3XrELHLekbMJeTQpIYFXTITvuqP657_i7pwqVWfkwWGjlCZ5Kz1lVkLtfS3vWq8FYLeU8S-EwEABinseicebkCkfV_QKn0cjs5lAMRsniu3MVV02yMkc6jlAIsoom8ebQxbfHw) *Example of the calculation of an averaged nodal value starting from elementary nodal values in 1D* For convenience one might prefer obtaining smooth elementary values. However, when we look for precision, it is convenient to give priority to the values obtained at the Gauss points. 2. **Going from continuum mechanics to structural mechanics stresses** The automatic methods to compute reinforcement rely on algorithms that take into account combined axial forces and bending moments based on plate and shell torsors with 8 components, or deviated combined axial forces and bending moments based on beam torsors with 6 components. Some structures may need, for various reasons, to be modeled using solid finite elements (dam, structures such as prestressed tanks: liquefied natural gas tanks, retaining structures). To avoid computations based on 8-component torsors, it is necessary to rebuild the Structural Mechanics internal forces starting from the stress fields along the segment as shown in the figure below. ![](https://lh3.googleusercontent.com/ikIDIcol1IKHJ6evqu9FLtEQzkS-Q8sbmOIuLGdKDOkiSMwIK9fIPvwF__T2lUhG4t_DFMZbyYHXaCEzJbIcyh-1Up9uicLVT59SASZ9HsgE3xcqlsCtisrKFtu6O88km6NSwKceZGhhIK9DmBvT1A) *Segment along which the stresses are used as a reference to rebuilding a shell type torsor* We consider the stress tensor expressed along the segment shown in the previous figure: ![](https://lh4.googleusercontent.com/IGEcOTQ6z2g3WX9MJgH7mRDEq_Au-W33eK8cmXUHK1cXcQA1W_3e_jJbvFf0trB-__pZNQWuhCiKRSVneczqp8WHMLky-EAsmwra2r7fD2UQ94j1xwwKIGPj2trQHnSA6ncnGMLGzi0uBN7SRZYrJA) To be accurate, for thin plates satisfying the Kirchhoff-Love hypothesis, we consider the following torsor with 10 components that will be associated with the stresses according to the following equivalence principle: ![](https://lh6.googleusercontent.com/7i_i10MQtT7DDwRKdyjneo78BXweFlr5Ht4WHjnXKhva2O4v1WOcr0zVXEV5C6KZqoRZRigDGlHJqgQKMQaY8ABGoUjJot2CWzQeXgihGMMcfIWU2Ip6vPe0GMCKc5LxMLsmEoWPynVih4aw7fBSDA) This continuous integration is discrete along the segment and can typically be computed from the stress values expressed at the Gauss points or the nodes. Multiple integration techniques can be used (Trapezoidal rule, Gauss, Lobatto, etc …) A continuous expression will be kept for the sake of simplicity, even if it is not rigorous in the discrete context of the values obtained by the FE method. Taking into consideration the Cauchy theorem equivalent to the shear stresses at the adjacent faces, this torsor is reduced to 8 components: ![](https://lh5.googleusercontent.com/-GY8U5cV0_n-glJmrRZnvYQrfnb_gETKOTwQsxbMEbCvRu9rogZjxz_EndOM0vcD1NjkBAa2WR_2VsYino9igMHxWno7q9ThuXWJuP4sHhuQIi610UwmxCcE591wb63eZbub8wAhrbAde1tLdgUdZg) Considering that this plate is an isotropic slab implies that the contribution of membrane efforts is neglected. ![](https://lh5.googleusercontent.com/jRTUtjjT38q-NzSlT2MR7mwzLK5C3Z5CdYStRxg-B6LH2DWcYWtUKV3XN09nJ3PIjUlubGDTG-UN0NigCJ6wiXda3NbtdqTTZIjqWGEMCAe3vcLHP8e4RyK4WQdC6BQrHjS_O3LPxHv0RnB_YTsHVQ) Then, it becomes a 5 component torsor (considering that the notation M\_x represents the bending moment activating the rebars in the direction e\_x), which are the internal mechanical actions in a plate element: ![](https://lh5.googleusercontent.com/BXpLxjhKLD_qS3Ztl7M4-m3x9r8errHi24h5ID6Q8iRVD1wzHZOfP82AE_yOaQJcpRM6XbdmgEyC91xdyZhqB-F8kHdSqTEy-LurtYD1Q9V-XrUuW9DkmBUJ8zUDhguDpOsxNxcHFadyP0i0P0ckgA) (1) Shear efforts outside of the plane (z-direction) with x as the normal direction (2) Shear efforts outside of the plane (z-direction) with y as the normal direction (3) Bending moment activating the rebars in the x-direction (4) Bending moment activating the rebars in the y-direction (5) Torsion moment on the cross-section of the slab with x or y as the normal direction 3. **Section method: elementary reduction elements (EF) to beam-type structural reduction elements** Depending on the stress state it might be convenient to build a model of the whole structure with plate elements including the zones where these are not appropriate such as posts and lintels. In these zones, one must restore a beam-type torsor to take into consideration more accurately the local behavior, in particular, to estimate the required reinforcement. A widely used technique to solve this problem consists of “cutting” the structure fictively and estimating the efforts at the cross-section. This “cut” must be chosen wisely to respect the Euler-Bernoulli hypothesis stating that cross-sections must remain plane. It is usually the case for posts and lintels. ![](https://lh5.googleusercontent.com/tfu-Ody9N56lWiWmlE06gvRSqv8iSpsGAnaxYgX8YZcw4EXcXAwKr_qNUwtIwmUYhhr_h2lPI1LM8z7wWtxPUy9yekQ7mBm4FssjiX08CMM6JKYuLOLi_amuMqKN7YLpLlKEqbUHOUj1sb11r4N6WQ) *Example of cross-sections in a lintel or post passing or not through nodes* We then build in the local coordinate system of the cross-section the beam-type reduction elements substituting the shell-type reduction elements. The latter can be the efforts at the nodes or evaluated at any point of the element coinciding with the section line and analyzed utilizing elementary form functions. For the example illustrated above, it can be written for the cutting line, where local and global coordinate systems coincide, that: ![](https://lh3.googleusercontent.com/_LTA1SAuYvEVTm4B8FRUwiJ9yPzN3mV74SlME2HVunGGwh0iBGeWaB3iEAPlwyeaiM47H8Fsr7MYvNLrJ3W2iLPOOkO7UiHI9c0e3azegmj3wrIQ4t7ko21P7gYxmxb5FuDAVA9DXG4UUUrc3aAWXQ) (1) Axial forces at the cross-section of the associated beam, i.e. the “cut plane” (2) Shear forces on the plane (3) Shear forces off the plane (4) Bending moment on the plane (5) Bending moment off the plane (6) Torsion moment # E2. Quantities in Dynamics #### **E2. Quantities in Dynamics** 1. **Time-dependent analyses** Post-processing of time-dependent quantities does not present any major difficulty as long as one is not interested in targeting a precise instant or in characterizing a single representative value at all times of the analysis. For cases where the loading is controlled and not random, a single analysis may be enough. If it is preferred to extract a scalar quantity representative at all times of the analysis, the choice of the standard is the responsibility of the engineer who analyses the results, and it must be justified. A statistical characterization may also be relevant (typically expressed as a percentage). If the engineer is interested in extracting a set of quantities constituting a vector, the problem of the concomitance of the normalized quantities (absolute, maximum, minimum values, etc.) arises. The time t at which a bending moment is maximal in a point for a torsor does not necessarily coincide with the point of maximal shear stress. When the loading has a random character, it is important to multiply the number of calculation cases by integrating the random character of the loading. As an example, if we consider N cases of calculations and we construct for a quantity of interest g_{i}(t) the corresponding dimensioning value G_{i} for a case i (it can be the maximum positive value and also the maximum negative value to then incorporate them into an approach of actions concomitance). We consider: - The used dimensioning value, which could be: ![](https://lh3.googleusercontent.com/uHq1OJZZgMpE6H9REp9Zpti3hTTbrzf1tMH0q5DyLq9a3zJRKs7telmVgQFoTRtQYCl_2GozAXPgSt1nwzz_Oacq1es42ogefhuymln4MY_AZK8nLLxws5sKboj2QmtIiLW4K15M8__uJz5sWwTDRg) - Its average: ![](https://lh4.googleusercontent.com/vN_ateSR0AE_HeGFGbOEIIEUD4lNphRmztv9H_lnfO_RWhaDQOqfoZnm-8qV6an1VotJ-lh8dmsuqDwaxB14mlENZaaAVn52IkGYlFCwTLXuAFAsu4tHOjrnBkg3JrHCKtfK4BC-IXWiwehwxEMF5Q) - Its standard deviation: ![](https://lh5.googleusercontent.com/moK5TnpMudIm87Y3mB73-DtK0p-6nqzUHofAoBWyv03FQveU72vGLjKwIPX-KYgEXacl4PS_ORKXk2vT783OVWsYOjnDyBxUlQsevLtyGMk4yGKWwardVk0wMBHyGVdhSvPfbmrMQPb8Url_7h1RJQ) - The estimation of the mean value of G for the N results: ![](https://lh3.googleusercontent.com/uFsH0MdDXgnjQtSI2T13-PaDKC6cdFuhnaC-tg466dTFWDkD2HmSv0p2Dk7yklZk9um9Ai-KnuiOhHAJHG7kRKDLkGeKXaU2E_85GbiEoZZwvlHlSfPTqwrNLi_TWSuZNIe8e8px7PtgOAIkfxe6JQ) With λ(N) calculated from the Student variable for N samples (calculation cases) for a 95% confidence level (one-tailed) such that: ![](https://lh3.googleusercontent.com/WgX1FbqiGAr2xUKI1t0-cLnksBql1bUUcC4BPBROTG3TyA6LxMm_FCOBcGTP9yZhN8W0fCdTutW_VCc6YAKW1G_t0CpW8EjVe3pCEyMz2WuSnid8KK1WzRp3tlNH-h98QolMxHlJMjAfoJ4QTpOe2g) The table below provides estimations of the mean for various calculation cases. ![](https://lh4.googleusercontent.com/BAa1qDvQBHY8cRjoOin6lk9r4bXFciue-kniuTyWu2nkvzKZ43LY9Fv-KIcLemjiCQVf7yWUKM2XMcj0qwMV1JZdwO_SXqxILctTMzIXN9CS4zs9q0uNQ9FW_P9EK69S8wGa1s5d9NiRYhBzbFs2cw) 2. **Seismic spectral analysis** The seismic spectral analyses provide representative quantities of the average of an extremum or period. The purpose of this paragraph is to draw the reader's attention towards important precautions that must be taken to avoid making significant errors in the calculation of the results coming from a quadratic accumulation. As mentioned in the dynamic chapter, it is possible to quadratically cumulate simply or completely the spectral responses of each mode. The result of these cumulations is a positive value. It is important to consider that any operation that one wishes to perform on a quantity of interest that is the subject of a quadratic cumulation (simple or complete) of the spectral responses of each mode must be performed before the cumulation. Let us take a simple illustration with the difference between the displacement of two nodes A and B cumulated simply on modes 1 and 2 (an illustration with a CQC combination would just be more troublesome to write using cross-terms): Strictly speaking, the difference evoked as an example can be written: ![](https://lh3.googleusercontent.com/dzHLznlFS2TXCZs0PX3M8ImFGuhY62YI3j6jXcYXA6tNbDXm2NHDB43X-FYlh_fy4QpvqEZ_s2BZvIfUAPXXF6pA9_FedGMNRaTQYW2yTJFZiPBtlHVboaV3lxN6jAKG67JZejGjnqoXGfNgsfFydA) Therefore, it is obvious that estimating the difference afterward is largely erroneous: ![](https://lh3.googleusercontent.com/QG5hJYoDb1oi1_YmCUiW49jN2SPLc51Prmm1xCKHbnTnjF-9kZy_26L3VhBDHa-1bUFNfH3SegDqlkUujgC22NdoqrN5Z-F-UZcNHsUaDQWTYzmgyJf8-_mTLXAHM87BP03n8CkqrU1lXeo0id4_3A) The first value is always positive, but it integrates algebraic differences of quantities in the same mode. The second expression might lead to a drastic underestimation of an extremum response. It can also be demonstrated by using the Cauchy-Schwartz inequality that the first estimate is the upper bound of the absolute value of the erroneous calculation presented in the second formula. A more complex illustration can also be used with the estimation of a von Mises stress based on the main stresses for 2 modes : ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-10/DexXt6MQDS8zjv7n-embedded-image-lcgcfex9.png) An ‘a posteriori’ estimation of the accumulation of the von Mises stresses is largely erroneous: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-10/BjRUuT1N6xXKm44a-embedded-image-i75apiwu.png) **Example of a specific application**: estimation of the opening of a joint between two buildings In seismic engineering, it is necessary to estimate the opening of a joint between two buildings under seismic conditions to ensure that there is no risk of collision. The accepted practice is to independently calculate the extreme values of displacement of the envelope of each building based on a quadratic accumulation and then to evaluate the maximum opening of the joint by calculating the difference between these two positive values. Thus, an unfavorable phase opposition of the maximum responses considered. # E3. The specific case of reinforced concrete #### **E3. The specific case of reinforced concrete** 1. **Overview of the common methods for designing the reinforcement of plate elements** There are mainly 3 methodologies applicable to plates that can be consulted using the following references: - *Johansen fracture line method*: - Save M.A., Massonet C.E., De Saxcé G. - Plastic limit analysis of plates, shells and disks, Applied Mathematics and Mechanics Vol. 43. - This method applies to weakly reinforced plates (reinforcement ratio less than 0.7%), allowing the appearance of fracture lines to be evaluated and the use of the reinforcement opposing those fracture lines. - *Sandwich method*: - Marti, P., Design of concrete slabs for transverse shear, ACI Structural Journal, Vol. 87, pages 180 to 190. - This method intrinsically considers the behavior of plates, it can be found in annexes LL and MM of Eurocode 2 part 2, - *Method of Capra and Maury*: - Calcul automatique du ferraillage optimal des plaques et coques en béton armé, Annales de l'Institut Technique du Bâtiment et des Travaux Publics, n°367, December 1978, - This method is based on the equilibrium of the cross-section in combined bending and axial forces, it is detailed in the following section. 2. **Example of the Capra-Maury method** A set of facets is defined, centered at the point of computation of the finite element code. This can be a node, a Gauss point, or any point where forces are interpolated. Its normal vector rotates from this point in the plane tangent to the mean sheet. The facet is marked by the angle θ between the OX axis and the normal vector of the element in its local coordinate system (see figure 2.1-a). The angle θ is discretized regularly from -90º to +90º (here with a step of 5º). The Ox and Oy axes are the axes of the reinforcement layers. ![](https://lh5.googleusercontent.com/Bv45oixHAqBykNMCQ4NnC5qlrsFvZFORmt_-YNNjRExovNCxBMet3p8IeJNKZYvMWnkZpoEEHjOvN_SYSTfcSNf4Y89JQCaplUGPDXUlhBUMW7y7g0k3VQUmF50cbOkrpOMTWyzcaQgo0Ao5_MPJ5A) *Reference facet parallel to the beam’s cross-section in equilibrium subjected to combined bending and axial force* For each of these facets, the bending moment (M), the membrane force (N), and the shear force (V) are applied as a function of the effort tensors using the following equations: ![](https://lh5.googleusercontent.com/nWE9BgzAXjaTXFWNutw6m-wiPFKxaVZTFxVXwcyxfSnQYZQsHLXbYPIn5vhRFh0iMhY5bM_U_n5DJb-rSZt1oKEEcb02CVQ7ZMcGeVk8TfErvs4YX70lnRkfzYFHZCyFVUL8LM8GIlh2FM2SP_FJAA) By using combined bending calculations, it is possible to determine the reinforcement area in upper and lower layers A_{S}(θ) and A_{I}(θ) required in the θ direction to reach equilibrium in the chosen reinforcement concrete section. The compressive strengths in the θ direction of the two reinforcement layers can be evaluated using the following expressions: ![](https://lh3.googleusercontent.com/WYSb31MoLONokyRzVXIQ6OLyigCXlQSZXcUgeHQstnyLvaIEdtK2v9ntI7NdrzXvqAvMDCdd9ULQ1--gf9faPRAZIeH1rfG9tBXn-hx3nuB3VmRpq6_IMLJtwXDqKgh-DBWDrciJNJC1QeCylZLhhw) where f_{yd} is the maximum allowable stress of the steel (identical in both directions). The strength is ensured if the resistive force is greater than the applied force, which is expressed as: ![](https://lh5.googleusercontent.com/4LwDsHHo9BtjuqCFLhv3dhkzKkzMQi1gFveyvviDh-a8aeUpnD1LpmTnGnivH-nYwGdhrbbJ0cxG_Wd7c2g0IDdVmNAnuPlywSNkBGb2wrx1__GSl8MF7UY2rpcwy_L814b1nOu4I4AaKj_C45uZyQ) Thus, by considering an orthonormal coordinate system with AXS on the abscissa and AYS on the ordinate, one can finally solve for the upper and lower reinforcement: ![](https://lh6.googleusercontent.com/aAO2Qdz0na53gw2xyPsINrCGq6n4-9cOngQThTBHaIjsMxEUciHaaeWEYO06zKAMAV2DAPoene544EGpXv5dxR0nuVcsmj0W_PbdGD5XQpHvFjzIQT4qc8cInM5lJ9dH8UWxcrOKWhciOpLjHPCDrQ) for all angles θ ![](https://lh4.googleusercontent.com/ukN59GrrsegsjuyLD3guV_WDUqVJVLSaHiBMmVN9opZq7P3WkQmbhIQ5oGB8zH9_gsJYDn2AHYpD5Nu_KsrwET9jL1rPFSCXle44ZTihEZ-kH-Z1agxpXL1tuqbLk6y8Mt4bV6gUfxQe7LyfhsGStQ) for all angles θ and ![](https://lh6.googleusercontent.com/nntpk_gvGhuh_-NyCUy0BFuE1tAkBUdO9PsBaim4wYY5mCwxbB0XSnK9c2laLHeD9Dj0C0GbgsjFCLj5v8Fpnwsq7ixwSX2PUjD20hwL_6WQgFU4UptveCEMzVTNHqZNw19ppyqWz3eXbruQaBa9_g) and ![](https://lh4.googleusercontent.com/fs4VhK79SHFiAB4oAtZNqwk5PvmPM68Br6NYoLWvKQ-uEaRHQ6f68pY8xapX55QiuE7KWMFB4TJoD-aticThn6Q6M9urkBI0_OJoEYJqw5IPrzqSSCKdIBT5kUywh2AW2l9aZgtdfJVhUStN0nkwFQ) minimum. The resistance inequalities define for each θ a half-space limited by a straight line with negative slopes that reflects a validity domain, as shown in the following figure. ![](https://lh5.googleusercontent.com/-lHJ38ZtJUB_0XMOP8N87DZM4FhDiwDi3K3uCrOvjgVuunoLLZzHpMJ8jIRlCgQPsdLOoPZo9nYkGDnNK2k2EbU4peXtmm6_LoqBOZPv5E-ElFbAByC8HnPZTDmqVULozbq4MoNz5cs_eDQLpOyQPw) *Resistance domain for a facet θ* By browsing through all the values of θ, one can obtain the validity domain shown in the following figure, delimited by the line ABCD. ![](https://lh3.googleusercontent.com/4aVGkecTWa3BhcV0Lpv1nnd7p6aMaRsG4sxkM2eyEN4995fUmUl8sNWCUHPU89hakpBgdT9TxcNgxMeTSc8mEOg39plh5DMxJaT51eRpAxY5sivyZjFsqe79AJrCmjKGInAKRd9LyUzpfDgZiTYiCw) *Resistance domain for all facets* For each point P in the validity domain, the total area of reinforcement can be obtained by projecting the point P in Q onto the first bisector. The distance OQ then represents the value ![](https://lh6.googleusercontent.com/QWjDHhEpdY_RN9Mg1JQWLADaliL1iwxxxEL3i3HqQW85Q0FoRLRJE_CQKAbgrGWsW_16hKZiQyVUbnDrg3JQ7Etnt92FNSSEp2o4UM3CxnKIA_fCgmxLXqG6xhRrq92lrElQrdvnbFFcQD9bn_6vqg) with A_{S} = A_{XS} + A_{YS}. Therefore, it can be noticed that the optimum reinforcement corresponds to one of the 36 points (considering the facet rotation step chosen if one facet is taken every 10 degrees for example) of the boundary (illustrated by the 4 points of the line ABCD ...) whose projection on the first bisector is closest to the origin of the axes. Researching this point can be done using "dichotomy" type methods. 3. **Connecting rod and tie-rod methods based on a finite element calculation result** In the presence of structural elements subjected to important point loads or presenting abrupt modifications of their section and geometry, the classical plane section methods of analysis are not satisfactory. These locations are generally reinforced using good practice rules based on experience or empirical guidelines. The strut and tie method (STM) is a rational design procedure for complex structural elements. The procedure is based on mechanics but is simple enough to be easily applied in design. In general, the STM involves the idealization of a complex structural element into a simple structure capable of representing the path of stresses within the element. The truss model consists of struts representing the compression fields in the concrete, ties representing the elastic steel reinforcement, and nodes representing the localized areas where the components interconnect or the areas where the elastic steel is anchored in the concrete. The struts and ties can carry only uniaxial forces. This mechanism must be stable and maintain the equilibrium with the applied loads. The failure of the structure is dictated by the failure of one or more ties or by excessive compressive stresses within the struts or nodes. Ideally, only the first mode of failure should occur. ![](https://lh5.googleusercontent.com/rmAkBb4if6QxSa4UlqZ9_-0i5XLJ-O1mQGg52_MAuMcvzpPaew_mgeuxe7EWvqopacFxKulCUcH-s2Geldv9C5OdzU0FwF62O_OjRLM382-edQwj1fX9ZS6tV5UhoMyZzYav9yjwokc5g9sWjMofvw) *Example of D region and system modeling to obtain stress fields and then loads at the ST truss supports* This method is applied to the so-called D regions. To characterize these regions, the distribution of deformations over the depth of the element is considered to be non-linear. Consequently, the underlying hypotheses about the cross-section procedure are not valid. The principle of equivalence cannot be applied here. According to Saint Venant's principle, an elastic stress analysis indicates that stresses due to axial forces and bending moments come near a linear distribution at a distance approximately equal to the depth of the element, h, away from the discontinuities. In other words, a non-linear stress distribution exists in the depth of a member from the location where the discontinuity is introduced. Then, it can be stated that the D regions are assumed to extend to a distance h from the applied load and support reactions. In general, a region of a structural member is assumed to be dominated by a non-linear profile, or a D region, when the ratio extent/depth (a / h) is smaller than 2 or 2.5. The shear extent (a) is defined as the distance between the applied load and the nearest support in simple elements. The approach consisting in defining a strut-and-tie truss can be summarized in Figure 10. ![](https://lh4.googleusercontent.com/60ozk59J9auQodU2uTi2udJYoouFSnSHnu2uLIB6TREaMvfBc5xLGli8J6AsPk5KUKIp04_6GKDJrYp2TQ5e9YYPqRhfeYISa843q6ROByKrpnTcoRaXWyitoP_vi8CLRReCauHegvnVJ9BPw5VmpQ) *The general principle of design by STM* The verification methods are expressed in Eurocode 2 part 1-1. The approach presented in Figure 10 is difficult to implement and depends strongly on the engineer who implements it. More and more approaches are being developed to automate this procedure. In France, the algorithm with code\_aster elements integrates a CALC\_BT operator that renders the procedure semi-automatic based on: - an analysis of the local peak fields of the major and minor main stress fields, - a cutout of the D region modeled by Voronoi paving, - the projection of the mean directions of the main stresses in the Voronoi paving stones. - a set of optimization processes. ![](https://lh3.googleusercontent.com/CzE-1kFNA6y_R5CHLsMg0C6IfAXIyaMZ1I4R1O07qhz-lJU_Ru-BjNBc_GzSJsswh69co6mPf1Q2LTr9u1x7C-zX8Dt6VXvoDsPdTIeRn2j4tZulupoFp_Fd1DalLBKQAHcgl9tytaSOhzFzfKGfqQ) *Reference example on the left - Solution obtained automatically by the CALC\_BT operator of code\_aster* This method requires a high level of experience and knowledge of the field. # Chapter F – Geotechnical calculations #### **Chapter F – Geotechnical calculations** **Introduction** Conventional methods for the design and dimensioning of geotechnical structures mainly aim to analyze the resistance to failure of an isolated structure. These analytical or semi-analytical methods only consider very simple geometries and provide little or no information on the ground deformations surrounding the structures. The increasingly intensive use of urban spaces and soils, occupied by a variety of structures close to each other, makes it necessary to control the interactions between structures. The designer of a structure must justify that the displacements induced by its construction remain below the threshold set by the client. Traditional methods do not meet this requirement, which explains the increasingly frequent use of numerical modeling and software dedicated to geotechnics that are adapted to design offices. Specifically, digital modeling is used in two different situations: - during the design phase, to justify the dimensions when traditional methods are difficult or impossible to implement, - as an expertise tool, to study the behavior of a damaged structure, to identify the phenomena responsible for a specific issue, and to justify the use of a strengthening method. Depending on the case, models with various levels of complexity can be used, considering the uncertainty of the natural soil's behavior and their spatial variability. Consequently, it becomes difficult to choose a constitutive law and determine its parameters. The user often has to choose between a robust model whose operation is well understood, but which does not account for all the complexity of soil behavior and a model that is potentially more accurate to describe the actual behavior of soils, but which includes many parameters whose roles are sometimes difficult to identify and quantify. The philosophy behind the design rules promotes the first approach, to use simple and robust models and ensure the safety of the design by inputting appropriate factors and carrying out parametric studies to estimate the sensitivity of the results with respect to the said parameters. However, this approach may lead to an oversimplification of the problem and can lead to overly conservative and unnecessarily costly designs. The other approach is to use constitutive models that attempt to better represent different aspects of soil behavior. A very large number of models have been proposed, but their practical use remains difficult. Furthermore, the idea of having one "universal" model that describes all phenomena is an illusion and should be abandoned. It is necessary to define the limits of the model chosen: a perfectly plastic elastic model or one considering isotropic strain-hardening, even with a complex load surface and strain-hardening law, cannot predict a progressive accumulation of deformation in a soil mass. Therefore, the use of finite elements requires the user to have a critical perspective on the soil constitutive model. Though, this is not the only aspect to consider: the result of the calculations can depend essentially on the 3D geometry of the structure and the geometry of the soil layers. It is sometimes (not always) justified to simplify the representation of the soil behavior and to focus on the representation of the construction process. In any case, the results of numerical simulations should be carefully verified. Finally, it is clear that geotechnical structures are made of soil, in contact with soil, or totally or partially buried; thus, numerical modeling must represent the mechanical interaction between the soil and the structure. This chapter is organized as follows: it summarizes the main features of numerical calculations in geotechnics before briefly presenting the verification principles adopted in Eurocode 7. Once these elements are presented, recommendations are suggested for good practice using FE calculations in geotechnics. It also deals with the features of dynamic calculations. **F.1 Geometrical aspects** [F.1 Geometric aspects](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/f1-geometric-aspects "F1. Geometric aspects") **F.2 Material non-linearities** [F.2 Material non-linearities](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/f2-material-non-linearities "F2. Material non-linearities ") **F.3 Soil-structure interactions** [F.3 Soil-structure interactions](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/f3-soil-structure-interactions "F3. Soil-structure interactions") **F.4 Hydraulic effects** [F.4 Hydraulic effects](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/f4-hydraulic-effects "F4. Hydraulic effects") **F.5 Uncertainties and recommendations** [F.5 Uncertainties and recommendations](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/f5-uncertainties-and-recommendations "F5. Uncertainties and recommendations") **F.6 Normative aspects: Principles of Eurocode 7** [F.6 Normative aspects: Principles of Eurocode 7](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/f6-normative-aspects-principles-of-the-eurocode-7 "F6. Normative aspects: Principles of the Eurocode 7") **F.7 Dynamic modeling** [F.7 Dynamic modeling](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/f7-modeling-in-dynamics "F7. Modeling in Dynamics") **F.8 Characteristic scales** [F.8 Characteristic scales](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/f8-characteristic-scales "F8. Characteristic scales") **Conclusions and references** This chapter presents an overview of the issues raised specifically by FE calculations in geotechnics, in statics or dynamics. Specific precautions should be taken when performing the calculations concerning the meshing, boundary conditions, phasing, the choice of constitutive models, and the setting of parameters. With a certain amount of practice and the constant concern to control the obtained results, a wide range of problems and structures can be dealt with. However, there are still situations that are difficult and/or costly to deal with numerically. Firstly, difficulties may arise due to the ambiguous mathematical structure of the studied problems. In dynamics, choosing a time discretization coherent with all the input data remains difficult. In statics, managing several non-linearities of different natures (unilateral contact, damage) may lead to numerical issues hard to overcome. One should also remember that the physics of certain phenomena remain poorly understood and described, which is reflected in the numerical analysis. It is the case for various problems such as the initiation and evolution of landslides, implementation conditions of tasks such as the compaction of backfill materials, the initial state of stresses, water content, and other parameters linked to the history of the structural elements, etc. # F1. Geometric aspects #### **F1. Geometric aspects** One of the advantages of the FE method is the possibility of describing the exact geometry of the structures even during the various construction phases. CAD-like pre-processing tools make it easy to generate very complex geometries. One of the features of geotechnical structures is that, generally, the earth mass that constitutes or surrounds the structure must be considered within the mesh. 1. **Boundaries of the studied domain** The first challenge is to identify the boundaries of the domain considered for the analysis. For a geotechnical structure, the horizontal and the lower boundaries of the studied domain are rarely determined with precision: the extent of the domain is then bounded by vertical planes whose position is generally fixed by using empirical rules. Using the plane strain assumption, for example, the position at which the lower limit of the mesh is set has a direct impact on the calculated settlement for a strip footing or above a tunnel. This relation is clear in the case of a homogeneous linear elastic soil mass. It can be reduced by taking into account elastic moduli, which increases with depth. Nevertheless, it is likely to induce a significant error in the calculated displacements. The ideal case is when a rigid bedrock has been found at a given depth, which assumes that the research has been carried out to a sufficient depth. To model a tunnel, for instance, it is advised to collect soil sampling way beyond the depth of the shaft, which is generally not the case in real projects. In the lateral directions, considering a domain that is too small can also significantly modify the response of the numerical model. Fixed displacements lead to an overestimation of the stiffness of the solid, and "smooth contact" type conditions lead to an overestimation of the displacements. The choice of the mesh dimensions adapted to a structure remains a largely open problem even if some authors have suggested practical rules. However, those rules should not be taken as absolute prescriptions (see Mestat and Prat, 1999). Consequently, choosing the size of the domain considered for the mesh is an important step in the modeling of geotechnical structures, even for relatively simple static analyses. In the case of dynamic calculations, the question of the size of the meshing domain raises specific issues and is a crucial part of the modeling strategy. This will be detailed in section 8. 2. **Soil heterogeneities** In some regions, such as London or Frankfurt, geology allows the soil in the vicinity of the structure to be considered homogeneous (in the sense that its mechanical and hydraulic behaviors can be represented by a single model). However, in other contexts, particularly in the Paris region, it is common for the studied area to include several layers of soil of very different natures and characteristics (particularly mechanical). Therefore, the elaboration of a computational model begins, as for traditional methods, with a detailed study of the soil layers in the area of interest. The goal is not to reproduce the exact geometry of the geological layers (which may be locally thin), but to define geotechnically homogeneous sets. 3. **Discontinuities** An important particularity of geotechnical calculations is the presence, within the solid, of failure planes that existed before the construction of the structure or the implementation of the studied load. They produce a discontinuity of displacement between the blocks located on either side of the failure plane. The FE method is well adapted to search for continuous displacement fields, and the consideration of this type of discontinuities requires the implementation of special techniques (specific elements are generally used) or even the use of another calculation method such as the discrete element method. Behaviors such as landslides are extremely complicated to predict. Nowadays, it is extremely difficult to predict the occurrence and development of failure planes. Usually, the engineer is forced to consider an existing plane whose position has been identified with more or less precision using the adapted equipment (for example, inclinometers that follow the deformation of a slope). Solid rocks often contain a large number of fractures with directions that are seemingly parallel to one or two main directions (local diaclases). The fracture distribution is diffuse, and random, or at least impossible to characterize completely at the scale of the solid. If the global behavior of the solid is of interest, it can be modeled as a continuous medium employing a constitutive model, which incorporates, at the calculation scale, the effects of the discontinuities: homogenization methods are generally used. One may also have to consider large discontinuities in a solid bedrock (fractures), which can be treated as the failure planes of landslides. 4. **An "open" material system and construction techniques to be modeled** As stated in the introductory chapter, a peculiarity of civil engineering calculations is the need to consider construction phases such as clearing or backfilling, implementing a concrete mass, tensioning cables, etc. Taking these construction phases into account within the framework of the FE method can be a lengthy and complicated process: the method consists of reducing the problem to the calculation of a stiffness matrix, a vector of nodal forces, then solving the system obtained by considering the boundary conditions. To model the construction phases, one must perform a series of calculations taking into account the change in stiffness of some elements, disappearance or modification of some supports, changes in the point of application of the loads, etc. Therefore, the issue is to propose simulation techniques that can take into account a large number of constructive arrangements within the relatively narrow framework of the FE method. It is up to the user to decide whether the modeling tools proposed by the software correctly reflect the phenomena involved. In the case of tunnels dug by TBM, the stresses applied onto the ground during the various digging phases are complex as the soil is closing in on the ring formed by the segments as the TBM advances. Pile driving is another example, which is difficult to simplify to the FE method framework. # F2. Material non-linearities #### **F2. Material non-linearities** In geotechnics, it is very rare to be able to study a structure exclusively using linear behavior assumptions (except for certain dynamic analyses). It may be useful to first perform a linear calculation, to check that the geometry and boundary conditions are correct and get a preliminary idea of the deformation that the loading may cause. Nevertheless, the results should be put in perspective as they can be completely wrong in some cases: for an excavation in front of a cast wall for example, the kinematics calculated with linear behavior are clearly different from the one observed. 1. **Constitutive laws** Even when limited to cases that are perfectly saturated or perfectly dry, the behavior of soils is complex. In practice, elastoplastic models are most often used, which give a force-displacement relationship that is non-linear but independent of time. The effects of creep and viscosity can be considered for particular applications when required - and if the corresponding parameters can be obtained experimentally - but the use of such models remains limited. Among the elastoplastic models, perfectly plastic linear elastic models are still most often used (see the survey cited by Gilleron, 2016). The use of non-linear elastic models associated with one or more plastic collapsible mechanisms is gradually becoming widespread, particularly under the influence of software developers: in some cases, they give results that are much more representative of reality (for example, for excavation in front of a molded wall), but the influence of each parameter of the models is not necessarily well controlled. Generally, the choice of a constitutive model for soils must consider the objectives set for the calculation, the type of structure (and the type of stress to which the soil will be subjected), the level of precision of the available reconnaissance and laboratory tests. 2. **Initial state** For non-linear models, the stiffness of the material depends on the initial state of the stresses in the studied soil mass (and possibly other parameters, such as strain-hardening or damage). Therefore, the determination of the initial stresses has a decisive influence on the results. Unfortunately, the initial stresses are generally evaluated in a very simple way: they are either assimilated to a "geostatic" stress field (for a solid with a horizontal surface), or obtained by applying gravity to the whole mesh from a state of zero stress. These processes are relatively poor compared to the complexity of the rheological models used for soils. However, they remain unavoidable in practice, for lack of a better way of estimating initial stresses in the soil. # F3. Soil-structure interactions #### **F3. Soil-structure interactions** Geotechnical structures often combine layers of soil with metal or concrete structures, which are generally much stiffer than soil. The interaction may be limited to a few points where the structure rests on the ground, or it may be continuous over a significant surface, such as the top surface of a tunnel, or retaining wall. The interaction will be treated more or less precisely depending on the case. In the case of tunnels, for example, it is very common to consider a perfect bond between the ground and the vault because of the construction method: with traditional (sequential) methods, the retaining wall is made of concrete sprayed directly on the surface of the ground uncovered by the excavation, which in principle ensures good continuity of movement. During tunneling performed by a TBM, efforts are made to ensure good force transmission between the ground and the segments by carrying out backfilling injections into the space between the arch and the ground. However, in older tunnels, the pathologies observed (or the tests carried out in situ) may suggest that contact is locally lost between the vault and the ground. For instance, it can be due to water seepage that may have washed out the ground: the modeling must then describe more precisely the contact conditions between the ground and the vault. Covered trench tunnels present a different problem, as the ground around the structure is backfilled. The modeling of this operation may require explicit consideration, using specific elements, of the interface between the vault and the ground. It is also common to introduce explicit modeling of the interface between the soil and the structure for retaining structures, when backfilling behind a wall (the phenomenon of soil sliding at the interface with the structure being similar to that involved in covered trenches), or when excavating in front of a cast wall, for example, the mass of soil supported may slide and present a vertical displacement greater than the height of the wall. The question of modeling an interface between soils and structures must be considered on a case-by-case basis. One can introduce contact or interface elements specifically intended to represent the mechanical interaction between the two, but these elements introduce new parameters, which can be difficult to identify (such as the normal and tangential stiffnesses of the interface). This modeling approach presents a risk: the interface elements tend to control the behavior of the structure and to blur the role of the soil behavior, giving the impression that the response of the structure hardly depends on the soil anymore. **Reinforced structures** In many cases, the soil is reinforced by inclusions with very high stiffness and strength characteristics. These inclusions are discreetly distributed in the soil and very slender: piles, micro piles, tie rods, wall reinforcement in reinforced soil. This geometrical particularity poses various difficulties. First of all, strictly speaking, a row of piles is not equivalent to a continuous wall, and the use of plane strain assumption is not justified. In practice, one would adopt, for the planar calculations of the wall, mechanical characteristics "equivalent" to those of a row of piles, using assumptions that can be more or less difficult to justify. The same applies to the parameters of the mechanical interface between the soil and the piles/wall. The difficulty is the same if the wall is represented by surface elements or by linear beam-type elements. To overcome this difficulty, 3D modeling can be used. However, because of the dimensions of the cross-section of the inclusions, whenever there are more than a few units, it becomes impossible to represent in the mesh the real geometry of the inclusions: for a reinforced earth wall, with reinforcements of 5 mm x 45 mm section, at a rate of 4 to 6 reinforcements per 0.75 m x 0.75 m, and for a volume whose dimensions are of the order of ten meters, the number of nodes of a mesh that would respect the real geometry of the inclusions and that would give an acceptable discretization exceeds the current calculation capacities. We can therefore propose to represent the inclusions by 1D elements (with or without considering bending effects). This approach is questionable from a theoretical point of view because the introduction of a linear density of force exerted by the inclusion in a 3D medium is not compatible with the classical representation of internal forces by a stress tensor. It can be used, however, one must be careful in the interpretation of the results, at least with respect to the stresses in the vicinity of the inclusions. An alternative solution is to adopt homogenization-type approaches to take into account the influence of inclusions on the overall behavior of the structure. More or less complex models have been developed and implemented in some software. Whatever the choices made (calculation in plane strains or in 3D condition, discretization of inclusions - by linear or non-linear elements - or homogenized approach), it is necessary to represent the mechanical interaction between the pile and the soil that occurs at the contact between the soil and the sidewall of the pile, and also between the soil and the footing of the pile. Modeling the mechanical interaction at the footing of the pile is particularly difficult to master. Modeling a single pile by volume elements, possibly with interface elements with the surrounding soil, gives results that depend on the mesh and the constitutive model used for the soil. It is necessary to use a model that reproduces the soil failure in compression if one is interested in the pile failure. For instance, models such as Mohr-Coulomb or Drucker Prager are not suitable in this context. In some 2D or 3D models where inclusions are represented by bar or beam elements, a fictitious end (e.g. a horizontal beam element perpendicular to the pile) is associated with the inclusion, in an attempt to better represent the interaction at the footing of the pile: performing studies to determine the sensitivity of the results to the dimension of the added elements seems appropriate to verify the relevance of this approach. Finally, other modeling techniques are available, which propose to explicitly integrate an interaction model for lateral friction and another one for peak interaction via ad hoc elements. Without going more into detail, let us highlight the fact that the user is free to choose between numerical simulation techniques and models, which have a direct influence on the obtained results. # F4. Hydraulic effects #### **F4. Hydraulic effects** 1. **Hydromechanical coupling** Another peculiarity of geotechnical calculations concerns the role of water in soils. When a mechanical load is rapidly applied to a saturated layer of soil, instantaneous deformation, and pressurization of the fluid in the vicinity of the applied load occurs. Depending on the hydraulic boundary conditions, the gradient of the hydraulic load causes the fluid to be set in motion, leading to pressure redistribution and delayed deformation of the soil. Therefore, a problem of hydromechanical coupling must be dealt with. A solid theoretical framework was established by Biot (1941) and developed by Coussy (1991). In terms of numerical resolution, the coupled problem is much more difficult to deal with than a classical problem, for several reasons: - the problem involves, in addition to displacements, a new unknown field, the water pressure field, - it is necessary to specify boundary conditions specific to the hydraulic problem (define the parts of the contour that are impermeable and those where pressure is imposed), - the solution (in displacement and pressure) is time-dependent, - the mathematical nature of the problem to be solved is different, - the permeability of the different soil layers must be described quantitatively. Complete processing of the hydromechanical coupling is rarely performed. One generally tries to limit oneself to a decoupled approach to the problem, in which one calculates the evolution of the pressure field while neglecting the deformations of the solid. However, this decoupling has the consequence of strongly underestimating the duration over which the pressure redistribution occurs. 2. **Unsaturated soils** The treatment of unsaturated soils complicates even more the problem as the transition from near-saturated to unsaturated zones introduces additional unknowns, non-linearities, and parameters. Again, the complete treatment of unsaturated soils remains rare. It is preferred to propose simplified solutions, neglecting partially saturated zones for example. Defining the initial state in the case of unsaturated soils is extremely complex because of the lack of experimental methods to characterize it in situ. # F5. Uncertainties and recommendations #### **F5. Uncertainties and recommendations** 1. **Uncertainties** There are many sources of uncertainty in geotechnics. The first is the relative lack of knowledge of the geometry of the soil layers that make up the solid being studied. In addition to the geological knowledge about the area where the structure stands, the main sources of information are the boreholes drilled on the project site. The extrapolation between boreholes, especially if they are far apart and not located at the exact location of the future structure (which may be modified after reconnaissance, for example in the case of tunnels), does not necessarily give an accurate representation of local variations in layer thickness. In urban areas, the presence of heterogeneities (cellars, wells, foundations of previous structures) is often difficult to detect. The other source of uncertainty already mentioned concerns the initial state of stresses (and possibly pore pressures) in the soil mass. It can have a major influence on the results of the calculation: this is particularly clear in the case of tunnels, where the loads considered depend on the initial stresses. Finally, the choice of constitutive models and the determination of the parameters of these models introduce a significant uncertainty on the representativeness of the calculations: if the constitutive model does not capture a phenomenon that controls the behavior of the structure, the result may be qualitatively and quantitatively very far from reality. 2. **Recommendations** In general, the user must be aware of the objectives of the calculation he is undertaking: the approach is different depending on whether one is trying to justify dimensions or to evaluate the influence of certain constructive provisions (the number and position of the struts, for example). One must also be aware of the modeling choices on which the calculation is based (even if these choices are sometimes partly imposed by the software). One must be able to identify the phenomena to be taken into account, which leads to the choice of a quasi-static or dynamic analysis, the consideration or not of the hydromechanical coupling, etc. One must choose between a 2D or 3D calculation. Three-dimensional calculations remain rare for the moment because of the time required to prepare the calculations. However, for some problems, it is clear that two-dimensional calculations can only give a poor indication of the behavior of the studied structure regardless of how long the engineer took in determining the soil parameters. For instance, the study of the stability of the tunnel face cannot be considered outside a three-dimensional context. The same is true for the study of bolt reinforcements of the tunnel face. The development of pre-processors specific to each application should simplify the use of 3D calculations and improve the representativeness of many finite element analyses. In geotechnics, special focus should be given to the choice of soil parameters: it could be the subject of a whole book. Most advanced constitutive models do not come without a detailed and robust parameter identification procedure, mainly because the model equations cannot be solved even for a simple problem such as triaxial compression. One must therefore calibrate the parameters so that the modeling of triaxial tests, for instance, outputs results in satisfactory agreement with the test results. A trial and error procedure is used, and since the agreement obtained is evaluated subjectively (because we can choose to better reproduce one part or another of the experimental curves), it is not guaranteed that two users will obtain the same parameter values from the same tests. Thus, all constitutive models do not have the same qualities. Some have many parameters, each of which influences a particular aspect of the soil response (but which does not necessarily appear in the available test results). Other models, on the contrary, have a relatively small number of parameters, but each of them can simultaneously modify several aspects of soil deflection. It makes the calibration much more complex. The last recommendation that must be kept in mind is to check the calculations as much as possible. There are not yet any general tools to measure the quality of a calculation: research work aims to provide error estimators, but their use in geotechnics remains rare. It is therefore necessary to look in-depth at the results: some inconsistencies are sometimes easy to detect. If there are any doubts, it is useful to have the results checked by someone else. In any case, it is highly recommended to carry out parametric studies to get an idea of the influence of certain factors, in particular soil parameters, if it is not certain that their influence on the results is moderate and that their value has been determined with acceptable accuracy. # F6. Normative aspects: Principles of the Eurocode 7 #### **F6. Normative aspects: Principles of the Eurocode 7** Numerical modeling always had a particular relationship with calculation standards, which essentially focus on the verification of ultimate limit states by calculating safety coefficients or the equilibrium of forces integrating partial coefficients. Indeed, numerical modeling provides first and foremost values of displacements and deformations and is therefore a tool very well suited to the verification of serviceability limit states (SLS) for which the partial coefficients are equal to 1 Its use for the verification of ultimate limit states (ULS) therefore initially appeared to be limited. From now on, particularly with procedures aiming to reduce the shear properties of soils (for example, the "c-phi reduction" procedure), it is easy to calculate a safety coefficient. It is also possible, through the procedures suggested by certain calculation standards, in particular Eurocode 7, to consider the results of numerical modeling both for the verification of the ultimate limit states and for that of the serviceability limit states. However, Eurocode 7 in its current version is not very clear about how the analysis and processing of the results using numerical modeling should be conducted. Indeed, the three calculation approaches proposed by Eurocode 7, which allow applying partial coefficients on the actions, the effects of the actions (bending moments and shear forces in a retaining wall, axial force in a pile, etc.), the properties of the soils (c and or cU), and the geotechnical resistances, have been designed to be used with limit equilibrium methods. The verifications related to the application of the Eurocodes are mainly transcribed in the form of comparisons between actions or effects of actions and resistances. Nevertheless, several publications (Potts and Zdravkovic, 2012, Tschuchnigg et al., 2015, etc.) and reports of different working groups convened for the development of the second generation of the Eurocodes make it possible to outline verification procedures. First of all, it is important to underline that the weighting "at the source" of the soil or rock properties, i.e. the possibility of reducing the cohesion and the angle of friction before carrying out the calculation, is not allowed because it leads to results that cannot be interpreted. Different procedures can however be used and are summarized in the table below. *Synthesis of the different types of ULS verifications***Type of ULS verifications** | **1 - Structural ULS** | **2 - Geotechnical (and structural) ULS** | **3 - Geotechnical ULS** | **4 - Structural (and geotechnical) ULS** |
Type of procedures | Multiplication of the effects of the actions by 1.35 | Reduction of the shear properties of the soils | Estimation of the resistance centered around a specific geotechnical structure (pile, tie rod, etc.) | Increase of the loads applied to the geotechnical structure |
Comments | Must be combined with the verification of geotechnical ULS | Must be combined with the verification of structural ULS | Must be combined with the verification of structural ULS | A priori, this approach is sufficient on its own |
In the wiki, by misuse of language, the term "bar" is often used to refer to "beam" type elements and not exclusively to "bar" type elements in the strict sense (i.e. working only under normal stress).
**A few reminders:** Computer calculation is based on a representation of the structure by a set of beams whose intersections are **nodes**. Its purpose is to determine the displacements of the **nodes** of the structure, i.e. the displacements of the ends of the beams, under the applied loads. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/qdOyYNrbCgm0EZ7e-embedded-image-y2wd3bcu.png) *Figure 1 - Sign convention - forces and displacements* The forces at the ends of the beam depend linearly on the displacements at these points. It is shown that there is a matrix relationship between forces and displacements for a beam connecting two nodes i and j, such that, for a given coordinate system, \[K_{ij}\]\[q_{ij}\]=\[F_{ij}\] (Figures 1 and 2), allowing the components of the vectors \[F_{ij}\] to be expressed as a function of those of the vectors \[q_{ij}\]. \[K_{ij}\] is called the stiffness matrix of the beam, \[F_{ij}\] the force vector at the nodes, and \[q_{ij}\] the vector of nodal displacements. *![](https://lh6.googleusercontent.com/rOHCiKt_le6Cz6bwKMpTmd2whHhIZiV6sDNAl9-O4Q4nUetzRfcj6YBarhoNDT4wJXJ6-uwzZAxm--__UfupDO-85zBOXJRc5GU3DlZNysVkNuHPBQBDe7h1psUhtVaQayEy_U6QvPcRru6hzmeGnA)* *Figure 2 - Stiffness matrix of a bi-clamped beam* The matrix \[Kij\*\], associated with the global coordinate system, is deduced from the matrix \[Kij\] expressed in the local coordinate system of the beam by applying a transformation \[Λ\]T \[Kij\] \[Λ\] (figure 3), making the displacements compatible with those of the global coordinate system. \[Kij\*\] = \[Λ\]T \[Kij\] \[Λ\] is then the stiffness matrix of the beam expressed in the global coordinate system. *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/iWRzPnPLSutb2W6l-embedded-image-a9nif9mh.png)* *Figure 3 – Rotation matrix* To calculate the displacements of all the nodes, the software: - "assembles" the matrices \[Kij\*\] of each of the beams to form the overall stiffness matrix \[K\] of the structure (figure 4), - inverses \[K\] → \[K\]-1, - multiplies the matrix \[K\]-1 by the matrix of the external forces \[F\], previously brought back to the nodes (if they are applied to a beam other than at the ends), in the global coordinate system, to calculate the displacement vector \[q\]. *![](https://lh3.googleusercontent.com/rK8z68fL9mEyLR8V1q8APLTac7ufMlaaY5lsA53b53IloZBCuNbXEN_hIi5yttC5KsMVxPLomsbwtKIs0GQkNXB9SkiWL2g7QKBX3blKEN7SzWVUX1Mum8MpAM9FOCrl_Qsm-lvgLaxdhs5-p4dDtA)* *Figure 4 - Principle of assembly* Finally, to calculate the internal forces of the structure, the software multiplies the stiffness matrix \[Kij\] of each beam by the vector of displacements \[qij\], in the local reference frame, at nodes i and j. Thus, the forces are calculated at the nodes and added, if necessary, to the reactions of the bi-clamped beam (i.e. the forces introduced in the global model, but here projected into the local reference frame of the beam) - see the second example below. The forces and displacements along the beams can easily be deduced from those at the nodes using the Strength of Materials formulae. **Application to a simple example:** ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-10/1ALZ8ZfBC6FH0joi-embedded-image-8bddmenr.png) *Figure 5 - Calculated structure* This example is processed using a spreadsheet, the source file is provided in Part 3 of this guide - it can be downloaded by clicking on the link below. [**Source file in Excel format of the example above.**](https://wiki.afgc.asso.fr/accueil-gtef:annexes:annexe1) This spreadsheet covers two examples: the example developed below for a 2-beam structure (to remain easily readable in paper format) and a second example with 4 beams. These examples allow you to visualize and understand the sequence of tasks. The required beam characteristics for a plane problem are the section S, inertia I, Young's modulus E, length L, and orientation α about the horizontal for instance. ![](https://lh6.googleusercontent.com/4vQkgGYKoUkoBlzZKTxPQjbXoEgQJZ1ACSfI1Xg0mnk8ArT3mJtDFpt0jZzN9gm-Zk_R8-fiJIACrVxhQ64fJive8c_taeeF7lQLDkrCO3wm4uxvV_cWZ5EVGgEj0SHowarsaLDsWFGZHyseEeAxIg) E = 36 000 MPa for all beams. The numerical values of the stiffness matrix for each beam are easily determined from the literal values in figure 2. *Beam 1: Stiffness matrix* ![](https://lh5.googleusercontent.com/4i_cyufvbKZ4BBQ-jaqvKYcaFK0mvRY1nFGoWJ6OCUUZPxzJS3ziM2emhASwgeoREuFEwyGrsnp7b7gwxDkXXPwZszyBgk4zTQM22w8phoc1M0TbVci87R8Jct1b55ky1OnVEGeen1BKuhnzuNs6pQ) *Beam 2: Stiffness matrix* ![](https://lh4.googleusercontent.com/tc6_NQn_2bgCeNEMl4qAkFkznaKXLNMFZycFfrzHcS5ZGN1n7ETroZAvPBqG4R_Z7nGtmfPCD6fyPzD30Ta1YK8wO2eiGbbGrZdMuJ9HauJLfFbMJzDGWmkdpbyRPWypvB9AIpdrSJslLHKL67lswA) The transformation is applied to these two matrices to make them compatible with the global coordinate system. Rotation matrix for α = 1.571 Rad: ![](https://lh3.googleusercontent.com/hAlWElQ3ntrBejVAq9tqjbFFo0X4fMrrJx_ZVB3w44h0icTWdwkqx96nGjcm4L18QXOZuPdXDEGzg5FRDjYQbVvdslKVKR0Boq8ooHoD-xBtQwwf6Kr5rsqfUvPg2R9nql5oNHvHKtrHHUe7zdFVYg) And its transpose: ![](https://lh4.googleusercontent.com/bSe0cFzl_EUyWQ4RDOY2MRUv5wnjDMKU4XwgRFsZkTbpttNJSuRB3gwxRxFg3RwUJvLWauEJiBffL-9yHUtnbTcPzVwE789fKSEwfjyUxg8lTStbQ7gmNovYDYCaBCCaDlfS3mKZsiid9VkiDLKYgQ) Rotation matrix for α = 0.197 Rad: ![](https://lh6.googleusercontent.com/EHRTvnYFK6O3h5fNHWiTXtTU3zLL8TirN9x-4617m-J-M1bQjmRUfY0qx3MlDsHm-zQXEhi7FLjyj6FdkOuCwskzAGcgYp6Nk7BwXWRHJMsqUaC9_bWeIrPxcCD-Lqvv277LmdlBe2f1BI4x4s_oqg) And its transpose: ![](https://lh3.googleusercontent.com/yjcgkk6S3-cdDyCJOJOfOLemc03Y5KDi3wmUP5U8N8lHT4YRM_j6oXtSTu7HlOM7A6f0sKlT8E51rtgv_ih-hVtjdxkX0wtRqN4X1ip98PRN--7OQmu0qX05thXk4ngaFpALiTxGca9RalZlKYbraQ) Beam 1 - Result of the operation \[K\*\] = \[Λ\]T \[K\] \[Λ\]: ![](https://lh5.googleusercontent.com/bYiikquB4j6wpeftEEKpYIs2gz4Ybns9-Zd1r1snQmHv7jyKMNios42GdnSy_hD7gDlUG8k4XNKQnwXHz--RSC0Z42Ok6zqOZdROk5MbqkIXIR0P5XMTH9aP8wLtE9VUlsCi7y7GWh1MR1TvIwbRFw) Beam 2 - Result of the operation \[K\*\] = \[Λ\]T \[K\] \[Λ\]: ![](https://lh5.googleusercontent.com/c33JgmGXHu5i0izDGeIXq6bkCIDPzMEhPSMSRSWNlySNHUmvtzxFMkgF5II9MxQaLRbBHcMoX1rz7_Uz4Nj6gqaOEM7GJXzfDtw25q2Mk2IEfSl6P2NrvI2ZjLPd2HGLNmP5NaHnCg-V81_xfKe3zg) All these unit matrices are then assembled, i.e. all the matrix values relating to the same nodal displacement are cumulated. For our example, it means summing the values of the two matrices corresponding to the common nodes (in the general case, the beams do not always connect two nodes whose numbering follow each other as shown below): ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/oyKAe6hrjeaVN6UJ-embedded-image-xczagjsq.png) The blocked displacement components can be removed from the matrix since we already know that their value is equal to zero: ![](https://lh4.googleusercontent.com/_XsjDSdjXHu9vRXHSDb-0Sd1RgmRUUbppkBXhG8FGfzaagMtB9AZbc_c-H1dhMf_L31cINlIfcYod8jSVyZlXqVmLpjKFRXkkFWcrdqaS2Nut24-DBI9U_prsOWrmTEPCYOCzbqO1e6dz4k7dph2Rg) This matrix is easily inverted using the spreadsheet: ![](https://lh4.googleusercontent.com/Cp36d8No2J2r6J2AgAbSsHSfXcR7BwG4e0BwY8P2WT3XB_hvkamnq8pJcxvZnuL_DnIODd8pu43sEKpuJcPidM_aMYpEIkBoj7fAW2X6HIUJjVoXQSV0aOJxu61JLZDkOD2ngQD1HIeLbtg8Los4QQ) --- **Load 1**: External forces applied on a node ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/FUDaZJBP1RQPhf1N-embedded-image-fcgmrcuw.png) *Figure 6 - Load definition* The nodal displacements are calculated (in the global coordinate system): ![](https://lh6.googleusercontent.com/hMkgFGKkccIJzEesc0M65QmQVKJAbGoIRUTkWId77xRS-o0hizTErfyQPnb1LoHT8SgrjEbz0P3fouQjB_4xq7i7vWa_b7cBs0WUWtQU-HmnQqZ4DUmQBi6Xawh1ZxM2BjTnr0hcttTtffBWnGDR2A) The forces in the column (beam 1) can be determined after transforming the displacements to the local coordinate system of the beam: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/27myy3gezUflMhb4-embedded-image-rntd8bay.png) We have a compression of 12.68 kN, a shear effort of 1000 kN, and a bending moment that changes sign along the beam (we check that 1000 kN \* 8 m - 3654.89 = 4345.11 kN.m in the base of the column - ok). *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/KaXPIE9RQt5IURrw-embedded-image-v0ytbgyl.png)* *Figure 7 - Diagrams N, V, M - example 1* --- **Loading 2**: External forces applied to a beam (i.e. other than at the nodes). ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/jeuTxrV80V4A0VGV-embedded-image-avnomlg2.png) *Figure 8 – Loading definition* In this case, it is necessary to calculate the support reactions of the bi-clamped beam under these forces beforehand, as they are the ones that have to be incorporated into the matrix of external loads (the software only knows the nodes!). A bi-clamped beam reaction table is enough. Of course, the sign conventions must be observed. Application to the horizontal distributed load p = -1000 kN/m on the column (figure 8). In this case, it is known that the clamp moments are -pL²/12 and the shear forces at the restraints are +/-pL/2; therefore, with L=8 m and taking into account the sign convention: ![](https://lh6.googleusercontent.com/iWk9y_U86TOjsJM5ePTyzA74TLsPbsHnm4uta0z7jpHDPHNfrz5Fsp2vibjkT4D4053V0QgoQzJy6PPGy0_WUMJSFPnxvbKQeJqVaMOD7E1cVT3swfGc6MVh4tK4Bg7Sb_IFHfmJFDdT_nUgzEKgbA) Multiplying \[K\*\]^{-1} by these efforts provides the values of the displacements of all the degrees of freedom. It is then enough to multiply the stiffness matrix of beam 1 by these displacements to recover the forces at the nodes. ![](https://lh4.googleusercontent.com/pK0ifablCvpK9h7KpQ_IFYq3b7FoF5GGhUby6jD1IZ_GNo-UlgomOjEgcoQu8RfEmZMo6jViaRfHxUfi60-qMkH1YBhW4EbLHTWUeS0m3XLmO3rWpyeLL4YAEI1gQU9zBwRuaqjo7QRk4wWbQeqkIw) The efforts in the column (beam 1) can be calculated, after converting the displacements from the global coordinate system to the local coordinate system of the beam... ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/ukk26BMzqUHOLVjA-embedded-image-6idv5yxh.png) ... and add them together with the forces of perfect clamping, with the appropriate sign convention: ![](https://lh4.googleusercontent.com/JJytMK8ueg6Hjhsvxd41esu43w1r9dLJqFq_fBJHjsj8F4mtZ1y59_roNm4_AOjFU2oIx3YfpXFKVf5eK2B6GX2dSmdVc2wQ__TLt6uLBNL2kUZqtYWWWT7vW6wNBPhWI6MtKLcgYh6un73TTHo_Zg) We have a compression effort of 1298 kN, a shear effort that increases from 0 to 8000 kN (pL=1000 kN/m \* 8 m = 8000 kN), and a bending moment at the base of the column which is much higher than the perfect clamping moment. The same methodology applies to beam 2 to obtain the efforts at the nodes. *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/lJi4D5Y1rZwF8AzM-embedded-image-f6mtcktb.png)* *Figure 9 - Diagrams N, V, M - example 2* --- **Cases where the beams present important differences in stiffness:** For example, the vertical beam is stiffened very strongly. We decide, keeping a length of 8 m, to increase its cross-section to 1m \* 1012m (b\*ht). The matrix \[K\*\] is shown below. The difference between the larger and smaller values can be easily observed ... which can lead in some cases to numerical instabilities (the resolution leads to dividing the matrix terms by one another). *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/fA4bHa7UdWp1d1ii-embedded-image-vu2w3tz9.png)* *Figure 10 - Matrix with contrasting values* # A2. What is a finite element? #### **A2. What is a finite element?** The resolution of the efforts in the elements is carried out following the calculation of the node displacements. The method is specific for each type of element and depends on the software used. However, the main principle is common to all software, it consists of "isolating" an element to calculate the forces at the Gauss points from the nodal displacements. The position of the Gauss points is normally specified in the software documentation; in the case of a 4 node shell element as below, they could be located at a distance from the edge of the element equal to about 1/5 of its width. ![](https://lh3.googleusercontent.com/qw7L8Y5ncCnD8ldmFLRyX_VkhYSihxd64xLINrXDKYEWcE5uQNgT6YRRsg6-uH7at0lURyXSHdyfbMAaA4LpKSjfNa0MLoxzPQ9e2tsKDxybO9WwFkSLAnvNZG50BJzTjDXr79sAAl7RU0_1aTpK8g) *Example of a 4-node element* The efforts in the center of the element are calculated as the average of the forces at the Gauss points, the efforts at the nodes are extrapolated from the Gauss points. ![](https://lh4.googleusercontent.com/9osD1-jiHDkYUZbKKLvskrksPYrqWSQ-EB6DUSaeMo45uBknwE-p919EWpTvZXru13P_h_BI0tsRImbRaa6SEToqElf3hGXksags9auF8VFzQV0R-I9oSuW7VWwXyDT-FxnMFnf3-VdMY7S3y1Zfhg) To summarize, the software calculates: - the efforts at the Gauss points G1 to G4 from the displacements at the nodes n1 to n4 - the efforts at center C which are the average of the efforts at the Gauss points G1 to G4 - the efforts at nodes n1 to n4 which are extrapolated from the efforts at the Gauss points G1 to G4 ![](https://lh4.googleusercontent.com/AUaIXgP60ge6sowo5_lVXSoMZ1jbUKSxA8X6zNufEodEi5YAmT51Yj6pR8CjF_xlN939YXskkotbG2Cd3xAOLYK1qq2n3YJYJJTmyaxpVnJHQWmOi4DCqMR5g6yO-TL1XGiQG8uoF7Rca2G7tim5lw) These calculations are carried out for all the elements. In the end, there are as many efforts at the nodes as there are elements connected to this node (here 4 elements E1 to E4 connected to node n1). We can then deduce: - either the maximum effort at the node (maximum of the efforts calculated from the elements E1 to E4) - or the average effort (average of the efforts calculated from E1 to E4) Main remarks concerning common usage - Generally, quadrangular elements will lead to better accuracy of the results than triangular elements. - Results at Gauss points are the most accurate, but they are generally not accessible to users. - The results at the center of the elements are more reliable than the ones at the nodes because they are not extrapolated. - It is up to the engineer to choose the type of result (maximum, average, smoothened, etc.) according to the behavior of the structure. There are no predefined rules. [**Example of a load on a bridge slab illustrating the differences in results during a FE calculation.**](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-d-simple-example-modeling-of-a-br-wheel "Example D - Simple example: modeling of a Br wheel") # Chapter B. Computational objectives and necessary characteristics of the tool #### **Chapter B. Computational objectives and necessary characteristics of the tool** Creating a finite element computational model includes several steps. The choice of the tool is critical and depends on various criteria. A successful model requires good organization and preparation. [B.1 to B6 Criteria to be considered ](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/b-calculation-objectives-and-necessary-tool-characteristics "B. Calculation objectives and necessary tool characteristics") [B.7 Organization of the computational model](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/b7-organization-of-the-calculation "B.7 Organization of the calculation") # B. Calculation objectives and necessary tool characteristics #### **B. Calculation objectives and necessary tool characteristics** Creating a finite element computational model includes several steps. The choice of the tool is essential and depends on several criteria. ##### **B.1 According to the object to model** First, computational software must be adapted to the object one wants to model. a) The complexities are different for bridges (standard short-span structures or complex structures with several spans), buildings, or geotechnical structures (retaining walls, tunnels, dams...). Depending on the size of the object, one or more modeling scales can be defined: - a **geological scale** (which aims to process a structure in its environment according to geological data), - a **global scale** which aims to handle a structure as a whole (longitudinal calculations of bending for bridges for example), - a **semi-local scale** with a more refined mesh for some elements of the structure (transverse calculations under the actions of axles for bridges, for example), - a **local scale**, with very refined modeling and post-processing of the results (calculations of reinforced concrete for punching, diffusion or bracing reinforcement, for example). b) An object can result in several models that complement each other.**Scale** | **GLOBAL** | **SEMI-LOCAL** | **LOCAL** |
Bridges | Longitudinal bending | Transverse bending | Stress concentrations (anchorage or deflection zone of cables, concentrated support) |
Building | Load path / Bracing (wind, earthquake) / Dynamic calculation | Local bending of horizontal elements (floors, foundation slabs) | Concentrated, accidental loads (anchorage area, machine supports) |
Geotechnics | Backfill, retaining wall | Faillure of anchored tendons, draining... |
**Object \\ Advancement** | **Preliminary Study** | **Pre-design** | **PRO** | **EXE** |
Bridges, Industrial Building, Civil engineering structures | Ratios, Feedback, Simplified global model (a 2D model is preferred) | Global model | Global model + semi-local verifications or even verifications for critical points | Global model + semi-local + generalized local |
An equally important resource is the staff, i.e. the engineer in charge of modeling. They must be trained to use the software. If the engineer is new to the software, the learning curve should not be underestimated, as the time required to design and develop the model can be greatly increased. Tutoring with a senior engineer is strongly recommended, despite the time investment involved.
##### **B.6 Depending on how user friendly the interface is** Finally, making the software user friendly is essential. a) A software with a complete manual (installation, handling, and operating instructions) is always much appreciated. The presence of a catalog of examples and applications, tutorials, and manipulations are extras but also valued. b) The possibility of programming (creating and reading a text code in a programming language of one's own) allowing intuitive and fast data entry is an asset. It can offer many possibilities to the user, for example, to automate the modeling of simple and repetitive model structures or to adjust the layout of the results, by providing text or Excel outputs adapted to the studied sub-structure. c) Confidence in the software saves a significant amount of time by avoiding superfluous verifications. Thus, having regular updates is an indicator, as is the existence of an available and reactive technical hotline, capable of providing punctual assistance on a specific model. Of course, trust does not dispense the model verifications explained in this guide. d) The version of the software can also play a role, in the case where certain features have been added/removed or where the stability and/or speed of a version is not satisfactory. e) Some software have complete libraries (materials, profiles, bolts, assemblies...) that save a considerable amount of time. Functionalities specific to civil engineering projects also exist, such as the application of regulatory automatic loads (types A(l), Bc, LM1, LM2...). f) Depending on the standards that apply to the project, the software can propose loads, combinations, and pre-programmed verifications. This is a helpful feature but it must always be checked using simple cases. g) A render function is an advantage because it allows visual verification of the type and orientation of the profiles or bars. Besides, some software allow a 3D export which is a very useful communication support in meetings with stakeholders (see also chapter E.3 for the BIM part). h) A software that specifies the line of the data file that contains an error or the list of wrongly modeled objects (overlays, ...) in the spatial model offers a real advantage. Error messages must be clear and precise (if possible, in the numerical language of the engineer). **Experience feedback**: Feedback is important: meetings or feedback documents should allow drawing positive and negative lessons from ongoing or completed projects. They must cover the methods used, but also the IT equipment used or even the production level that was reached. # B.7 Organization of the calculation #### **B.7 Organization of the calculation** This is an essential step to be carried out at the beginning of the study. 1. **Preliminary reflection on modeling** A preliminary step is essential for the modeler: the analysis of the overall behavior of the structure. Indeed, it would be foolish to start modeling a structure before understanding its overall behavior. A first sketch of the structure reveals a good understanding of the behavior and will be used as a framework for the creation of the model. Mainly, this analysis of the overall structure allows distinguishing the main elements that reflect the behavior of the structure. Among these main elements, one will distinguish for example : - for civil engineering structures: the load-bearing structure of the deck, the structure of the supports, the bracings, - for reinforced and prestressed concrete buildings: columns, walls, and slabs, - for building structures: columns, beams, bracing elements. The model must be based on input data, with at least: - a general assumption, which contains a description of the object, the standards applied and the loads applied, - sketches or general drawings of the object to be modeled, - a general construction principle, - an outline of the static and possibly dynamic behavior. Modeling does not replace these elements of preliminary reflection.BIM and modeling: The designer may be tempted to use the input data in an automated way to build his model. This is a frequent argument of software publishers. In this case, he will have to be particularly vigilant about the quality of the inputs provided (it is indeed not uncommon to find 3D models with geometric nonsense) and the level of detail of the input data (quantity of hoppers for example). In the case of automated processing, special focus should be given to the geometry construction process, especially at the connections. Thus, the analysis phase of the overall functioning mentioned earlier is a way of preventing any anomaly.
2. **Input data validation / Input synthesis** All documents defining the geometrical assumptions, materials, loads must be referenced with their origin, index, and date of issue. It is necessary to validate the coherence of these different documents. For example, are the architectural plans and the structural plans consistent with each other? Are there any geometric discrepancies between the different plan files? Are the data exhaustive? Are infeasibilities already observed (e.g. complex load path, lack of bracing...)? This synthesis work allows us to highlight the missing input data and/or likely to be modified and to define the conservative measures taken to compensate for the missing data.Based on this preliminary analysis, certain decisions will be immediately imposed on the designer: exchanges with the client, revision of the geometry of the structure (design revision), input of parameterizable data...
This synthesis phase will ideally take the form of a "Modeling Note" that will evolve as the model progresses. The aim is to have the hypotheses validated by all the participants in the study very quickly to avoid modifications, which are often long and complex. ![](https://lh3.googleusercontent.com/sksH-DAIw6rLFProSJvKV549-qsqHIgOTBEcypNDRgaR6-qDWXHxW_pNgzMbpe8PHi8xqKJw7haJhXDijgGEHyj75UdAJuwMjyBpT_2nUXbbFELqnd3Ywxmh_5jVgwmYlrVvJlTJi6NYsXubxfYKrw) 3. **Specifics of the study** All the specifics of the study must be listed at the beginning of the study: - the physical constraints of the project (important heaving, urban area, construction phasing, ...), - the study constraints (tight schedule, numerous interfaces, missing data, ...), - the particularities of the model (size of the model, non-linear, earthquake, ...), - the requirements and sensitive aspects of the project (slender structure, asymmetrical, heavy wind, etc.). It is necessary to show that the modeling will consider all these points. 4. **Planning of the study** It must clearly show: - the deadlines of the main modeling phases (geometry, materials, loads, interface or soil-structure interaction, combinations, etc.), - the deadlines for receiving missing or modifiable input data, - the deadlines to send the deliverables used as input data to other study stakeholders (interface) and for other deliverables, - the consistency of the study with respect to the dates of the phases. 5. **Modelling Principles** The goal is to explain the calculation methods, making sure to: - clarify the principles of the structural model, the methods to consider loads, combinations, ..., - justify all approximation assumptions, - if necessary, present small test models validating the hypotheses, - present the sequence of calculations. # Chapter C. Good practices to create a model #### **Chapter C. Good practices to create a model** The different levels of analysis and the complexity associated with the model have already been defined in the previous chapter before the modeling stage. This chapter highlights the simplifications that can be used to create a model that is structurally representative of the real-life structure and the loads it is subjected to. The different levels of investigation and complexity associated with the model have already been defined before the modeling phase in chapter B. This chapter presents the possible simplifications one can adopt when creating a model that is structurally representative of the design of the actual structure, its behavior, and the stresses it is subjected to. [C.1 Input data and units](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c1-input-data-and-units "C1. Input data and units") [C.2 Modelling of the main elements](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c2-modeling-of-the-main-elements "C2. Modeling of the main elements") [C.3 Finite elements and meshing](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c3-fe-and-meshing "C3. FE and meshing") [C.4 Modelling of the non-structural elements or the equipment](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c4-modeling-the-non-structural-elements-or-equipment "C4. Modeling the non-structural elements or equipment") [C.5 Boundary conditions](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c5-boundary-conditions "C5. Boundary Conditions") [C.6 Connections – links – assembly ](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c6-connections-links-assembly "C6. Connections - links – assembly") [C.7 Eccentricity ](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c7-offsets "C7. Offsets ") [C.8 Combined cross-sections (beam/deck)](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c8-composite-sections-beamsslabs "C8. Composite Sections (Beams/Slabs) ") [C.9 Materials](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c9-materials "C9. Materials") [C.10 Behaviors specific to shear and torsion](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c10-specific-behavior-in-shear-and-torsion "C10. Specific behavior in shear and torsion") [C.11 Loads modeling](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c11-modeling-the-loading "C11. Modeling the loading") [C.12 Further information related to volumetric elements ](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c12-more-about-solid-elements "C12. More about solid elements") [C.13 Further information related to non-linear calculations](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c13-more-about-non-linear-calculations "C13. More about non-linear calculations") [C.14 Further information related to prestress ](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c14-more-about-prestressed-concrete "C14. More about prestressed concrete") [C.15 Further information related to phase calculation](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c15-more-about-phased-calculations "C15. More about phased calculations") [C.16 Further information related to structural dynamics and seismic calculations](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c16-more-about-dynamic-and-seismic-calculations "C16. More about dynamic and seismic calculations") # C1. Input data and units #### **C1. Input data and units** The input data must be consistent, whether these values are defined in the model itself or come from other files such as a library of profiles or data from other software (\*). Some elements of the methodology are provided in paragraph[ B.7 Organization of the calculation.](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/b7-organization-of-the-calculation "B.7 Organization of the calculation") (\*) Special attention must be paid to the units and signs when introducing stiffness matrices that model the foundations or other parts of the structure, especially if they come from another design office that uses different software. Moreover, for soils, one should verify whether the characteristics are expressed for the long or short term. Material characteristics, especially for concrete, must be consistent with the analysis conducted (see details in [paragraph C.9](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c9-materials "C9. Materials")). The unit system in which the data are expressed must be known because it will condition the units of the results. The use of SI units is preferable.One should ensure the consistency of the stresses, lengths, modulus, and stiffness units.
# C2. Modeling of the main elements #### **C2. Modeling of the main elements** **C.2.1 Creating the geometry** The first stage of modeling consists of creating the geometry of the model by defining points, lines, boundaries, areas, and volumes. The notions of nodes, elements, and meshes are associated with finite elements. In some software, the geometry can be defined before creating nodes, elements, and meshes. In others, the geometry is established outside the software, using diagrams or Excel spreadsheets, and the nodes, elements, and meshes are then defined directly in the software. **In any case, the sign conventions used by the software must be known at the start of the modeling (direction of gravity in the global coordinate system, sign convention for bending moments, forces, and stresses).** Some general notions: - **Nodes**: their presence is essential at the supports, the joints, and the boundaries between geometries. Depending on the software, nodes should also be present where the data will be extracted. Please refer to § D.3.2 for more information. Depending on the software, a node must also be provided at each load application point. Finally, depending on the phenomena one wants to quantify, for example for large displacements or dynamic calculations, intermediate nodes must be defined on the beams to accurately represent them. Defining the points of the geometry means incorporating all these node requirements. However, the number of nodes must be limited to keep the model as light as possible. - **Structural elements**: in most non-solid models (bars, plates, shells ...), the elements will be modeled at their average fiber. This is the safest method for the good transmission of forces between elements and the consideration of secondary effects. In the case of beams for which the loads are located on a particular face (bridge secondary beams, for example), it is possible to define the element at this face and to create an offset, if the software does not do it automatically. The positioning of the average fiber of the elements with offsets is discussed in [§ C.7 Offsets](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c7-offsets "C7. Offsets "). In the case of beams of variable height, the mean fiber is no longer a straight line, which leads to multiple local coordinate systems for the different inclinations and can complicate the exploitation of the results. If the arch effect is not considered, the model can be simplified by keeping the neutral fiber straight-lined. - See also the calculation examples for beam grids for which simplifications can be admitted ([Link to the examples](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-c-beam-grillage-modeling "Example C - Beam Grillage Modeling")). **C.2.2 Degree of simplification: shafts and openings** Depending on the study phase and the type of calculation carried out (for example stability or load reactions), not all the openings will necessarily be modeled. **The case of buildings.** For buildings, when the openings are considered, it is advised to integrate into the geometry the shafts of non-negligible sizes and the ones which may affect the behavior of the structure (at least in the bracing elements). The latter will be cut according to the intersection wall/wall, wall/floor, shafts, to have a mesh as regular as possible. In the case of modeling a building, the shafts are defined as a function of: - their size (any shaft in a wall or slab whose largest dimension is less than 1m is commonly neglected). - their spatial distribution - small but closely spaced openings can be considered as a single opening whose dimensions correspond to the perimeter of the envelope. - their influence on the force transmission. Particular attention must be paid to the lintels of doors in structural walls (and bracings). Indeed, these lintels might have numerous openings, so they may no longer be able to fulfill their structural role. Consequently, the model must be adapted. When the openings are not known, the modeling of buildings subjected to horizontal forces (wind, earthquake) must consider conservative measures concerning the large shafts (generally for ventilation). It is often necessary to reduce the thickness of the lintels fictitiously or even to remove them from the model. Example of how to model a group of openings: ![](https://lh6.googleusercontent.com/fxVr7ebBphR2V0TXrozkVhCL8oBAzppyn7C2cqn4m3-O9BxpcUobUKNNfA0qKoWiJNxGl7VSFf8GnyLk3s-bE6eFebkI026IJLyLhGdqJiagiILXrYc-PpfSVPZ2MWG0fjNdobMYZ-4HTSUWjTQIEQ) Example of a structure with close openings... which clearly cannot be neglected. ![](https://lh5.googleusercontent.com/Wg7tFehFuoaYQVVp1YZ1nOBydFovH4BLBvQ7Qc81fE8caHfWW4gsZCpE2rBDrxk-DNZpN5Fc1IcaZFguz0MvYE_I-O0SafRRaLjeKBu4RIOxPgaXmdx1e3VvpWXsQc0RFEXUiv4yx-hLl2-r83v-WA) **Case of steel construction**. The CNC2M recommendations for the dimensioning of steel beams with openings in the web according to NF EN 1993 states that an isolated opening with a maximum dimension less than 10% of the height of the web of the beam is not considered significant. When modeling these openings, the same rule can be applied. Nevertheless, this opening must be considered when verifying the resistance of the cross-section according to NF EN 1993. In the cases where there are wall collaborations with diaphragms made of ribbed plates, according to EN 1993-1-3 § 10.3.4, small regularly distributed openings whose cumulative surface area represents up to 3% of the total surface area may be arranged without any calculation of the diaphragm. It is doable as long as the total number of connections points of the panels constituting the diaphragm is respected. Thus, from a modeling point of view, such openings may not be considered. **C.2.3 Degree of simplification: curvature, slope, ...** When modeling the geometry, at the structural element scale, the curved elements will have to be represented as accurately as possible, knowing that the meshing phase will discretize these curvatures by a succession of straight segments, depending on the mesh size chosen and the nodes already defined. The part of the Eurocodes NF EN 1993-1-6 dealing with the strength and stability of shell structures gives some indications on how to take curvature into account. For bridges, the effects of slope, curvature, and skew angle must be considered, and their non-inclusion in the model must be justified. For common straight structures, since the slope is normally limited at the design stage, it can generally be neglected. On the other hand, for curved structures: - depending on the level of the supports and the hyperstatic degree of the structure, the slope cannot be neglected. - whether the structure is curved over all or part of its length, the centrifugal force and the slope must be considered. It should be noted that the standard NF EN 1991-2 indicates that the centrifugal force, including dynamic effects, can be neglected if the radius of curvature of the pavement in the plan is greater than 1500m. - curvature and skew angle create non-negligible torsional moments in the structure even when the traffic is transversely centered on the structure. To establish an order of magnitude, a structure can be considered as being of low sensitivity: - to the skew angle when it remains greater than or equal to 70 degrees. - to curvature when the angle between two adjacent supports is less than 0.3 rad. However, it is difficult to establish general rules and the reader is invited to consult the design guides specific to each type of work (PRAD, PIPO, PICF, ...). *![](https://lh5.googleusercontent.com/5QFR0zM1tfPOFl-NPvvIv0r-hkCxHYkhU9wW1SBzvrepecDJVlk1ddXbnO6kgwhhXS_Wh7gVmi5Zru8-xMcEDZ131ebguUqcO-hnYuRA8njl15mYl0MLDniZXgY1MVyiEZ_GrRNrCkp7t0d-qRhG9w)* *Illustration of the angle between two supports* The example of a girder grid "[Modelling the same structure using different approaches](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-c-beam-grillage-modeling "Example C - Beam Grillage Modeling")" (in Part 3) illustrates the effects of skew angle and slope on an example of girder bridges. **C.2.4 Degree of simplification: Alignment of structural walls of variable thickness** In the case of a building, a vertical alignment of the elements is recommended to ensure a simple load transmission. However, various requirements (sheltered equipment, available space, etc.) can lead to certain offsets from one level to another. A simplification of the geometry during the modeling can however be made (mainly to avoid excessively heterogeneous mesh) by aligning the vertical elements and even the horizontal elements. This simplification results in a good representation of the overall functioning of the structure provided that the recommended constructive arrangements are respected. However, it is necessary to make a local verification of the proper functioning of the transfer of forces and to reintegrate the actual offsets in this local verification. Similarly, for steel structures, in the presence of footings or tubes of variable thickness (ferrule for example), a single average plan is usually used. For example, a tank composed of shells of different heights and thicknesses will be modeled with cylindrical surfaces with: - an identical radius equal to an equivalent average radius. - appropriate thicknesses according to the height (shell thickness). The value of the equivalent mean radius can be defined according to the Seismic Guide for Storage Tanks DT108. This guide brings examples on how to determine an equivalent uniform thickness, which allows defining the value of the equivalent mean radius = Internal radius of the ferrule + Uniform equivalent half-thickness (see example below): ![](https://lh6.googleusercontent.com/-WgqzEGSvuBKH6vdYGjDtcPJ7zwGAIjBI7zPU36E96Y613oxSsfC2RZ5ktI_hYTOp518RoUW4RkK1xaGEysLBJoqST9AQRAAumO4i1wus5cM_V4n1INr1pVh6SuyWk--m8FG6I7y8svFhL58yASGQg) ![](https://lh3.googleusercontent.com/CUDZHjXuehbypke_gOfaHBY08ppjZmkyc57wZ_kw9m5v5pzcJeG16wmZ3CDrupyTSstw89gI_xRvpC8iUrPLxwQYYwlA3X_EvXvimJALLfmnN-NyBtSVKs0rCRZr0IrZIG2WATeY415HfygkUEt7Gg) **C.2.5 The use of symmetries** As discussed in [Part 1 A2. The dimensionality of the model](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a2-the-dimensionality-of-the-model "A2. The dimensionality of the model"), when the structure presents a plane or planes of symmetry in its geometry, it can be very interesting to limit the calculation time and the size of the model by using this symmetry and model only a part of the structure. Appropriate boundary conditions must be applied on the plane of symmetry. However, it is important to highlight the fact that the loading must also be symmetrical, and that the solution obtained will be symmetrical (for example, the antisymmetric natural frequencies will not appear). --- **Example 1: 4-span symmetrical bridge** The spans are 60/100/100/60m long. The bridge is symmetrical with respect to its midpoint. One could be tempted to model half of the bridge, by placing a symmetry support condition at the center (on the right side of the figure, vertical translation blocked, rotation blocked): ![](https://lh5.googleusercontent.com/JXg95RgCjGU0KqNmTbYI28_8f5Ozrta3Kw2N2rlx-NbMfEWmuYbr1XSJWNrICkmiol1hPq3y9TQ1lKimzOer1K3CJXt7gFneEsVit-g2_2Xt6qkXsTalMiaL-s2JKyDg1QyGbjTPzSuUYuKzPlzmvw) Symmetrical load case: ![](https://lh4.googleusercontent.com/aYhrS_uNgvAL_PHJX_eyWn9ddSGkk-1Xacv0-yWG0hstA7l0YRcBSWBzuqjS8YsiZ834XkCEZVa7IHFEf_L3biJyQFnGIkMYjDS7eRKJ1McoPiXOpLZZgf2gdZQjWblbCer9-BuYNIOCWYxgnw8cVg) In this case, the results are identical for both structures. ![](https://lh3.googleusercontent.com/6x6hJXtfSvKvN0QnDnnf43NYRsJL24u-HwU8je3X6txWjvFCXPMN5XZkLqA6wtuegYI-tRPN9YBNOvcQweBidbydrLcBY2l5wN4V3Y7nUEAV8u4R3DuwKoXuVGossEsRIZs5rih6hJhtaj8MISb5nA) Case of asymmetrical loading: ![](https://lh4.googleusercontent.com/nIKuVVD_2qZjs5Ta9IL_iJqA5EZssXyFlItzDpLIfpR4X7l24NbPoWSzWQX4yokEGdTqvu-O5KuF7ZlfSoGvT8z0yBj7PBbLcdA_kQoI9LAN5088QWTDAsXTdNTBUZygsAjnzi4UGDrBuJwNSPSnDw) In this case, there is a significant difference in the results: ![](https://lh5.googleusercontent.com/A2_-MwBYredQBTJrslHhQBF2O0En15iC77o8oKRzCzO8fWVOpVptF1Q15086g9B2FQov0l2vCg6KLvtLt8JILKpfZw4q4IwY-YkR7NvvqvuCsdHB_IwAOWb0NcW1Ps4KBmFj1ltHHuafCSxTWmkDdw) The examination of the bending moment influence lines on the second support in both configurations provides an immediate explanation: ![](https://lh3.googleusercontent.com/5C3kQFc3-2uGBWWyfzJd2nSq8W5cHdsKEy6t5BV61ddpEPxTCvxS3fm9rO1CXSSW3vgAeC0WEWYQbqQWAHSoH8yliphZVT51RzVBdP5RQy-2km9l1uUn-jiu8iFc9FqpyHkTd817CwStv3JKqNq8Ig) --- **Example 2: Foundation mat** Square-shaped foundation slab modeled with shell elements. The nodes have 6 degrees of freedom (ux, uy, uz, rx, ry, rz). ![](https://lh5.googleusercontent.com/3ZpnPem5PHakcCEF4X3GA4lAkY5osTquMjL4exiam-s1gyhOr96Q6PnWwRlO5cePM_n9WOHr7VhKlxaoEWQwb2WklddnyI6m2pwHwNKiIG6U8pNdQxQW3b7zGiKUoY2i5Tbz156b78_83C61-Pkyfw) Because of its shape, it contains planes of symmetry. The following plane of symmetry was chosen as shown in the figure below: ![](https://lh6.googleusercontent.com/_rPw-5tTySg8-8-b_V2tPEWwtvWUp4c1dngnicHQXlZUqAgNfeNg-e49xLY0I5RxHMXIoUUeLoUxCJW6maHJlMV58jf242tzMGt6zS_OVxUzpzhhe8O69sKOc1e4hMPYl3qSPgoPok5Xhq_l0aFGcQ) The foundation slab can then be subjected to a loading that is either symmetrical or antisymmetrical. For example: - if a bending moment is applied around the Y-axis, the loading is symmetrical. - on the other hand, if a bending moment is applied around X in the forward direction, the foundation slab turns upwards on the side with nodes Y>0 and downwards on the side with nodes Y<0. The loading is then antisymmetrical. The conditions that must be applied to the nodes on the plane vary. In the first case, the nodes located on the plane of symmetry will be: - free for translations ux, uz, and rotations around y. - blocked for translations uy and rotations around x and z. In the second case (antisymmetric loading), the nodes located on the plane will be: - blocked for translations ux, uz, and rotations around y. - free for translations uy and rotations around x and z. It is important to note that considering the different types of loading, in this case, leads to creating two models differing only by the boundary conditions associated with the loading, which is not prohibitive. --- In the case of dynamic calculations of a soil volume, particular attention should be paid to the lateral boundary conditions of the block to correctly translate the conditions of non-reflection of the waves (see Part 1, chapter F.8). The definition of these spring-damper element systems is outside the scope of this guide. ![](https://lh6.googleusercontent.com/9YsE0WkRcrsoMHCa9MJfdEb-wwkKatkVlZJBNFRsLGuW_z_AdZG444GW7jEFTIiY5QdTGZ6m4oeyMZDc8IqSt1cf9Eg7W-7IWGlsG3CmovrLhJfjPllIHom4vWsLNGpsYGCz2cvqBvUD9XAsoRpUOQ) © doc PlaxisEven if computing resources are very powerful nowadays, the use of symmetry remains an approach that can be very useful for complex calculations and/or for large models. It presents several delicate aspects that need to be understood.
**C.2.6 Modeling of the foundations** Most of the time, the soil is modeled by support conditions (simple supports or clamps). Before modeling the foundations and the soil in detail, the sensitivity of the structure to the flexibility of its foundations must be assessed. If the structure is sensitive, the soil must be considered: - either indirectly through elastic supports or stiffness matrices, the parameters of which should be calibrated elsewhere. - or directly by modeling a certain volume of soil (soil portion + boundary elements). Note that this type of calculation requires special software. In the case where the reliability of the soil parameters is low and/or their variability is high, it is recommended to perform a range calculation. In some cases, having to model the structure with its foundations is a regulatory obligation. Refer to the NF-EN-1998-5 §6 standard. For more details on boundary conditions, refer to § C.5 Boundary conditions. **C.2.7 Modeling of bracing by bars**Beware! In the case of steel structures, some very slender elements (braces or cables) can only work in traction. If the modeling does not take this into account, the strength and stiffness of the bracing are overestimated for both static and modal calculations.
--- **Example of a simple braced structure** “As-built" modeling of a braced frame, but without considering the fact that the bracing bars will buckle as soon as they are put in compression: ![](https://lh5.googleusercontent.com/GOFIHFZJeFEfvaCgd97op3oh9-axHPsGQVn5zVaUfh1SY_kuQNoHqusMo5cLnvpksqeBgPw00_zXhqDovryit1c0E4r7E3fAL6NL3zgySa6cIhd1VqurATuM0LusuBpdo7776UkrBrK6YlWK6wFIbQ) In this case: - the horizontal deflection is 4.4 cm, - the maximum force in the diagonals is 321kN. ![](https://lh4.googleusercontent.com/VPf5kft_KDHcu2W9D2KO_zN2hCaHY2Swf99uZVVWC-S7jdbaSmQCDN81hFYqcGyXCPhkCqa3hFaFZaPk7Ef60INjSUqW5o9HnXUgBVXDFCvhxA4vry1LSkDfVFYPTw502UzDSRGMmLwDDPJK-xZWgA) Because of the buckling of compressed diagonals, for the overall behavior, one diagonal out of two should be removed, ideally those that are compressed, but this is not a requirement: ![](https://lh3.googleusercontent.com/P0qbufO-d_uqdrfj_-ZirTf3UCYNuJdr5ybqNSB3GCFxpBo1Cq8ZSEFCrRF5__QV9IzQT0ILNLxq_bXRIx1Mp8vJSyp6mWTsJWtN91O416kng8xHKInDOUubO33dx7wNOzbAiPjbpAe3jNHRLdKIFw) In this case, the displacement increases from 4.4 to 7.6cm. Thus, the stiffness of this pier is divided by 7.6/4.4=1.73, which may have consequences on the verification of deformations and the calculation of proper natural frequencies for the seismic calculation (Error of the order of 1.730.5 =1.31). ![](https://lh5.googleusercontent.com/mj0m-ZuVQDlii-vvCTFkuDiqs4hQHpMmx_gf-IU5-rU1bNdIUm7moyiyDIB-ffFJQ52oT_bChzImuN3nVUsgYzZOqW5QPF-rg7bxAw-JyEmm7Ovbheg0utJPUmtAa5EB4v9EShf_Zrqt9DlvfypsdQ) Consequently, the efforts in the diagonals increase from 321 to 641kN, which is logically about twice as much. --- **C.2.8 Structural Zoom - Local Model** For problems related to the local functioning of an element or an assembly of a structure, it may be interesting to build a localized model by imposing boundary conditions that reproduce the interaction with the rest of the structure. This is for example the case for spacers of mixed slabs, support zones of complex structures, or an arch/deck embedding in a bowstring bridge. Sometimes the entire structure is modeled using beam elements except for a part modeled using plate elements. In this model, which incorporates beam and plate elements, it is necessary to check carefully that the transmission of forces from one to the other is carried out correctly (for example by ensuring the sufficient rigidity of fictitious connecting elements). See C.6.7. ![](https://lh3.googleusercontent.com/okjN1nFjHet3XMeNc1qeS7oI9Y-j48lRjzPTfGPPb6UJx3o_DkOrpZnAFS3Fahw4XrH0eUmLwjK0gMbXjx2F0pLbL-H2kejPUpzjAoO0K5xNpU3fRByfo7tp1Czc87N0SNUhx8q0P6Byu5ZB9cgoeA) *Global modeling with beam elements (pseudo-volumetric view)* *![](https://lh5.googleusercontent.com/zjVgbhmMEsKQEuBCb-WyYHX_K2D3D5ptlzKbDhjDCsx67iX5z6Z3gVNK3rXTgN3rNpOg3nYHCt-dIwJME3tuIs5-OQPgk6JDgNbiKtWmzdsJZv2xxANLweCugHKc3tWw5PSxoo2AZPwn_vSGm4FCVw)* *Local modeling with plate elements (view of average surfaces)* # C3. FE and meshing #### **C3. FE and meshing** **C.3.1 Types of finite elements** First and foremost, the user of FE software must ensure that he or she understands the vocabulary used by the software: bar/beam, plate/shell, surface/panel, etc... [Part 1 § A.3](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a3-choosing-the-finite-elements "A3. Choosing the finite elements") is a theoretical part devoted to finite elements. Most importantly, the different types of elements are described. The user should consider consulting the manual of his software concerning each finite element to check its degrees of freedom, the stresses and deformations it considers, and if it contains the activate/deactivate option. The questions to be asked are the following. Depending on the problem to be solved, do you want: - the element to work under normal stress, in flexion, or both? - them to consider shear and the associated deformations? - them to deform in-plane or out of plane? **C.3.2 Mesh shape** The first part of this guide ([Part 1 § A.3](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a3-choosing-the-finite-elements "A3. Choosing the finite elements")) gives details about the different possible mesh shapes for surface elements (triangles, quadrilaterals) and solid elements, as well as the conditions associated with these different shapes. Here are described only the rules to be followed once the type of mesh is chosen. Most software have automatic meshers with many options to improve and customize the mesh.**The main advice is to look for the most regular mesh possible but to refine it where necessary.**
In some cases, and depending on the software used, it is more interesting to manually create the mesh. This way, regular meshes are obtained, whose numbering can be controlled, which facilitates the application of loads and the exploitation of the results. There are rules on the **slenderness** of the elements (the ratio between the smallest and the largest dimension must be greater than 1/3) and **on the distortion** (respect of the flatness of the elements). Distorted elements can affect the relevance of the results. For instance, for a non-linear calculation, if an initially highly distorted element is located in an area of high deformation, the distortion of this element may become more pronounced, causing the calculation to be interrupted because the limit criteria have been exceeded. Some software points this out. Moreover, there are rules to follow concerning the angles or **aspect ratio** of the elements. Some software can test the whole mesh according to this criterion, if necessary, by weighting it according to the relative surface area of the finite element. *![](https://lh5.googleusercontent.com/Rwv8dChhGhLDl-7lWdrswWEZzgrO2sGMhTymLkUIwT6UFIcIeEWAaUKqf0GFb9n3uNjIkmoxrbo3Bdz29Ibpfg_NvofElZWGbwlONefffzWEbMa2mcdoTMtDAUeuvIgZ_mjwHjgK7vZZXllpELzbAA)* *Example of detection of the FEs that do not meet a given ratio criterion* The aspect ratio of a triangle is the value 2Ri/Ro, where Ri is the radius of the circle inscribed on the triangle and Ro is the radius of the circumscribed circle. The closer the value is to 1, the better is the quality of the triangle. This is the case for equilateral triangles. Conversely, when the area of the triangle is zero, the aspect ratio is 0. *![](https://lh4.googleusercontent.com/wHWm2RvcqvSZxQxvAzBJfigNkYXQ110deWI3EUL8caIooE75hLqkCHzeaDCFSfr7ZXoQZm-0ORR5ioTxpgqn7hR_HB5ypzSudSOer3-9sWL7rvol7btpWdiqprrC-w5S-mWpovPHND885IfN6Yy4HQ)* *Illustration of the definition of the aspect ratio* Remember that a triangle is said to degenerate when its area tends towards 0. In any case, one must look at the shape and the appearance of the mesh. If the mesh does not look good, it is always possible to test another mesh option, to create nodes, or to cut elements to improve the mesh.**The ratio between the smallest and the largest dimension of an element should be greater than 1/3 and the aspect ratio should tend towards 1.**
**Example**: a parallelepiped of 160x160x160mm³ with one side containing a circle. The average mesh size should be approximately 40mm except in the center of the circle where the average size should be 2mm. 1st mesh: the modeling of the surfaces is carried out in an elementary way. In the first one, the circular surface is meshed with a mesh size of 2mm. The remaining surfaces are then meshed with an average mesh size of 40mm (in general, the surfaces are meshed in the order in which they are created). 2nd meshing: the modeling of the surfaces is improved. The meshing is controlled starting from the central surface. *![](https://lh4.googleusercontent.com/v9kJpyzWWkv7QjEyDdlR3Z3-6K7hZHfmw3jlePZmcKVRznWaps-rj9yOByZHX2trrnRyArjFPPwiIDp-knYREWs2UaxD2qTpqsUIQclsG-gn-8Ll84hOLRjHz_keMSu3MUkSEQcvIZnc0QrLi8CPTw)* *Surface creation order 1st mesh* *Elementary surface modelling = Non-regular mesh + degenerate elements* *![](https://lh3.googleusercontent.com/4P3ZnaTpLaGQv-JiMED_x7wwjjhdjx4DeT1kJKYTtegZ1ONj3aN_SbYE5Cnbmote_PM3PphH7OYC3u7kkwDbPI3qCYCxsrSNQqK_ulILGqaoZNNS9NRGW-zyJ9MLaeT1E6RptHoiriQcUYTVIHNKwQ)* *Adjustment of the geometry 2nd mesh* *Improved surface modeling + controlled mesh = Meshing and satisfying elements* *![](https://lh5.googleusercontent.com/wdvjdu-9PmOMwtC2EkTxZq6fyh0MHrfNMUtQ-tcdKr9ZY8QT95w8s_fb2vPAM-zgOpq_LjfeUzfrt08nHJmbExT2rRs4k_JkvJfj4rjCK81v9fSo3R51D84m3w6fs_BOFXJwRVqwZTi6aCh_0HizBw)* *Example of degenerate mesh*A good mesh is always "aesthetic", it should not be visually shocking.
**C.3.3 Mesh size** **The objectives of the calculations must be kept in mind when determining the mesh size.** Firstly, in a model, one must distinguish the elements for which results are expected and the ones that are there to reproduce the rigidity and mass of the structure.For surface elements and for elements from which results will be extracted, it is usual to respect a mesh size between 1 and 2.5 times the thickness of the element.
Larger mesh sizes can be adopted for elements where no results are expected. The areas of particular interest in the analysis of the results and those likely to have a strong gradient of stresses and deformations must therefore have sufficient mesh refinement and very few degenerated elements. Example of refinement of a mesh in the corners of the building via an emitting point (refinement of the mesh on a concentric approach) to apprehend the problems of thermal gradient in the floors: ![](https://lh5.googleusercontent.com/-e0eEL_ihDZTQ_rj56inkqBJjhled4veauAZZYCQkuekOXR1h9LvZaqHpirRT9iLlq3iP-iFRiyYc1d8CTRkP6Aww8UgWTW-aazKgzg51Ihvpao6T-xqn9YIJ9nX4IaEMKX0MAR7kImK-XXMWbtT0Q) It is important to ensure that the evolution of the mesh from one point in the model to another is gradual. When moving from one area to another, the mesh should not vary too abruptly. The size of the mesh must also be adapted to the capabilities of the software and the available calculation time. Before starting the real model, it may be useful to produce a model with a simplified geometry (parallel or orthogonal sails, absence of beams and shafts...) and to launch the calculations, to check that the software does not contain errors, outputs the results within a reasonable time and that it can process the results fluidly, especially if multimodal calculations must be conducted. A sensitivity analysis (by dividing or multiplying the mesh size by two and comparing the results - see the next paragraph on fineness testing) makes it possible to set the optimal size without mobilizing superfluous resources. For linear calculations of 1D elements, the problem is smaller because the finite element results are derived from the beam theory and do not depend on the mesh size. On the other hand, the display of the results can be misleading. A typical rule is to have a discretization of the order of 1/10th of the span. For non-linear calculations, it is usual to refine the mesh near the plasticization areas. For soil modeling in seismic calculations, a mesh size smaller than or equal to 1/10th of the excitation wavelength should be applied (see [Part 1 § F.8](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/f8-characteristic-scales "F8. Characteristic scales")). **C.3.4 Mesh refinement test** A test that is often performed consists of making two identical calculations on the same model, one with the refinement of the mesh improved by a ratio of one to two. The main results given by these two calculations are compared in the areas of interest. This exercise allows the refinement of the mesh to be adjusted to the objectives of the analysis. As the calculation time varies exponentially with the number of degrees of freedom of the model, the reduction in the number of elements can be appreciable in terms of computer downtime and memory required to store the results, if it does not lead to a loss in the quality of the results. Conversely, it may be necessary to refine the mesh so that the results are valid, but generally, this refinement will only be carried out on the areas of interest.The mesh quality indicators provided by the software is related to the shape and distortion of the elements, not to the relevance of the mesh size. The refinement test is therefore always useful, especially for large models.
It should be noted that there are a few software packages that have an adaptive meshing capacity according to loads and deformations (this option is rather useful for non-linear calculations). --- **Illustration** Example of the impact that changing the mesh size has on the results of a floor slab analysis - from the top to the bottom, mesh sizes of 20, 40, and 80cm, respectively. The maximum shear which is equal to 0.92MPa with a mesh size of 20cm increases to 1.49MPa with a mesh size of 40cm and 1.22MPa with a mesh size of 80cm. ![](https://lh5.googleusercontent.com/f4h9EN-9CgyI6GaTOlpJuQ4w-lKjJr1tAss76rnBPC81Cz3-Uzj9BhHID44FZPuDCNRB0_D9c-HaxcrhsivGgm3K-vxWTOhErm_2EGp5WDI7GllnmBqYPGGDAADT6320T-gnW1wmHETu3YzJ0gjZLw) ![](https://lh3.googleusercontent.com/mEez3cvpCtyuN2yMkXX2KhKZM5syrXh-0YEKke0oxr1ZyDAB3N6D6yjgkUyolq3P-E3ZWPlvbuFuABgr66Ikyxuch896n3s7cnyZYBsYPVTnz7jgv1A-YrfZnFScjmo6BYEQg3E07w23MoTCJUV3eQ) ![](https://lh4.googleusercontent.com/q59Fn9WbPqzfh9t5RC1h0N_ZnYC5o7xfPS11bnlcJpCHHxU47jpqDC7_9INjhX2nMLobr4efO4HnpHT3Lgbq2sk91-mijAkscxxEtLaSs2uyv4DUxXUD1Q_Bhud8MoZCOilYwDa2oU9OzBgAGp6inw) --- **C.3.5 Orientation of the local coordinate systems** The orientation of the elements has an important impact on the post-processing of the results. Verifying the local coordinate systems should ideally be done before introducing the model loads, as these might be referred to as the local axes of the plates. In the case of 1D elements, the X-axis of the beam elements is usually directed from the "origin" point to the "end" point, with the Y and Z-axes being in theory positioned in any way relative to this X-axis. However, the position of these Y and Z-axes must be homogeneous for elements of the same family, on the one hand, to facilitate the application of transverse loads (e.g. wind load), and on the other hand, to read the extreme fiber stresses which are defined by the Y and Z translation of the neutral fiber. In most software packages, the local axes of the elements are oriented by default either with respect to the global coordinate system of the model (alignment of the local Z with the global Z) or with respect to the order in which the entities are created. It is always possible to force a homogeneous orientation on a set of elements. Similarly, for 2D elements: - the outgoing normal must be known when defining load cases (earth pressure, fluids, or temperature fields). - it may be advisable to follow the logic of determining the outgoing normal, both for the input of the concrete covers in the case of a reinforcement calculation, but also to direct the element beforehand according to the assumed direction of the reinforcement to be installed (or checked). One will try to follow the same logic for the whole model (e.g. upward normal for all floors) so that errors are not induced in the exploitation of the results. - a uniform orientation also helps avoiding discontinuities in the display of stresses for a given fiber in two adjacent plates, for example. --- **Example: Plate and local coordinate system of elements** Subject: the direction of plate definition can, for some software, generate the orientation of the local coordinate system of the elements. Example: Plate 6×6 m² (modeled with 2 plates of 3×6 m²), supported on 4 sides, loaded with 3 T/m². *![](https://lh3.googleusercontent.com/dc6LzDYQgY7GRoTFqrowitPqGp-5kAWhRyiOSB7WBTfsKUnOjtLFMz9ljr27bxeyOQ_DNvO90mxkomQ5X4XuTpPTRqjTTKhPLeiDxCc0WcnD88JU1_rkfesIOhM1NB8L7vOCwAqwH2s-HEEeC-h6Vw)* *View of the local coordinate systems of the elements* *![](https://lh6.googleusercontent.com/y7C7RuWDGnU4Wo_pL-sjG66rPZ4703NfnxaWmti8xNUPemvsS9gYwD5ReSp89Ck7MNgzLsKyEF1CljS9PKtXLs-0Czy4fYiAjKXahEngXZM7x8wASRUzgt9oqgzOiWwTbnWt16n95x09UBA7ax6nIA)* *View of the bending moments* Then, there is a sudden discontinuity of moments on the connecting line between the two plates. This discontinuity, which has no real origin, is solely due to the change in orientation of the local coordinate systems. In particular, the change of orientation of the local coordinate systems as shown above will be a real problem if the software is asked to calculate average forces in a given cut-off point... ---Check that all local coordinate systems have the same orientation.
**C.3.6 Model size** The calculation time is often a determining factor in the cost of the project. Therefore, it is always interesting to try to optimize this calculation time. The calculation time of a model depends on many parameters: - the number of degrees of freedom (number of nodes x DOF). - the performance of the machine. - the software performance (algorithm, parallelization, ...). - the amount of data saved (temporary non-linear calculation). - the type of calculation (linear - non-linear). Depending on the software, it is often possible to optimize the amount of data that can be saved and the number of degrees of freedom. On an ordinary project, a model will run at least twenty times. Any gain in calculation time is appreciable. There is no need to systematically save the result files, especially if the model runs in less than two to three minutes. These files only clutter up large CO2-generating clouds. **C.3.7 "Merge" or "Combine" option** Most software have the option to merge nodes or geometric construction points that are very close to each other within a tolerance set by default or by the user. This avoids mesh discontinuities. This operation presents certain risks, particularly in the presence of expansion joints or the absence of welds that the model could ignore. In the presence of joints, the user might choose between: - representing the joint with its width (modeled distance between the 2 lines defining the 2 edges of the joints). This is easily visible when manipulating the model and less likely to be "merged" by mistake afterward, but this may lead to elements with heterogeneous sizes (associated with the size of the joint) if the ends of the lines do not meet, - placing the points and lines in the same position in the model but modeling them independently. It is then difficult to check that the joint is well represented (unless the node numbers are displayed later) and node "merging" operations must be carried carefully. - use the linear release features offered by some software. The merge operation may also impact the node links. Therefore, the mechanical links between nodes must be defined after merging. **C.3.8 Group of elements (for visualization and later processing)** Most software offers the ability to define groups of nodes or groups of elements. This feature is very convenient and facilitates the assignment of materials and masses, the application of loads, or the post-processing of results by elements of the same family. **C.3.9 Reading points for results and meshing** The points where the results are read are a consequence of the verifications to be performed on the structure. The needs of the study may require several points for calculating stresses on the same section (for example for normal and tangential stresses). The calculation mesh (i.e. the set of nodes) and the points where the results are read (sometimes different from the nodes) should not be confused. Having many reading points does not make the mesh necessarily sufficiently precise. In the example below, the multiple isolines of transverse moments, especially near the supports, could make it seem that the calculation is accurate, whereas the mesh is too large to obtain reliable results. ![](https://lh4.googleusercontent.com/5vvDncsKfCwyI_dIrdAYAbBtC7TlVdVW5ORUjSBs29nnRaoSnMqVDMM7tAK9nQd34CKnf0qYoA6mWHB4yDcq0kypV76SHamAVnG55PP0uS4kYzv3ge54eCm17VRYMLRRLNqAv5aOThrpbGwpttMN2w) Indeed, the reading points may give the illusion of a refined mesh even if it is not the case. The results on these reading points are interpolated from the results at the nodes. By plotting the bending moment and edge diagrams in a cross-section, this becomes clear (the slab is seen from below): ![](https://lh6.googleusercontent.com/lwYEq_nHq7flUIqE1bqE97LjS2wxinoar2i4cnNXYi_h1IQH7IkO-Olw3AHvWMjnVUczLvTmkafrtxS3pEZKqDlire5l_l9xyV8slmM6cu5s2V7f9AeFPVbkPky877l9gXvCVldQDxgRWFd1QLyZOQ) By refining the mesh, the graphs become: ![](https://lh3.googleusercontent.com/1FUlUof1zpqpF5EpvFGgpJWUxgN782pms9aJl-9W384L2lkW9ROGV5bDpcKn1_0iFlZK8nSG7-_SMo5vrqCKGTqJXJosdWcy6XgKqk3FLlBAOJmh2k0pMKl-jXafzO57-LBh1ktjrHvhuNRB8iSPiQ) ![](https://lh4.googleusercontent.com/7IrYBFrZBD5bXPRuyDJ0bU76E-LZL6ez9j8US4KVTvvDyoyZJS7ninQmNj2zF4RVYSOqc8HLXdiWtbpUug7pIi-mCpJ0JhTjDmrSVobU0sX6P4HjO3ol4aCmpsAv8j9ZBe7yNdPw5H3M7gSGDcBPJQ) As soon as there is a singularity, in this case, the support line, the size of the mesh plays an important role in the accuracy of the results. You only need to refine the mesh to see this: ![](https://lh5.googleusercontent.com/3Y27uSze5wCTUavRE6dJPSTW7EyEUrZ-VPdf-THQv-5hwlUQqm8NOYfpWlogO_xDNSW9nCScfR-pelXIKSxZFtUQDWyrGzzt7ZDE2CSnQkOQneajeUT18PMj0ay9ixd_22emey49xowt5SrSYsQleQ) The calculation of the integral of the efforts shows a strong impact (in this example) on the shear efforts (deviation of 22%) and a very weak impact on the bending moment between the coarse and the refined mesh area. ![](https://lh4.googleusercontent.com/ttFF45dWTmqOXt-SOF4cLOByhrA-aSca8D1askMuUoESQw6OjLlBAzmMU1_IWQGBkI6LYRvxMwDt-vNggU88nQ3ZenTrGv5lzHupjfDK201vVV3J_9upyE6CaihQForbN-xzXnsZVrjf5TUO7T_Pgw) *Integral of the shear efforts - plate with two single support lines* *![](https://lh5.googleusercontent.com/Q5lLEBPd1iBHmVHD_un_avy1WBus_sd8zyammkbO_zQX88_NmjNAnPBuvIUthZhHCeKLwuOrA2z6mfmiOAKoVl8pOg3eXGo7hTspTN8qN5LrElRENKzuhmBvMNN581ewnXTjz2xO0Kv72VvlkLzstg)* *Integral of the bending moment - plate with two single support lines* It is enough to create a singularity for the moment, by clamping the edges, for a deviation from the moment to occur (of the order of 17%) *![](https://lh3.googleusercontent.com/kQw5RM1-uiBUjz0svcDPEk2QPOAcaBwHKWp7y5h0tmMZ359PwfY51oWbnrKkim93QXeLg7w54dlW5EUDuTiEMCdS2cgZQ0mdVzoVGF-SLRZRVQ9mONhdo_x62yBsckyY8urkLPYYVbH1sZF593M1LQ)* *Integral of the bending moment - bi-clamped plate* # C4. Modeling the non-structural elements or equipment #### **C4. Modeling the non-structural elements or equipment** Non-structural elements and equipment are elements that do not play any structural role in the behavior of the structure. Three cases can be distinguished: - The element has a low mass and a low stiffness compared to the overall structure. In this case, it can be neglected in the model, - The element has a low mass but its stiffness cannot be considered negligible (e.g. some facade cladding restraining the movements of the supporting structure). In this case, its presence can modify the behavior of the structure, so it is necessary to consider it in the model (at least by considering a fictitious rigidity), - The element has a non-negligible mass but its stiffness can be considered negligible. In this case, an equivalent mass must be included in the model.**Equipment/Non-structural element** | **Negligible mass** | **Significant mass** |
Reliable stiffness | Not considered | Mass to include |
Significant stiffness | Stiffness to model | Mass and stiffness to model |
Be careful: the slab is loaded only in Z, but to ensure the stability of the calculation the translational motion in X and Y and the rotation around Z must be blocked. In this case, 2 points were blocked in Y and 1 point in X. (NB: stability in Z requires a minimum of 3 non-aligned points blocked in Z).
In a 3D model, an embedding means that the 3 rotations and the 3 translations are blocked. In practice, without giving any choice to the user, the software can proceed in two ways to block the displacements: - A method that is always numerically stable, which consists in suppressing the DOF in the solution of the problem because its value is zero (see [Part 2 - A.1](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a1-what-does-the-software-do-in-a-finite-element-calculation-the-example-of-beam-structures "A1. What does the software do in a finite element calculation? The example of beam structures") - in this case, a 5×5 matrix is used). - A second method consists in numerically placing a very stiff spring in the fixed direction so that the displacement is numerically close to zero. (see [Part 2 - A.1](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a1-what-does-the-software-do-in-a-finite-element-calculation-the-example-of-beam-structures "A1. What does the software do in a finite element calculation? The example of beam structures") - in this case, a 9×9 matrix is used by adding terms of very different relative values). It is important to understand how the software proceeds to be able to detect possible numerical instabilities that can lead to a halt in the calculations or unbalanced results. **C.5.2 Modelling different types of supports** Generally, the supports can be considered as fixed, except when the ground intervenes in the behavior of the structure, i.e. when there is a static or dynamic interaction between the soil and the structure (SSI). For instance, to model a soft ground generating differential settlements at the supports, or to define a seismic behavior. Structures are based on three types of foundations: shallow foundations (isolated or spread footings), foundation slab, or deep foundations (piles, wells, bars, rigid inclusions, ...). *![](https://lh4.googleusercontent.com/BciKdZPfFTPVzjA6G8MCfjGggnP8bNcz4lQZUVmriScSIBGcGdy47EMg7UIILSreQf80Es6JiAppasjpmYlJ06EIRk0zAjYSE3q35c1ebGIdvdzNnYY4eQcbx_6TAwYLhytqAZB4rqdndYGmkeZ8_Q)* *Illustration of shallow foundations, foundation slabs, and deep foundations.* **C.5.2.1 Shallow foundations – For supports under columns** Shallow footings are modeled using punctual supports. They can be modeled in 3 different ways: *![](https://lh5.googleusercontent.com/gLe8fcUizX8Z0b96KQQjtcmlp6qfu93iJJFMrMrt4M7siBtI2PkvGP_rz6AfA6t6NUMQaJaBWKoBX3nWb7NgHp0eTC8GQxIxMHd3lk8Hdlk45rDfWniJQjRv7n9NMIgkdzadcq-PBnf0H00XZkChQg)* *Illustration: clamped support, hinged support, and elastic support* Clamped support: the 6 degrees of freedom are blocked. Hinged support: movements are blocked and rotations are free. Elastic support: the support is defined by 6 elastic springs (one per degree of freedom), or stiffness or impedance matrices. Stiffness of the elastic supports To calibrate the stiffness of the elastic supports, the stiffness at the interface between the footing and the soil is required. This interface stiffness (usually denoted kv) is taken from the geotechnical report. The term Kz (static stiffness of the spring against a vertical force) is obtained by the formula Kz = kv x S, with S the surface of the footing. ![](https://lh5.googleusercontent.com/4N-OB798_44DpKacQ830X2ARBJehxLUbNeOYoDi37kyedxMcyUAJsRwfBVz1FCc1Q_C9W80gzUlO20bcVQz4A98C6IEuKcC0TmO208hOsP0vkGutYfpg7ffpD4O6-PxEXu4smuZYeUORoFHH2gteeg) The terms KR are deduced from the formula KRi (in N.m/rad) = Ii x kv with Ii the inertia (in plane) around the axis of rotation i of the footing. For a rectangle, we will find the terms Iy=b.a³/12 and Ix=a.b³/12, a and b being the dimensions in plane. ![](https://lh5.googleusercontent.com/qAUxc7_9ioCqtYqlDS_DebTJ1Eq66QBZUCXnmPX-FybXvCGxaKpDg94U18RkVvw4wo9UCGNuXitTQA7SmoCVXlqwVUhdRv2hX_FbN-NKkM8tIH1PO7-9E9dqsiRL-Di4cOim-i8otMnpox_Mj6EtbQ) *VIEW IN PLANE OF THE FOOTING* Particular attention will be paid to the notions of long-term, short-term and seismic stiffnesses provided by the geophysicist, which differ significantly. **C.5.2.2 Shallow foundations – For supports under thin walls** Thin walls are generally modeled by plate or shell elements. Two types of models can be defined for the support. **Method 1**: By defining linear supports distributed under the thin wall. This case is similar to that of the columns (see above) by distributing the punctual stiffnesses linearly along the wall, or to that of foundation slabs (see §5.2.3 below), but considering only one direction of calculation. ![](https://lh6.googleusercontent.com/1CpIvIn4sbIagt5Q8Pf2CTosELey9fuqrwsGLNdmV14oo52qBj4obuqeMMBh-3HnlaLW-sdhwmBoeD8T1XKYsUuw45B2n1d1h1C-XHIQprOO4BcTNBLpa3cPuQgmSfruFiIlo5Tgtr_yj5yEsfKCCw) **Method 2**: By modeling a single central support to recover an overall torsor at the foot of the thin wall for designing the foundations. A rigid bar at the base of the thin wall is then necessary to distribute the forces. The support conditions are identical to those of the columns (embedded or elastic or with stiffnesses). ![](https://lh6.googleusercontent.com/YHqjqimK7Cpf5p4vHfOMw3vL3TTuDmWu8BBD-ulQ-LQFSC0Q-F5qC8131uA9KGraDRLEL01uLl-So3-BKZVFvtnV-aode25QTXH-HzE2af0CHow0XDEuFOqac_H7n725q3F_8ooKBNsQ0TMnuywwmA) In both cases, the units for the introduced stiffness should be verified to remain consistent with the physical units provided by the geophysicist: are they N/m, N/m², N/m³? Is it also N.m/rad or N.m/deg? (or derived units: kN, MN...) **C.5.2.3 Concrete slab foundations** The support of the foundation slab on the ground is modeled by placing springs under its various nodes. The spring stiffnesses are then calculated according to the same principle as for isolated footings. They can be differentiated according to the loading zones. Be careful, the stiffness must be proportional to the surface area of the node (a possible issue in the case of an irregular meshing, if this assignment is not automatic in the software). Some software also offer "surface" springs on plates. In any case, one must verify using a unitary case the good concordance between forces and displacements. ![](https://lh4.googleusercontent.com/RtwTouJT_C7e8avaG1dYgUoDtadj40pxTbdfe-RDrT53zthb8QajyoZyfTjoYX0zu6_dz0ODU62quU-iAecAMDlIFAG_SiGPUXTv7fUXrcwEnTiwXu3u4_U1U248RB047Ueq4jttf5GuLdRSv6fAng) *Soil modeling using a spring system* In reality, the horizontal stability of the foundation slab is ensured by the friction between the concrete and the soil, and a possible lateral abutment. For the model, either horizontal surface springs under the concrete base or springs on the periphery (punctual or distributed) will be chosen, depending on the internal verifications that must be carried out.Caution: for models with horizontal surface springs, the horizontal stiffness is related to the friction between the foundation slab and the soil with possible slippage. In the case of a shrinkage study, an overestimation of this horizontal stiffness will artificially constrain the invert and may generate significant and unrealistic tensile stresses.
**C.5.2.4 Pile Foundations** Pile foundations can be modeled using 3 methods. *Method 1*: each pile is modeled using a beam on an elastic soil (or elastic linear supports). The horizontal soil stiffnesses depending on the characteristics of the soil layers (Kx and Ky) are generally determined by the geophysicist (pay attention to the mesh and the concordance of the units). A vertical support is positioned at the base of the pile to represent the point stiffness. ![](https://lh3.googleusercontent.com/0OfdGmilbTTpPKx7BticTLUM7lRjHFdExilCn6Grm1KqXe-LznMqu5c57Jr4fffM3ekD3zz_pQr0FfEzOf7dArvmh4ig2A4stfDBjjB1IwxdLiYrWy_J61sADpsSAjWkR5zQs6rr8xvRJvh2LUrLaw) *Method 2*: (intermediate but little used) each pile is modeled by an elastic support (or matrix) characterized by 6 stiffnesses that are generally calculated by the geophysicist. ![](https://lh4.googleusercontent.com/AE3YRp4nxnX0CZ749FVqz2Y0kv_3hlLNu3FvvO1eYZY2uAIT1RDXXEHTz0aOIRg76VOqiVF3ROD12osg04BDur2pg-q6dGld_GgwdxAQd6R_41546aA0tB1QAI5aJopn13gUqWA0y1gB_4S61kB1JA) *Method 3*: It is possible to replace a complex foundation by its stiffness or flexibility matrix, which integrates the overall configuration of the footing with the set of piles. The foundation will be modeled in the general model by an elastic support at node A, whose 6 stiffnesses will have been calculated beforehand from a local foundation model. See the example below. ![](https://lh4.googleusercontent.com/vGTCy8A1-uwsSPxPPtKEpA8vesgenRRuMFVGAx7epHbc0yY3rlNwjPytZMiNPNyrc48vUehTyM2zC3kXyG9LItB_dnEJ0OfeXwhF56SC5AXx3lRix0sEpRqXn1LxIkZVfXnUEatGxmPr1awbzOL3Gw) Because of the coupling between horizontal displacements and rotations in deep foundation systems, there is no apparent reason to neglect the cross-terms (non-diagonal) of the stiffness matrix. However, very few software allow considering the whole matrix, which is a problem. It must be demonstrated on a case-by-case basis that the "diagonalization" of the matrix has no significant impact on the stresses and displacements of the structure. Methods 2 and 3 allow the size of the model to be limited, especially in the case of many piles. On the other hand, the first method gives the stresses in the piles directly. More generally, in global models, piles or groups of piles are modeled by springs (method 3). It is only for designing the piles themselves that one may want to model vertical beams with springs (method 1). Specific software can also be used. In any case, it is important to remember to include in the Kx or Ky coefficients all the normative requirements such as the group effect. Finally, if the piles are calculated by an entity other than the one in charge of the superstructure model, iterations may be necessary to achieve the convergence of efforts. --- **Example of calculation of a stiffness matrix.** Data: 1.20m diameter piles, Concrete Young Modulus E= 30000MPa, Ksoil= 6495(kN/m)/m, footing height 2.00m. ![](https://lh5.googleusercontent.com/uaRx0tmj7r9lyGjsPhB1ctoPqW-BWBrKc7WpmeKGL8uMIVkpn8scqFoz--E7vH6CV4HK38Ty5tyu_5akhdVMa_TrOpDgvDFZKXxtMEH3axYKRHDWLjW_m8nj4724gZBqT9L9q0IWp82JYHwxVhRYSw) *Geometry* *![](https://lh3.googleusercontent.com/KY2kOZT28_rwmmDEXAF5uMlN68FP1sPUiIt-YDvg5Pqxfd10QFFtn2kRyjM8HxGq8blvsFdTYb-DuWm2UOYMUlW6ViMs6u4H1NXF2jwd2L1I84yhe7vCw-DBBoKNC5m2RNNNvWREihP1aBhTd35vTA)* *![](https://lh3.googleusercontent.com/Ov7Q-Kr1VZQyBr8E7UvOv3eq1GCk5Ne6kUiw5tuBPWEHUg06Ta8moqzeuLnAk3M24rKa0ybnrZK314hkknWG4t7hZQ_aSwf83GfRHqmutmn8MjCcThQE4Ce1VBNgi5TI9Exnao_hBDC8KLu2Yuugvg)* *Unitary results (1kN or 1kN.m) introduced* Results: ![](https://lh3.googleusercontent.com/sVXne_34uXM9LwwA_2FWxUMm4zFyotVx36Xl5tJvei2jVwlEoo5lQbPpO9q8xkhqokLBBMmUtLe99roDLUHEYSff7E2OMPhlyC44vs42FhEPVvksF2yeUM41BS4qg8AmUb9hhAUqBhFRJf61vl_pUQ) *Displacements under the loads = flexibility matrix \[S\]* *![](https://lh4.googleusercontent.com/fL6VkqzQanlp9A7FcsWb2emrbiba23ZYQ8M9Su1R4tmHXyIyMuFyZOXW5f72EL4EfjeCA8PfX1dDQcNuX1a0BNOAa3-eXDjM2uuknbN9LDfTCRv6ytN9UTjCEHXs1CVuV8d_cHjOYj37CjDTaLAV1g)* *Stiffness matrix \[K\]=\[S\]-1 - (units : KN, KN.m, m and rad)* (The matrices are easily inverted using a spreadsheet). An indication that the cross terms were not considered: a pile of height 10m and section 5.00×1.00m², E=32000MPa is added to the previous model. The same stack is modeled with a 6-component elastic embedding, which are the terms of the diagonal of the matrix above. A force of 1000kN longitudinal (respectively transverse) is applied at the top: ![](https://lh3.googleusercontent.com/ogFbG3fLXF_msjqZ7A49i1IoT-tmQNA0bOwtUkTHQ3GLF4ivsydRrFUynycgL89yRHTEN-HY7MEj1zG_69QJEXoM5Iuz3gIdA-QgRsCpgKsekC-tjbsnqfyCPlqggZW6358sUnnwOZhguSP1S3Bq9w) In this case, a deviation of about 13% on the longitudinal displacement (respectively 17% on the transverse displacement) is obtained - the flexibility of the pile comes into play but it is identical in both cases. It is up to the engineer to judge the impact of this possible simplification. --- One of the topics that must be addressed in the general hypothesis report is related to the simplifications that will be accepted or not for the SSI calculation. On the one hand, they are related to the consideration of the short and long term modules of the soil (ratio of 2 on K) and of the concrete constituting the structure (ratio of 3 on E). On the other hand, they are related to the constitutive laws introduced for the soil (linear, with several slopes, with a possible plasticization step). Depending on the software used, wanting to integrate all these factors can be very complex, leading to the assembly of several differentiated models and the need to carry out certain verifications manually (replacement of plasticized springs by an equivalent force, for example). In some cases, it may be interesting to perform a range calculation, distinguishing between resistance and deformation verifications. *![](https://lh5.googleusercontent.com/iZ71p2QdyUq7e_A8z0VQfkC8wTBrEOoddHorg7AS6bhqSyM8hKknxIy4rIYuoM89gqyOJX-OkvsCyxZtwCZ1rBQ8Er2KEQHFnbauj2T7z1jb8vO1TM1OCmp77WwXUpmlrC9lmwtl-mU0ey0CGzCS5Q)* *Illustration of the complexity of the constitutive law of soil springs* **C.5.3 Modeling of support devices** ![](https://lh4.googleusercontent.com/NpbkNq1TeSCv3a9vYrZTePvgluY40mtfLFjM8NSKEO4k5NhYnBELiOfbue4GC5JBdZnuU3N4eznqciYk1DdyWuK3sMzilQpHo_-w3VIPF6Ltu21tAZL5gAkM1S4IEfdeMFuo-LHXK1JYY0Q32SSZ0w) There are two ways to model the support devices of a structure: - either as a support, with the degrees of freedom and flexibility parameters of the device. In this case, the support reactions are recovered, - or as a bar element with several modeling possibilities (described below). In any case, the support devices must be placed at the real location (transverse and vertical offsets), otherwise, large errors will occur. It should be noted that the behavior of the support devices can be a source of non-linearity (sliding supports, for example) and may require a de facto non-linear calculation. *![](https://lh5.googleusercontent.com/NuDK9GN8wugD8Jq-ex_Td3wxu1IToOb9adc87d78V0EQ8B_11_Oa8wgoYe3ZEuKdbBBLc9tl4ocdG3Fcgf8txiFy2pEU0c-O6agQFokwHvUNZljEnpB7c5fHUuNKGJfFCZis3_UtcsChhxCevq-i4w)* *Example of a bridge pile model including the elastomeric bearings.* If bar elements are used, there are several possible choices: - some software propose elements resembling connections that can reproduce the characteristics of the bearings (it is not strictly speaking a bar), - one can also use "spring" elements between two bars, if the software allows it, - one can define a "shear beam", i.e. a bar that is very rigid in bending but with a calibrated deformability to the shear force. The software must necessarily consider the shear deformation (option not activated by default in some software). It is defined for this bar a weightless section, an elevated inertia, a strong straight section, and a section reduced to the shear efforts, allowing to find an equivalence of the support device (for the GS/h bar ⇔ G'S'/T for the support device), - finally, we can use a classic bar, working in flexion, embedded in the bottom and free at the top. It is defined for this bar, a weightless section, a section reduced to the shear efforts, and a calibrated inertia is then defined to have a global deformation equivalent to that of the apparatus (for the 3EI/h3 bar ⇔ G'S'/T for the support apparatus ). ![](https://lh3.googleusercontent.com/toJJBs05LHhpbPrgH_wvEgysRCs_m4rL1pqVKN0EHC0S_y5XQ5pTtkKj1fqUm-0gD9cZWnshqnDtWAzYcgPwNxXokCZvaPcsrZjwhwN8-Ie00a8rleejHCy3owaAA1-yVJVzBTc4C6bVJcayhN70PA) Regardless of the method, **the element must have an overall behavior equivalent to the characteristics of the supporting devices**, as defined by the standards for supporting devices (NF EN 1337 series) and **it must not introduce any moment neither in the deck or in the pile (other than that related to the thickness of the device).** The illustration below shows rigid extensions allowing to model the top of a pile supporting two isostatic spans, simply connected by a flooring. *![](https://lh5.googleusercontent.com/4iGehOOmH3fAInLAtcS149RNhW8oV6kzNOwN4N53pCi_lmom1qI2oA_n0b81tE-ud457J8ahqSGfV_eK_x6Y9MonaPXkw4eBn6WIrY9LxsW2Sihhs8hd3I060EZKHsWZe-uYeoTEJ4HDwSYmImHAtg)* *Modeling details of a pile supporting two isostatic spans* # C6. Connections - links – assembly #### **C6. Connections - links – assembly** **C.6.1 Releasing the bars/springs/degrees of freedom** In all models, the default connection between two beam elements is perfectly fixed. However, it is necessary to be able to release degrees of freedom on some connection nodes between elements (beam-column, sliding plate). Each software have different functionalities to do so. It is important to rely on the software's manual and to check, with simple load cases and with static or modal deformations, that the behavior of the connection coincides with what is expected.Care must be taken into maintaining the stability at each node such that not all the bars arriving at a node are released in rotation or displacement.
**C.6.2 Mesh continuity** Sometimes the number of elements on either side of the connection line (or surface) is not the same. Thus, there is a risk that only the common nodes (in green) are considered a connection. (figure below). *![](https://lh3.googleusercontent.com/ZaPivIoqvwwzQ46pD-c8iIrl2Q0YCqI7yZjKUcIb_AJ0HOYZ4rIx914A0b22KmGWJgUFN5fnA_jt2ew7g4pY6Q4D8uZ4kCJEF-RxgcijiUQ-qdfpOKQUqgIwH8JVQHzqDkJfdr8xvHKWV4FIHa3xmA)* *Bad connection between finite elements of the same type and DOF* More commonly, a transition zone can be created using elements containing the same DOF per node with suitable geometries (figure below). *![](https://lh5.googleusercontent.com/KA6GSZR0ynPToIW9TnTloNY4uSZwrzkSYDX0_UMrWq1gefs8i3TbgMYKfCZJGOPQiWr89NOkI2Kmbw4bUX-OdLYfHjcbIhGHmtX0lr8-JlKIDSvGjjgNamI0KL6Ok8sxoyPDcQWcF0f9cM00qHp-HQ)* *The meshing of the transition zone* **C.6.3 Connecting different types of elements** Using elements of different nature in the same model introduces complexity and one should always question the necessity of mixing the elements. This complexity arises at the connection between elements of different natures. They can be beam/shell, shell/solid, or beam/solid connections. Particular attention will be paid to the possible connection of different types of structural elements: element with 6 degrees of freedom (UX, UY, UZ, ROTX, ROTY, ROTZ) / element with 3 degrees of freedom (UX, UY, UZ). This type of connection can cause the appearance of instabilities or unexpected joints. Several software packages compensate for these difficulties with specific elements capable of handling these links and degrees of freedom problems. This should be checked and the relevance of the local behavior of the model should be verified. **C.6.4 Connection between a bar and a plate** There are three cases: - either the beam and plate elements are in the same plane, - or the beam is a rib of the plate, - or the beam and the plate are perpendicular. **C.6.4.1 Coplanar Beam and Plate** For a bar element connected to two plate elements, the transfer of moments should be ensured by means of additional elements, or by the introduction of stress equations linking the degrees of freedom. In the illustrations below, in case 1, there may not be an accurate transfer of moments and nothing forces the bar to remain perpendicular to the plate (intrinsically the shell nodes cannot block axis moments perpendicular to the plane of the FEs). Case 2 consists of imposing an equation that links the displacements of the plate edge with the bar. This is a reliable method, but it is not proposed by all software. Cases 3 and 4 consist of adding rigid bars to reproduce the displacement dependence between nodes. Special attention must be paid to the definition of the rigidity of these bars, which can be a source of instability in the software. *![](https://lh6.googleusercontent.com/kpjNuAZpzqz98FgKjo4aPiSpfjz-HP0duTn3afKCtuDlPKSxs_C7wjPsvW_qFwyQqEba2g1KvlN3qXm_VHSUSr3NpG1WQBqrOanI7Vv9jGVrPiLq0DxHrHV-kSLSsgGOq6IBAAIw32IqWuD9s3kY-g)* *Connection of elements of different nature - Moment transfer* **C.6.4.2 Connection between a bar and an out-of-plane plate** The case where the beam acts as a stiffener associated with the slab as in the case of ribbed slabs is discussed in detail in [C.8 Composite sections (beam/slab)](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c8-composite-sections-beamsslabs "C8. Composite Sections (Beams/Slabs) "). **C.6.4.3 Connection of a bar perpendicular to a plate** The last case is that of the column-plate connection. The big difficulty, in addition to the transmission of bending from the bar to the plate, is the transmission of torsion from the bar to the plate. By default, the plate does not have a rotational DOF around the axis perpendicular to its plane, so it cannot take up the torsional moment brought by the column. Therefore, it is necessary to find the right kinematic connection conditions. To ensure that the bending and torsional forces of the bar are taken up by the plate, it is necessary to have rigid connections at the junction (in red on the diagrams below). ![](https://lh6.googleusercontent.com/Jf_-H1CyaZiAqGPh2t1GbA1Pj5rvwBsO3idmgrGRgzWpw6HNDoSY9wfZxZv7aKvbnLoBS3-BznFoZle-J87auF_jqz43ckO7vtO_locf4wR3_t455xzxFZrdX8mlB7iMEI8M8mXcT8l4djgtRRZF7w) *Modeling of the bar-plate connection (deck supported by a column, seen from below)* --- **Example of the column (1D element) embedded in a plate and subjected to torsion.** Illustration of the consideration of the different number of degrees of freedom between elements of different nature. ![](https://lh3.googleusercontent.com/rZ_ciWB_FRc7FSRowp4kuK2Z332dzkJUlzOmq5Fu5zcoAqGhMBROwxbHgGsJF2TaptFeis6yoSeBTelv6KgZw-iOLyp1lihAWoW-QMUqxxy0rMkm0VC4Tp34k_uqifQGkbQBSGAJHmFNlAi2S9xFDA) The model simulates a 20 cm thick concrete plate on which a concrete column of 1 m diameter is "embedded", simply by connecting the lower end of the column to a node of the plate: ![](https://lh3.googleusercontent.com/HAqyv-NJ3jR-QQbZN6aYeBm5r37MhXwVBLVvsMuVmIwiMg_tKWygskgaoIh5NP4DntNAbtOlvhIoaO5Vlp5pLv5OSPRQ8jG1T-wbWKXHnd-_3dXpzYSalNhe95GaT7pv2ox4RNXMkcC078OA_kjwfw) The horizontal translations are fixed at the corners of the plate to block this torsion. The torque introduced is 10 MN.m. The results are as follows: ![](https://lh5.googleusercontent.com/WuggEYlcJKtls6aIa5wZWfl_Zm-thOMfnPi3c4Uoqv0Qv77gTAaUbuLbRmorie4Xk1epbrdBprtfSeH--wc7VWOpdWuTzJgjF1xWitzgEbfgxmo1FtWEa2saAVIsxZ_rKEi_5rR8QVPdjqFWFx69ZQ) Unfortunately, the numerical computations converge, but ... several aspects of the results can and should attract the attention of the modeler: - the value of the rotation, both at the head and at the foot of the posts (54.2 radians!) ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/7Lq2eWLsJdudGU6W-embedded-image-dutetgzz.png) - the presence of Mz moments in the corners while the supports are released in Rz - the sum of the reactions is not zero - finally, the value of the reactions Fx and Fy seems low (order of magnitude to be found: 10000 kN.m/7 m (lever arm)/4 points = 360 kN). ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/IU6n9E5lPbnRfBKB-embedded-image-abkch8uk.png) It is enough to create an embedment using (fictitious) bars at the foot of the column, in the slab ... ![](https://lh5.googleusercontent.com/6T_r9_h3jEqKF9P0RQMDsjvYSVUndlgQGDod3IBGCULs6oJWtGvmbMOs14YJsi1Lz1HNjBR87avihYmsfCu4YhdVIl0FD30TSV93nlh9ddZVy0LOCluFY9NYOy7hXansl2bZmiHUpjjwP2iaTpsc0Q) ... to obtain accurate overall results. (The local efforts at the foot of the column are of course disturbed by these fictive bars). ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/p2IjOOxF6eaPoKLQ-embedded-image-kwrii8ph.png) ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/gHhXYndAhfS19cp3-embedded-image-s6hpujwh.png) --- **C.6.5 Plate/solid and beam/solid connections** In the case of plate-solid connections, it is necessary to establish a connection to recover the embedding moment. As in C.6.4, you can either create a connecting plate on the surface of the solid (on one or both sides) or extend the shell inside the solid. *![](https://lh5.googleusercontent.com/ZSJddpfeOOMVZzRrYWGh9w0O-2bR_B7sqxse1_kVcChdFAyjAyb37IiHxbsZMRknSr0XsmMVGMIUdlI-_Bj40OM9Ip79qM88tEdcnjCpKi3lvUsji-2ptfdDIrp90pgcGkKsrUL29pbXwqOwDqoXnQ)* *Modeling the shell-solid connection* The same reasoning is applied in the case of a Beam-Solid connection. **C.6.6 Stiffness Values / Stiffness Deviations / "Rigid elements".** Many software offer "rigid beam" or "rigid link" elements. This type of element is sometimes a kinematic dependency (mathematical relation) between two elements and sometimes a fictitious bar whose stiffness is very high. However, the presence in the global matrix of the system of elements with large differences in stiffness can cause problems of convergence. See the final example on matrix calculation presented in [paragraph A.1](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a1-what-does-the-software-do-in-a-finite-element-calculation-the-example-of-beam-structures "A1. What does the software do in a finite element calculation? The example of beam structures"). **These instabilities or numerical errors do not necessarily appear with an error message.** In most cases, it is advisable to use elements whose stiffness is defined by the user and to test the influence of this stiffness on the global behavior. **C.6.7 Linking different types of elements: Structural Zoom - Examples** - **Insertion of plate finite elements in a global model** To understand the specific behavior of a particular area of a structure modeled using 1D elements, and to avoid having to manage a model that is too heavy, it may be necessary to insert plate elements instead of the initial bar elements. The connection between these two parts of different nature is made by means of links or rigid bars in "cobwebs". Examples of connections of a model composed of beam elements with parts modeled in plates: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/CwAcciVSs9p0xpbI-embedded-image-govxjvjd.png) ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/ADuTn2YEO1QqQgMy-embedded-image-6ehrdty3.png) - **Structural zoom** One may also wish to model only a part of the structure with plate elements and impose at the boundaries of this part the **displacements** or the **efforts** at the nodes resulting from the global beam model (principle of structural zoom). These displacements or efforts are then transmitted to the plate elements by rigid links made of beam-type elements. These areas of connections between beams and plates must be modeled far enough from the area to be studied to ensure that the efforts introduced by the rigid connections are correctly diffused to the studied zone. For example, as part of the analysis of a connection zone between two RWB (Reconstituted Welded Beams), the zone was modeled in plate and shell elements (see figure below). At the ends of the RWB modeled over a certain length, torsors are introduced through rigid connections, with the structure being supported at the level of the lower plate. The view below shows that these rigid links are located sufficiently far (about 2 m) from the area to be studied. It should be noted that the plate is sufficiently rigid so that no rigid links need to be created. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/eEg9CCF0HouuVc9a-embedded-image-jznw8yvg.png) The following example represents the structure of the girder of the extremity of a relatively wide bridge. The two support reactions are introduced (on the right) under this girder, which is considered perfectly embedded in the deck (on the left). They come from a global beam/plate model. The self-weight and dead loads on the girder itself are modeled, if necessary. This approach simplifies data entry, as it requires only a few support reactions rather than the complex torsors to be obtained at the interface with the deck due to the nature of the global model. *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/kYP87vNAZS39Xu4Y-embedded-image-n5wcruzd.png)* *The global model with simplified modeling of a girder in an extremity.* *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/Rwa3z8CgrrlgRLos-embedded-image-3gvke2dy.png)* *A detailed local model of the abutment box* # C7. Offsets #### **C7. Offsets** Most finite element software offer several options to define a beam on a fiber other than its neutral fiber. This option is very useful, for example: - to easily create links between elements of different or variable heights (or thicknesses), but with an aligned face (see below), - to define the geometry of a variable-height deck (it is easier to introduce a fixed upper surface and to introduce a vertical distance between the upper surface and mean fiber that may vary during design), - for the application of loads on one side (for example on the upper surface of a bridge, for the creation of “load trains"). However, it is necessary to define the offset between this defining fiber and the neutral fiber, this offset being the **eccentricity** that can vary along the beam. In case of doubt about the operation of this option, you can check it with another model where each beam is defined at its neutral fiber by creating the offset yourself with rigid links. The subject of offsets is partially illustrated in the document ![](https://lh6.googleusercontent.com/xZ-_PuwQt1XAnQ_p02a5HLo_hOAJlpPA0VrXVfR8lEwwtCs6Myvce55EnsyGz_88ctkl2c0KhF-1wlgi3t0Wpu8NSBWBAnhCCg75nz1StcQ3eGQy0IbjR0Gacke1teXyK4B1RSqhAMROLWBj2sHXaA) [Example of Prestressing and Offsets.](https://cloud.afgc.asso.fr/s/CnNKt5sF2smWZr6) *![](https://lh4.googleusercontent.com/6lML4tFQUizUeZbiVhe87AnoVJKQWTLasVTmYLm2XzLjvXorI5xlO8spFxKlkKxVShnFLfbk58u0c-aIRtOoO4wdgdCsPNPpZ_wUqsvNBv-LE_Espg3HmTgalFnUwOON0_xyw7ME6Xh-Wb8qgQOoQw)* *Illustration of the offset of a series of beam elements with respect to a horizontal upper surface.* # C8. Composite Sections (Beams/Slabs) #### **C8. Composite Sections (Beams/Slabs)** Composite sections are made up of the assembly, rigid or elastic, of elements of different nature (wood, steel, concrete, ...) and/or at different dates. We study here the most common cases encountered in modeling: - building floors (slabs + beams), - bridges beams (prestressed, precast beams), - girders of mixed steel/concrete bridges, - mixed building floors (steel beams + reinforced concrete slab), These elements complicate the calculation with different approaches depending on the case studied. ##### **C.8.1 Floor beams of buildings** This chapter concerns the floors of buildings calculated from a global model. **C.8.1.1 Calculation principle** The difficulty with this type of analysis is to reconcile the finite element calculations with the design regulations for reinforced concrete. Indeed, the reinforced concrete regulations (BAEL and EC2-1-1 §5.3.2.1) are based on precise rules on the effective flange widths, on the offset of the bending moment curves (which correspond to the formation of the connecting struts), and on the deformation diagram (consistency between the deformations of the slab and the beam). However, the finite element models are based on Strength of Materials and not on these regulations. In any case, the calculation of the reinforcement must be performed: - by considering the direction of the slab's span (in particular the prefabricated elements), - by using the efforts from the model, - by correcting them to account for the effective flange widths (non-participating zones of the slab weigh but do not add to the strength), - by correcting for additional eccentricities not modeled (vertical or horizontal - effect P-Δ), - by redistributing the bending moments, - by performing a regulatory calculation with these post-processed efforts **C.8.1.2 How to model the beam/slab floor** The first aspect concerns the floor modeling method. Indeed, several options are available: - to model only the beams, the loads being directly applied to the beams, - to model beams and slabs on the same average fiber, - to model the beams with an eccentricity with respect to the slabs. *![](https://lh6.googleusercontent.com/KIOw_7p2GOFdt-PlF2KQ0YcPd0aE7F_oDeL32Qnp3RNzC5wuHl4SQuAkZrD_xg2hZSzuF1MFpteJ147SjxnfgWCvmgMyKCaip0m6T0BMM9pBX0HT4EZCB2llhS0fZXfLDgmfguU3f31iBmV6g6_sbg)* *Illustration of the last two approaches* The comparison between these cases is made by using the following example: A structure with 2 spans of 8m each, beams with a cross-section of 25cm x 50cm spaced 2m, and slab with a thickness of 15cm. *![](https://lh4.googleusercontent.com/6Wj7998ylsRiCWbVw9LTCcFusD8vqIqnlKMT4oJiP3vEz_-xKJm5DaZY4mQGCW95EfJ6WVga5SJhM1OAcxR8P0Oprd5AZfgp5cuf_RVlxsWFYigm249alj73qjTeRjTnl7mclvzvyzRkLBw51Iwr5w)* *Plan view of the slab* *![](https://lh4.googleusercontent.com/m3YQGm2qdMzJs7IPHypbU1bRpggHneN1SCcz_wtpCRtJjM0U3fYZMitu0PvpGznR_dtJzVKcWCjWAgMShBsJs9H3wa4DLqTOd1kd3d8qTqGcJtEGv8GvyFoa_iSVlTGcu9ttCDmGdv5Xrony1cfgxg)* *Cross-section* We will study the central beam: Load = dead weight + permanent load (cladding) of 3 kN/m² + accidental load of 5 kN/m². We study the ULS case (1.35 PL + 1.5 AL). There are 3 types of modeling: - Case 1: the slab is not modeled, which means that the beam is calculated according to the usual methods for reinforced concrete - Case 2: the slab is modeled on the same average fiber as the beam - Case 3: the slab is modeled with an eccentricity with respect to the beams **Case study 1: modeling the beams only - the slab is not modeled** *![](https://lh3.googleusercontent.com/gc82NfOTyN9ftmE12GQoONhwWC5lxjO2bdZRDYEXL-Nn01G0H4FkRlDWTRguDv6L9z6rNJC1MLY-KH6T7rcTijH5_JuTcxWuPNiTE5ukPvOVo5ElE1I9VV5npKHJVZYrWrIEwMOFm77mVlFjv8Hsjg)* *Modeling scheme* *![](https://lh5.googleusercontent.com/KhK-3rNlI6ru634Cyaprmu6CGQ5SefkIJkp6Vg1WX9o6C9mZ-k5oG8OiufF43wiIoulMV-PKsALmT394q2hjcZVjqlfrns25pZpuFvZkViBVqUm0EMfLxfjYi4clb9_DYGws2jCJs5piYI3O53FyOg)* *Bending moment diagram (kN.m) in the beam* The bending moments are equal to -264kN.m on central support and 149kN.m in the spans; they are consistent with the classical calculation methods; this requires reinforcement of 19cm²on central support and 10cm²for the spans. **Case Study 2: the slab and the beam are modeled on the same medium fiber** *![](https://lh6.googleusercontent.com/OBeGPFJg2PoQwfsAipgRbrghHGD6NfDcFCNTlvdJrY7dipU56G14TXiYKSI0AGvJKtplEhOizKfC-ck2biOfJa2OqCzUsfISLAGhbF_xxMO4cvryr8m3kQbsEGHPXOKPeLHN43zh-yobfs6FqOgZeA)* *Modeling scheme* *![](https://lh4.googleusercontent.com/DgMlRKb4m0FdTHfK50emKqckrwZOePwD4IGbK2QMZNkmbT0FK41Ih4Ji7xrkJG3yDdtywLxmdBDZ2bZf7ZmsAQE077DCTsO7tbZk-f55QO-GCFaWZ7lDPby4JgMch2l8zuUOeNr-niQ4S62u_90OWA)* *Bending moment diagram (kN.m) in the beam* The bending moments in the beam are equal to -166kN.m on the central support and 94kN.m in the spans; these forces are much lower (-37%!!) than those calculated in Case 1: the calculated reinforcement is only 11cm² at the central support and 6cm² for the spans. *![](https://lh5.googleusercontent.com/HYHQMn2lTgd6ep0Cz6F8M2VGuhoPi7Fp4rUPCHQ1bK8unf4vK7mz3cLA0a3IS_InwgQiAekXbXGa4tOz-06jJVC7faS9dQfDYP4jCdYgJF1m2sUgVw7273MJjqmRbLNf48jhtDYiywGRai5zFj-HCw)* *Longitudinal bending moments in the slab* The bending moments of the slab are equal to -21kN.m/m on the central supports and 12kN.m/m in the spans, which results in a reinforcement on the central support of As = 5cm²/m, Ai = 0 and As = 0, Ai = 3cm²/m in the spans. **Case study 3: the beam is off-center with respect to the slab** *![](https://lh3.googleusercontent.com/7buIjdN884AzYx7lF8dA2aCn18nHk0gU9Kqxe8-uAM_jYdY5xlgkeiBEVYegbe4vsjhI-Z4ixabD3EAH2kXHR-kKIed1e4d8jphrl1X_fRdGREPVF2tiO_CTSKcQJuGPdeeQXcUmIPu4brablfHG9g)* *Modeling scheme* *![](https://lh3.googleusercontent.com/tcwqD6YgvaOrImanzhcj7KFHRaSVAfSpgFS7xN90_Zq1RuT5SV9W0tOlAlKW49VqV7qNoMPAX0KCmA82lp7yk-ksxIxtqlsIoMkECNXiYw8_jesMvhia8ZFkqseATVTypSaZTxxk9-ujhlL6QmtGYw)* *Bending moment diagram (kN.m) in the beam* *![](https://lh6.googleusercontent.com/C7oxqE_2AL54buhgpDzYIbupuFRyddfA9-r3LTQtIPRo2kKryZBOSZ-dJ53l1-lUcY47oNS4ZRaZzSzHMGQ2yBWwZzINjZZlxeeTv76rOp1HTg2fGX7wRvw7fgqoDmKyTAE7smTbCxE3bNEqfz9Ajg)* *Axial effort diagram (kN) in the beam* The bending moments in the beam are equal to -47kN.m on the central support and 21kN.m in the spans, but they are accompanied by axial forces (tension on supports and compression in the spans); the calculated reinforcement is then 10cm² in the upper layer and 2cm² in the lower layer on supports, while there are no steels in the spans!!! *![](https://lh5.googleusercontent.com/eT_MoehKWR0ZrLPUFff-QCXNOCADUB1jptGqOUsBQYbceLbteLd2RZH5qwAHoCHMIr967HkKqDII_qYCivvzpX7Gak0uPGZYtqCmL1ziVFh7_cz97Y3rWHEl-56h7qXUp7KLAtVRxM5oXc9AYrNJbg)* *Longitudinal bending moments in the slab* *![](https://lh5.googleusercontent.com/KiCOjB4md1V7fxu_SZKVWWKbXuDgTX13ma3MRRjjzWIrHops63A9BwSn_Pfhoixi-snbVfaAbY-rvdFgHgqdHiIn06mil-szy3mCzKnnauGR3UDilC09oQxhnqHbZ3PzcO-oM1JaumjUT96m2dy_VQ)* *Longitudinal axial efforts* The bending moments in the slab are equal to -17kN.m/ml on the central supports and 9 kN.m/ml in the spans, they happen simultaneously with normal efforts with peaks on the central supports. The analysis shows that case 3, with the offsets, is unusable and incompatible with the normative verifications because normal forces and peak forces appear in the slab. Indeed, how can the bending moments be redistributed considering normal forces? The tables below summarize the main results. *![](https://lh3.googleusercontent.com/UxdQgRMfr8lbE4jrOxCcb9DcUX4-4VSaqjhCDRqjfIZgpa6sUwYipvwYW9wGB8gB6CxEjx7A1kw4p1FhENWfqqtO1R09Xej09TagXUIVPWOieq7ue1xrrb7EJIFgRwYAsp-gCMhkXzn8WSBCud_0yw)* *Required reinforcement in the central support and the spans for the 3 calculation methods* Cases 1 and 2 result in similar reinforcement areas, which seems to validate the modeling of the beam and the slab on the same mean fiber, but the conclusions of this example should not be generalized. Indeed, as shown in the deformation diagrams of the sections below, there is an inconsistency in the spans with tensioned rebars in the slab, located at the level of the compressed zone of the beam. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/lLV6v5qQmWRKb0rD-embedded-image-nnpi6xya.png) This example shows that: - modeling only the beams alone gives good results, but this option is difficult to apply in a global model (how to transmit horizontal forces for example?), - modeling an offset between beams and slabs allows good modeling of the floor stiffness, but it is not compatible with the normative verifications (how to redistribute the bending moment diagram when part of the bending moments appear as normal forces in the beams?), - the reinforcement of beams and slabs should not be calculated directly from the results of the global model. **C.8.1.3 General method for the design of a beam/slab floor** The calculations of slabs and beams must, on one hand, consider all the efforts calculated in the global model and, on the other hand, respect the normative requirements. Let us take the example of a building subjected to horizontal forces (wind, earthquake, thermal, etc...): ![](https://lh5.googleusercontent.com/ymwYrPQYQCD9kHpjPJ9qCw5iuoQyUcQpIeGwbOoxUWnoeu52ojFWRQJydu1w6x-zWJ0zFu1MnxUqeCZr88FgNI6LnrI_gYwHEbKa2WeQ4Yit2Ed3lAT3zTQefqTDFcLLXiA3peJR9IutmrYbJ2cM8w) **Step 1**: Create a global model of the building. This global model allows the calculation of the forces in the diaphragms formed by the floors, which results in the appearance of membrane efforts (normal and shear efforts) in the horizontal elements. These are the forces that we will use for the rest of the calculation: Nxx, Nyy, Nxy in the slabs, and Nx in the beams. **Step 2**: Create a local model of the slab. Indeed, except in very particular cases, it is not possible to use the global model of a building to justify the slabs for several reasons: - phasing is generally not modeled, - pre-slabs are generally not modeled, - the position of loads in a global model does not necessarily respect the zones of influence of beams and slabs at the local scale, - from a regulatory point of view, punching, stress redistribution, stress discontinuities, etc., are not accounted for. In the local model of the slab, its geometry is extracted from the geometry of the global model. For the sake of simplification, beams are generally replaced by linear supports, while slabs are modeled by shell elements (bending) subjected to weighted loadings. It is this small and flat model that will be studied for the normative verifications, possibly considering the phasing, pre-slabs, etc... ![](https://lh6.googleusercontent.com/3o0ex6Bj31yZ94IHbI5OwY1eOzkdygRlUgCA7H4hisfZKZWG60mxGZrz2XxThu4xmhTgRwOPPxA-U7Ci3e1LdjlJCMnC6Fr6_4r6rkGv0ov7rm8uFcIix7IuIKZMiXBZgA2YYzvSTwbhH4iiMsCtAg) The bending moments (Mxx, Myy, Mxy) in the slabs, resulting from this local model, must be cumulated with the normal forces (Nxx, Nyy, Nxy) of the global model to calculate the reinforcements and carry out the normative verifications (pay attention to the combinations). **Step 3**: Create a local model for the calculation of the beams. Indeed, for the same reasons as for the slabs, it is not possible to use the global model to determine the totality of the stresses in the beams. The geometry is identical to that of the local model of the slab, except that the beams are of course preserved. In this model, the slabs do not have to take up bending forces, they play the role of load transmission to the beams, therefore, they are modeled by distribution surfaces (refer to the documentation of the software used). ![](https://lh3.googleusercontent.com/Lt7ah8gvyS0ANxusZrBjt88GxFo1xkTv-7WWjz_QMiSDkCLiwPhvlLmOK8NA8wlIZiXa2CkIUvwRtSg3EPUozFhSDS7vtHW8Qz_T4rTNnetAkvr4h6n7i5n-bj0ir46VwO52i60EUWSe0imzFjaRVQ) The resulting efforts in the beams must be added to the normal efforts of the global model, which allows proceeding then to the normative verifications on the beams (either manually or using dedicated software). **C.8.2 Case of Bridge structures (ribbed slabs)** This approach applies to bridges such as PRAD, VIPP, ... For the calculation of bridge structures, if the Guyon-Massonnet method is omitted, it consists of calculating the structures: - in girder grids, i.e. crossing longitudinal bars, representing the section of the ribs + the effective flange width, and of transverse bars, modeling the slabs: the advantage is that we directly have torsors that can be used in the calculation of reinforced or prestressed concrete, the disadvantage may be the placement of loadings, especially moving loads, *![](https://lh5.googleusercontent.com/RfbG7L0M5tvQAjD6lGsEqcAfHBzjP07KS3Qk4pYA4NANCYjzEFptuolnyQQ_05SGLVz1obLqou7TAgnnYuvQWXfQx8hn07zzwUbu-3nZ11YowUKA2qHTgODbdesGkKPglxQndLfETgqgertoJrMVYA)* *Beam grid model* - in beam grids using ladder beams - can be advantageous for a phased calculation, especially if one wants to model in detail creep or shrinkage effects - as in the third approach above (C.8.1.2), by modeling the ribs with beam elements and eccentric slab in the form of a FE shell: the main advantage of this approach lies in the easy application of the loads, the disadvantage is that one does not directly obtain torsors that can be used in reinforced concrete calculations. It should be noted that the beams modeling the slab must be perpendicular (or almost perpendicular) to each other for the model to be valid. --- To illustrate this approach, in particular the reinforcement of the slab and the ribs, one must start from the example discussed in C.8.1. ![](https://lh3.googleusercontent.com/pCKCIP1-ZRGEVQ4dKiMcty5cmslqWeoDd8AcQlqt8w9eozfXt-XXy1XSpxSwBR37XS_L7Ej_vxWe9pqSNHZ6TNzgM42EAbSG_ft5S69M3x6H6D62OvYGpDwUdtrdtE_zNzh3Ni56ficDZBiiNPnt5Q) *View of the model - 25cm x 35cm drop-beams and 15cm thick slabs. Spans 2 x 8m - beam spacing 2m.* The calculation of reinforcement directly from a reinforcement module is not recommended if the assumptions used for the design of reinforced concrete are to be considered. A small post-processor (a spreadsheet) is enough to calculate the bending moment and the flange width assigned to the rib, as shown below. Application to the central beam of the model - section on the support and section on the spans (note: both spans are fully loaded, without considering the influence line): *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/hRSUZDoVqIeYYu4a-embedded-image-qnrcvvmh.png)* *Bending moments (only the drop-beams) - kN.m* *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/bUIGo9D9WAQugF5A-embedded-image-ggbhvjsb.png)* *Normal force (only the drop-beam) - kN* The methodology consists of applying the plane section remain plane assumption and calculating the (elastic) equilibrium of the internal forces. 1. The stresses diagram is extended to obtain the stress on the upper fiber (slab top) 2. The normal stresses on the composite section are zero: the integration of the normal stresses must be equal to zero, the effective flange width of the slabs is deduced 3. All the geometrical and stress parameters are determined, then all that remains is to calculate the bending moment resulting from the stress diagram. **Application to the case of the supported section:** ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/YB28pSJlL0zQbjb0-embedded-image-4e2bh5nw.png) A reduced flange width (47cm) is observed, which is logical considering the shear drag effect. As=14.4cm² (ULS calculation). **Application for the span section case:** ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/fNLH3GGEhXKZffUW-embedded-image-3efjct11.png) A larger effective flange width (139cm) is observed, which logically is larger than on the support. **As=7.20cm²** (ULS calculation). If an **automatic calculation** is performed for the rib and the slab: ![](https://lh6.googleusercontent.com/8T7yVLRTEP8mEMb2lWc4Q4DhqZnLqSwFZ--t2oEMBO26G820wakDXHxpzMqfejxE9zWCqdNhf60XDFWNRGnCGXNL_WYfl0PMSmrXEK7qkxILRmwo-mGqcPfLS_chiuKzw28PkefEyXbE8IJjDgFQug) ![](https://lh5.googleusercontent.com/DGlYHRmBUzS8aAfUDLq0QgSuCezKAE_jojlw6kI6CV8ZEx-towD2Xsw8eILVQH11lWRw5Hk9z8AjQfld9Jp0ikOPr04AMh-xkexx9Nl5b2Q3JnyfmJsABCA3dAmCC2JZrw0zXlYFebZU-IT7fetoPg) → The software suggests reinforcement sections at locations that actually do not require them when performing a "manual" reinforced concrete calculation (it has been verified in parallel that no compressed steel section was necessary). → In the present case, the automatic approach leads to a slight reduction in reinforcement at the bottom layer in the span and an increase of reinforcement at the upper fiber. *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/yArZK1ibBUncUYeW-embedded-image-4deucatc.png)* *Mapping of the reinforcement in the upper fiber of the slab* *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/wzWOvoFLyx26C6ZU-embedded-image-xveucipz.png)* *Reinforcement in the upper fiber of the slab at the central support, central beam (18.36cm² along 2m)* *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/oHqOAmzUG8vvDNjC-embedded-image-emprszuu.png)* *Reinforcement in the lower fiber of the slab* **The efforts calculated using the beam grid model are as follows** and lead to 7.2cm² in the spans and 15.4cm² on the central support: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/Qwzrc2pupVmBa61c-embedded-image-p2imuplv.png) *Beam grid model (Mt = 140kN.m, Ma = -262kN.m) - without taking into account the effective flange widths* To conclude the above example, we realize that the automatic calculation of reinforcement is not satisfactory. Without considering minimum reinforcement, it leads to placing reinforcement in zones where the normative verifications would not require it and to under- and over-reinforcing some areas. Besides, let us recall once again that the automatic calculation does not consider the redistribution of the bending moments diagram, punching, or connecting struts... It is, once again, up to the engineer to analyze the results and to decide if they need to be considered or not. It should be noted that the problem of stress or reinforcement smoothing arises also when using slab or shell type finite elements.For a beam grid calculation, one should refer to the SETRA Guide "Advice for the use of beam grid programs" - PRP 75 - a particular area of focus is how to consider the torsional inertias.
Other examples are given in **Example C - Modeling of beam grids**. --- ##### **C.8.3 Mixed Steel-Concrete Beams and Slabs** Generally, the composite character of the sections is modeled. However, in some cases, the model may be limited to the main beam alone, without considering phasing, such as for pre-dimensioning. After calculations, the stresses of the steel beam are then used to dimension and verify the behavior of the composite beam according to the appropriate normative reference frame. The model does not detect that it is a composite beam and there is a small error on the stiffness, the acceptability of which must be evaluated. When performing a normative verification of the beam, the mixed character and construction phasing should be considered. Modeling Approaches: For a more rigorous calculation, it is possible to model the composite beam: - either as a beam whose mechanical characteristics consider the connection of steel and concrete. This way, the difference in Young's moduli of the two materials is apprehended via an equivalence coefficient - in this case, it is said that the materials are homogenized, generally by reducing the concrete to a metal equivalence (a), - or as two superimposed beams, one, lower, metallic, the other, upper, made of concrete, at the altimetry of their respective centers of gravity. These beams are connected at their ends by rigid links. This can make it easier to consider differential shrinkage and creep. If the structure is modeled as a whole, the longitudinal concrete bars described above are, besides, connected by transverse bars in a way that forms a beam "grid" (b), - finally, one can also choose to replace the beam elements of the slabs by shell-type finite elements (c). In this case, the calculation of the torsors requires post-processing, ideally automatic, following the method described in C.8.2. The approaches (b) and (c) should be applied for special cases. Indeed, although they may initially seem simpler, the pre and post-processing are always much longer than with a model of type (a), especially if a software dedicated to mixed calculations is used. In order to account for phasing, one must, at each change of state, either modify the inertia of the homogenized beam (a) or activate the beams of the slab (b) or the shells (c), once the concrete has poured and the formwork is removed for example. Of course, the creep of the concrete must be considered, either by means of an equivalence coefficient or a creep law and cracked zones. *Example of a mixed structure modeled according to approach (a):* *![](https://lh5.googleusercontent.com/XWaCym9uNW6c8PnEWjxqKI7O3-uC1QAQj5oBnenPvHqHGZVNlvcc3ZADxCeEOvCpdRoXBge-tKYbo0VWzKJfdcDLLoQhXtnt3nEgrU_uzPRvQ1z436pWbfvrvBlb3HfA81QUxKbH-IWdNNoFMetvMw)* *Example of a mixed structure whose slab is modeled with eccentric shell elements - approach (c). The steel beams are modeled in this case strictly according to the material distribution (metal only):* *![](https://lh3.googleusercontent.com/n8-uNiiBeDGwXQK8NzSqzev-cEEEHCYqgkiUhKbaxwlmAiSdlaNTIeo3umXxbHNmdPrFCV8rFML3bpqZcv9V0J2a2z5T-4Dnx5lPbYDN8_7dCe37fvXvTkLZjryqf_3oIg7FML4aWUmWmu4SOBzMRQ)* The use of software specifically developed for mixed calculations is always recommended whenever possible. See in Part 3, [**example B - Mixed and Steel Beams**](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-b-mixed-and-steel-girders "Example B - Mixed and Steel Girders"). ##### **C.8.4 Mixed floor (building)** A compound floor is composed of steel beams supporting reinforced concrete slabs (pre-slabs or not) or steel deck. **C.8.4.1 Weight and vertical loads: slab bearing direction** Stress calculations in a composite floor are performed by considering the resistance of steel beams alone. Concrete is then considered as a non-resistant dead load. More generally, these floors are made of collaborating steel deck that works in only one direction. These particularities require specific provisions in the models. In the case of simple geometry, the concrete slab is not modeled and the loads are applied directly to the steel beams. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/e5erSxJ5lr94RWLT-embedded-image-xppjowim.png) When the geometry is complex, the manual distribution of the loads on the profiles becomes too delicate, it is then necessary to distribute the loads using distribution surfaces. The most common software have this type of element which behaves like a very thin plate, without any bearing role but distributing the loads on the load-bearing beams. Alternatives allow to consider the directions of distribution of the steel deck, but the modeler must pay attention to respect the load-bearing directions, the verifications are essential. Let us take the example of the petals of the LUMA foundation in Arles made up of mixed floor with steel deck, they are represented in blue in the scheme below ... ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/II11j00otrIrBMHw-embedded-image-0vhosqqp.png) The blue distribution surfaces are meshed like slabs but do not contribute to the strength of the structure. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/JHB82J0ypP4el28k-embedded-image-omkfqjnl.png) ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/zRiqArAWoTfV3O9F-embedded-image-sdnjyhhs.png) *Plan view of the floor with the load-bearing direction of the steel deck* ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/knk1CSPJPLxiYBe5-embedded-image-rs6vboww.png) *Visualization of beam loads calculated directly by the software* The calculations are then carried out classically. The calculation of the slabs is then done by a specific slab calculation (orthotropic) between beams. **C.8.4.2 Horizontal loads (wind, earthquake)** In general cases, the concrete slab is not connected to the structure, so it does not participate in the bracing of the floor. The floor is then braced by horizontal metal bracing. However, in some complex cases, it may be necessary to brace the floors using the concrete slab. The modeling then becomes very complex: - the slab must be modeled with an eccentricity with respect to the average fiber of the profiles - it is necessary to model the connectors between the slab and the profiles - the slab/column connection node is different from the column/beam connection node *![](https://lh4.googleusercontent.com/quk8Aq212gBOKldR6fAvRB0OapEk3B6XIuSScMDHeH2rAt1bhVL2yIRJRtZZgnqCLCaeWRuuCyz-LI0Hinaez7QzYn-OGC2yYBDS3urnF8DeWlSLowSqRcHLz0vpaikUOyZaQAuhUFiFv4n7b9kddg)* *Mixed floor without slab modeling - Bracing provided by the profiles* *![](https://lh6.googleusercontent.com/_I1vvvbEBODKGiEAE7PbKL7yETLfI-o7Q9eeXmOBV1nIOswupqjQC4FtOeYz64HF7oa8TUT_nYjrkY7kxg0JkgPTSJ0sIVNxosbXL4YKcQBx_Yihbb42lelh7gVQDSUQ286W5h5EE-P81fAh8hsyhw)* *Bracing provided by the slab* # C9. Materials #### **C9. Materials** Part 1 Chapter 4 is dedicated to civil engineering materials and their specificities. Defining materials is a rather simple task when modeling because most software have predefined material laws that follow one or more codes. These laws correspond to a simplified "curve" of the material’s stress-strain behavior, which is considered linear elastic and incorporates safety reduction coefficients (on the modulus and the limit strength). Some very specific problems may require introducing a more complex curve (Sargin's law for example), which is allowed by most software. When using the predefined laws for concrete, one should be aware that the Young modulus is generally by default the short-term modulus. For long-term effects, for some thermal and seismic calculations, it will be necessary to correct the modulus. This is also the case for phased calculations where the modulus varies according to the age of the concrete. Similarly, the software considers a default value of Poisson's ratio. Generally υ=0.2 for concrete and υ=0.3 for steel. Some codes require that a coefficient of υ=0 is taken for concrete at ULS. In particular, see BAEL and §3.1.3 (4) of Eurocode 2. For all Strength of Material calculations that require considering the concrete cracking (seismic, second-order, mixed bridge slabs ...), the moment-curvature law of the cracked section must be considered. It represents the weakening of the section and the actual stiffness of the structure. Sometimes, the code provides simple rules for the adaptation of inertias. This may require iterative calculations, first in uncracked inertia to determine the cracking zones, and then taking into account the cracked inertia. It should be noted that some software allows to directly consider cracked inertia. # C10. Specific behavior in shear and torsion #### **C10. Specific behavior in shear and torsion** In general, it should be noted that beam element models do not systematically consider shear stress deformations, nor do they adequately account for torsional deformations. However, in the case of modeling a structure that is sensitive to shear and torsion, one must activate the option to consider shear and torsional deformations and to clearly define the reduced cross-sections and torsional inertias. It can also be noted that the phenomena with blocked torsion are impossible to model in beam-element structures because the beam elements of Strength of Materials are built on the assumption of conservation of straight sections (without distortion or buckling) and yet, their consideration leads to stress distributions different from those calculated in "classical" Strength of Materials. Considering the blocked torsion will generally require the separate modeling of all the plates constituting the thin profile of the section. Here are some examples of structures sensitive to these phenomena: - for shear: slender welded beams (mixed double girders, for example), console-type structure (bracing walls with a low height/length ratio). Failure to consider the shear deformation will result either in an underestimation of the deformations leading to an erroneous deflection or an overestimation of the stiffnesses, - for torsion: structures not free to distort (at one or several points). --- Comparing calculations of the angle of rotation of a cantilever I-beam **Data - cantilever beam:** - Boundary conditions: fixed in x=0 (θ=0, θ'=0) and free in x=L (B=0, T=0) - Length: L = 1 m - Loading: torsional moment at the end x=L: M_{x} = 10 kN.m - Cross-section: Welded h_{t} = 200 mm, b_{t} = 200 mm, t_{f} = 20 mm, t_{w} = 10 mm ![](https://lh4.googleusercontent.com/hlS0yTPYNgXnVlKC1iA-wKtHwo7m_QSNL_Di41Uz7kjugafM6Aj32g3myVdTwjydb3U2etgUfw2bRmuycEBLQaSHTjOMaccDP_lCC8sGWONByr7yUrQYeeZJY6dMxmFOmed7wnqQCfTYbp_x2RqKjg) **Plate element model:** *Loading:* ![](https://lh4.googleusercontent.com/DrLDG_VUci3ENn1nG-lS5UHw_uWMvG0ENascmXZMWB0h_OqRz1z6beQjzfiSwWiSL7mZ_aTyvLxFVioGfU0dhGi5ZWh_zYjID_rVYOiAB_MQrINGPm-VtIxIEg7ybcPjcD9bBSGI_tMjEjIFDoXiCQ) ![](https://lh4.googleusercontent.com/omHYx9s7CpfZru_goX-kUkSpD12PhdEz0uI4Sl9y4RBSMHA4DStP0_8lpLFADRpDLLNtZWEllKhA-YPuytu9AOosj_PQW87cliJJ0hAuWkAo1dro-x3_yYJSwD9Hkp8zoevCtrokk_HNeNE3pR2_5Q) *Reaction:* ![](https://lh6.googleusercontent.com/_yyyKY8e7tWj6Iw9KYIWHtrhsrBimIAJwmwVHTkL_k1a5gQ-RbceYi0SxRgq1CbMjskXSLCSAeKkohA_y8a8SyL5eSsP4I6epRQl4kep3m9hm0QgDB-zQ1zF9WRic3SGEANNmyoXtrypZIEicYu4QA) *Displacement θ(L)=0.042 rad* ![](https://lh4.googleusercontent.com/apqxzii_pUEQ_xST8TOEe-KNAdmuxe3rFjl0_0dhIxbsbCc4SKHKuyTpUxUjQ5GkQeFsg6qJc_9ljtgqteuff51QKR2G660h_2TuwzXgPlsfQeeSSsyrTLC8VvAZxgAGshKLu49-QwjAQ3MlwrrxIA) **Beam-element model** *Loading:* ![](https://lh3.googleusercontent.com/LCRu5IwNoZ5Ljy4eQfjyPOgAnGHQ1VqiUetGgsbPi8rkeuS4ngALFNzWlhf9qPWRp2cgaNNeXoNTqjXhL30rxM-7IK34J8coOHthNtrlmD7DY8s839UhDvxpEYY46cMloOVmFV8B93iCc9VHN6fgFg) *Reaction:* ![](https://lh6.googleusercontent.com/Dtnhc1AW6_I_rJ1ZpVUoruoYpsunHpboxCssn2vWChlG5CQpkXBPUQqHVokRm5PYPCsUN5dPYR5gyKe60jYUIom59OOct2ITfKjfX0n6mGiraVx3fGOW8EiEMpSfaJ83X1sNvQxIGjSuPur8UG8SPg) *Displacement θ(L)=0.1198 rad* ![](https://lh3.googleusercontent.com/sDVYbWFW2YWxqGm2s9bV4xpDapc4MVgNTg0N5kEbTudxJ6ZVf3-rbNHOKqzlg9FZctPpTsEnht7vrd5QqsmKNtxSLvqId7JGlN9Ov4zxSEnlz5JKeB3osu3B4OrLTPserbXF_XkWYPbTkEd4VpjI8w) **Analytical calculation** The differential equation for the angle of rotation is given by: ![](https://lh5.googleusercontent.com/31Sg9g_rHko_HlQjBLR5WKIxD2Flbng_R9dw9lAYiQFJtA2S4GHCxymqsdoprLD82D3yTJ2CVxIFH7ZqxogrZBRs_OqhPEJM8360RTqpERgnT5S-ceK0JTTEMi-SNSnisZUOw4dpyz3JElBFGDAE8Q) With the boundary conditions given in the previous paragraph, the solution of this equation is: ![](https://lh5.googleusercontent.com/MO0Xtm_ym5ZMnuwpJjyhXX0__ufKh5QsrAxVh8Pi_pqxGfOgeDsjV1pV7-5obICno8k29VAWejWvbm7IatLRSZ6LTKEz4CE5Xowp_W6FTWxo2zaal4Y0NTRWSLJ_Pw-okMKL0YFfLcGXNXyAQ6ta-w) With: - I_{t}: St Venant torsional inertia - I_{ω}: sectoral inertia - M_{x}: torsional moment - L: length of the beam - ![](https://lh3.googleusercontent.com/YiAqcoUHOzuQekZir7dT6DR9lFTEZw_Q1ex8jfE42lggmix6p7l1HvoCLrMn_7xpAUidWL79Rg1B6NYyQa5wJzJuKAJOp_cGgC-OUsUSvi6cbmjaqTlN_KNfZAJq1v3yEjj1zm1ImX2NGU1xG6MHkw) Application: - L = 1 m - G = 80,770 MPa - E = 210,000 MPa - ![](https://lh4.googleusercontent.com/CsREIpOTbhNsom1KmQKMMbXUcLCHZRgOYdzoIOS2HzxmnvO5L6x-S2-b1Pf94CBJH07VA_Ku8IzuBwOVrMdj_ulRNQ57j4LYA94Aw86H4VNZCrfrH3mWebHbQ296FSeh6_cdBPagWLLQ6lFjvmV0OA) (calculated by the software) - ![](https://lh3.googleusercontent.com/GshFEj33N-9C9LxQVj-Q1ibXO1sykNijK1x1tHV6McvUuEied5xx_ciIWlq_Gbny98Y7gpl0tC8_vELBQxJrBUhyRrQrKLDPf5ZfO1UVKR9xfmI6CWCgtb5fTuXwUwmc9GlAufZIJlvy2342pXA36w) (calculated by the software) - M_{x} = 10 kN.m - ![](https://lh3.googleusercontent.com/_f0QbgmwxU1INnR9kNlR1z_tDDTvUBx56e9skOUDvmfAONBfgL22x4VOQeFywfgwiXhbpU2lWKG1l1mh3h6nBFtx-AJ5H1ru5GcGFvtOFSCwm8TrIO5WpKonnrtFK24ksKLY7ldueL4bdi7CClgFfg) ![](https://lh3.googleusercontent.com/La5mcKBcHTxKgWIVAniA6L8tbB8MhGq0VrUoOYOY_8WhV-UCmvji7ee1OtqZeFanscTsF3IPMZMYOjkRi1JnbaiBXjlnlGI5sfkRqizE7G6A5ydtLVPaAhCL7GsWOrh_alVhy0JTMMi4T0WSfU8-FQ) The analytical calculation and the surface element model give the same rotation result θ(L)=0.042 rad. The beam element model calculation gives a result 2.85 times higher. In the beam element model, the stiffness due to the buckling inertia is not taken into account for the calculation of the rotation angle: ![](https://lh5.googleusercontent.com/dRxbA7HDH-lTZhJ9eMu9k56-T0t9T6cBue9YipsMpSDSufbSV5t3m8dTl13MarJkDOfMKN3_eI51FXrshy8oh-VO3a6SlKWw2IAm9XJNnsCHY2038K4sPU5ui18LGpH65fIG0wmwUOVUxfV0-c08bg) **Conclusion** In general, for beam element models, the stiffnesses due to the torsion of an open section beam are not considered properly in the calculations. In case of any doubt, a shell-type element approach on a simplified, global, or local model can help identifying the effects. # C11. Modeling the loading #### **C11. Modeling the loading** As explained in [chapter E](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/chapter-e-typical-post-treatment-in-civil-engineering "Chapter E. Typical post-treatment in Civil Engineering"), it is important to always verify for each loading case (permanent, accidental, and thermal), by computing manually the summation of the loads, the global torsor of the loads: reaction forces and moments. (Most of the software enable outputting the global torsor). **C.11.1 Thinking about the test load cases** It is important, as soon as the modeling is completed, to plan test load cases that allow validating the good overall behavior of the model. For example, unit forces uniformly distributed in the 3 directions, unitary punctual loads, or even temperature variations. For these load cases, the deformations (usual orders of magnitude in civil engineering, kinematics, or mesh discontinuities, ...) and the reactions at the support (all forces supposedly applied must be found in the reactions) will be examined. Therefore, these tests enable verifying the stiffnesses, boundary conditions, and internal connections. They can also be used to verify more complex load cases (order of magnitude of the effects). **C.11.2 The case of dead load** Most software automatically consider the self-weight deduced from the cross-sections of the elements and the volumetric weight of the material. This direct method must be systematically verified. Indeed, the geometrical simplifications necessary for modeling may induce a self-weight that differs from the one calculated with the drawings. A rigorous manual approach of the measurements should not lead to a discrepancy of more than 5%. In any case, any deviation must always be justified. As soon as the net cross-sections deviate from the gross cross-sections of the structure (e.g. if cracking, shear drag, or oversize are considered), the self-weight considered as dead load must be redefined, so the automatic option should not be used. Another option would be to modify the characteristics of the materials that are being considered, element by element. **C.11.3 Surface loads and linear loads** Surface loads are generally applied to the average fiber of the plate element. When considering the intensity and perimeter of the surface load, the diffusion of the loads up to the average fiber, including possible diffusion through the thickness of the concrete cover, must be taken into account. Furthermore, one must verify whether the surface load is applied according to the normal of the element (local reference) or according to the general reference of the model. Some loads (e.g. snow) are defined according to a reference surface (the horizontal for snow), which must be considered when applying to surfaces that are not parallel to this reference plane (e.g. a sloped roof for snow). Often in software, it is necessary to explicitly specify whether a load is projected or not. Other types of loads (wind, hydraulic pressure, ...) are always perpendicular to the surfaces. Finally, the orientation of the loads should always be verified as well as the deformations and reactions at the supports, just like for the self-weight case. *See the examples below.* --- Example of the nozzle with earth thrust loading Problem: model a linear load on an inclined surface. The software offer options when defining the load, which are sometimes not very explicit. Case 1: Load defined in the user global reference frame ![](https://lh3.googleusercontent.com/wg89ISQggOL1lTq6Sl93F4EZy8F9kQQ5k4QG-cAY_KVqQueTSBUPOWk45OqL5lu8bMQYptBLTM5PsWYZrEhHF_TdgVR_iSM6wGhYxDVWS18pcmgQXKqDS95XNfN3NLf8ho4V2Dji3_3PVeFbT7-uEw) The load applied to the bar is defined as a horizontal load per linear meter of the element. Case 2: Load defined in the projected reference frame ![](https://lh6.googleusercontent.com/90qhNTi665Ro5K1uaXxP1_z5a_H-DdzNx0opVRAXivVhjBHW4wr7wd5XGKdlK64y-xkP2t4-z2n1m1TKNuSecv9IaZ-smyeKV_nJT9qlnrqr9wij1jGvq-KWVvL90J9nWnPrbYRmlFCIjJ2oiAAidw) The load applied on the bar is defined as a horizontal load per linear meter measured perpendicular to the direction of the load (vertically in this case). Tip: Always check, on a simple example, that the option used corresponds to the desired load model. Linear loads are also affected by these problems of diffusion and coordinate system. Note: in the case of earth thrust, the best modeling technique is the second one, i.e. a projection of the loads on a vertical plane. --- **C.11.4 Thermal loads** Thermal loads are made of two types of loads: - Linear variations: a very common special case is the uniform variation, - Temperature gradients that result from a temperature difference between the extreme surfaces of a structure. It is essential to use test cases to verify the correct consideration of thermal phenomena in coherence with the clamping of the structure. It should be noted that thermal loads only create efforts (or stresses) if the structure is not free to deform (clamping, hyperstatic structures, ...). Concrete cracking can play an important role in stress distribution (see 11.5 below). **C.11.5 Shrinkage and Creep Modeling** In the absence of a specific software option, concrete shrinkage modeling can be performed by applying equivalent thermal load cases. Creep modeling can be performed by applying thermal load cases or reduction of the elastic modulus of materials. It is important to verify that the imposed deformations are consistent with the expected phenomenon. If there is any doubt, it is always possible to perform range calculations, to frame the short and long term (case of compound bridges, foundations, ...). --- **Detailed description: modeling of shrinkage in compound bridges** [Link to shrinkage modeling in compound bridges](https://wiki.afgc.asso.fr/accueil-gtef:partie-2:chapitre-c:c11.5) --- **C.11.6 Live loads** Understanding the concept of influence lines is fundamental for a good apprehension of the positioning of convoys, it avoids designing for too many load cases. In the case of complex structures, the concept is not easily applicable, however, influence lines can always be generated by placing unitary forces at different nodes of the structure. After post-processing the results, with a spreadsheet, for example, both surface and live loads can be positioned to produce the most undesirable effect. The codes frequently define load models that combine loads of different natures with concomitance rules and specific geometric configurations. They should be read fully and carefully. It then allows, thanks to the influence line, to apply the loads at the position that is most undesirable for the studied effect (deflections, forces, ...). **Loading according to the influence lines.** **Case of distributed loads that can be broken up and of convoys with variable vehicle spacing.** To our knowledge, all the regulations require to load the structures along the influence lines. Common practices or the phase in which the project is in (preliminary studies, pre-design, or even Executive design) can lead to simplifications: loading of two adjacent spans, loading of complete spans alternately ("one out of two”) ... [Link to the ECAM website](https://clb.perso.univ-pau.fr/rdm/isa2/Codes/HTML/ligne_influence/ligne_influence.html) In the case of engineering structures, more specifically for Execution design calculations, loading by influence lines is mandatory, and it is not enough to load complete spans or to make vehicles drive uniformly close to one another. It is therefore necessary to make sure that the software used is capable of performing influence line (IL) calculations, i.e. adapting the loaded lengths or adapting the number and spacing of vehicles in a convoy to obtain the most unfavorable situation for the desired effect, for example, the bending moment, the reaction of support or the deformation, ... 1. Eurocode uniformly distributed loads. We are looking for the maximum shear force (i.e. positive or negative) at mid-span of a bridge with two equal spans (2×25 m) and a constant section. We know that the influence line of the shear force at mid-span has the following shape: ![](https://lh4.googleusercontent.com/--hmSi9yyuBTyrSo2fumSWyKdbVyEiXEf9pExNvDyNwxglMqVpD_FhWCIjAinPZxgckhndHas1tCNGFA1gocAjF-TO0stLBFFodl300qgN3xvANErMyULLA6GILA58oge6SmwHgrcwsfYTSCnqaUdA) For lack of a better solution, one might be tempted to fully load one or both spans. The diagram below shows, for a unit load of 10 kN/m, the shear envelope for the cases: - Span 1 loaded ![](https://lh5.googleusercontent.com/wMJhWmqH_qd4TWEO13tOjMRX8qnK0TK154mKcs4UKtW4mRCxHHF4NFHLdkreeUWuJSdpLaOboinkVrp4nSuqCqJCjXtE7qfXlYy1cvLqcWJYvgf60k3Dq23XvxH_siCytfHFXovWTc44CfbjCEbdaQ) - Span 2 loaded ![](https://lh6.googleusercontent.com/9WAHpkCY0wCSOx0y7chC5yMyQ1iS1ThsYaHshE2LznymDPxlMlQTA4dFyJ7HpbYaucsCCfhX1_9uUm3-KpRxXmyvOWFioK6oIcd6a08fQdee8rEufGcgXOPNspKxNpj3dc9tmYaflNnWPQjie8Zypg) - Spans 1+2 loaded ![](https://lh3.googleusercontent.com/mmNsEzk9qhaF_19t03O2sSwbV_3_9UHpov7Zo6zE-xnWL5B8b19fOtmlfBS2T-l2Se3hHO4xN6etumxpr3DwgBe9qQopqwknwK0qCWXH58b1RTbeJBUI3mqXsWk25wngpWBbG8VNNfJEosLY1e2Zeg) At mid-span 1, one gets |V|_{max} = 31.3 kN: ![](https://lh6.googleusercontent.com/G1D59a5jze8XOUe4mG3I_7-Q76cx_0EEa47RgoP3jbNJS56CfDYskAkdUG7fQzrFJp0gY6AAc2JMJ_5q13UhgzD6rfjR2mPzGeIHCLsEWMs9JY5yV7mAHmvdQpziZRkBDz-_J1gx_RuppTHJgwv2OQ) The diagram below shows the same shear diagram, but with a beam loaded according to the IL: - Zone IL upper curve ![](https://lh5.googleusercontent.com/pIJzV_WeI-A9YwBlkWMX4Tkzx7UVsUBEOxjQHX3rp5cszKECZtksLCk8QzMN4LiR5PAVmXSJzR9h6EH4FUHVfOx7aFm5cEwvDN_dhUI_vEWbELeFIMBJRIgGblSnhdjsYvp21nQs7UYeuoUoBXe1sw) - Zone IL lower curve ![](https://lh6.googleusercontent.com/BlqBMaVFe-EfluINbEj-idcjQdksSHZa60ZgGmXZA8U59QkBKFmDu1OCsiRR0sXzgwtkmnWLwl0j_9Jh-vNgZRz2AckuzkV9GD2FNBdV_0FhnRrzI-8XqmrSnYB_Vu5A26dhZypd_JgMbe1PgMbc2Q) One gets |V|_{max} = 53.7 kN, which is a significant difference. ![](https://lh3.googleusercontent.com/oasDvtiCG1V8oh_7m9D_soEfu-1FsHOJwel9eKgJQEznUB54cnPrTmOcRe-Q_uvfq-d8MBs4fYhNfC5HswbQV6wbO_Qsm4XPJnTGpRsXOdAGP0UoMHaDGl_b-XZjh2hO2Ic1A7x8lOfDGkQy7wcmuw) The exercise could be repeated for all sections. The latter is particularly true for the loadings in fascicule 61 title II, which we must still use when recalculating for example: - Distributed charges A(L) similar to uniformly distributed loads, but which have the characteristic of varying in intensity according to the loaded length L, - B or Mc convoys, whose spacing can vary, sometimes with a required minimum distance. Convoy Bc is described below. ![](https://lh4.googleusercontent.com/h3f-fhZ38SqN2C7HQh5VITkfBi-jJdBTsWqo_yTn0pM-b4vS0672z-GIl9BRLyjHVVNiCQD3sqqOS-CrRHiWPuYxLxTJ-wgqSdRy9B2hiKkzUAujpgZLuZYvhzzRIT9916uZx0es046NCqyZw-r-Iw) **2) Illustration on the previous bridge for the case of convoy Bc for the reaction bending moment** The influence line of the reaction moment looks like this: ![](https://lh5.googleusercontent.com/clChDoe1a-0TB4SeJW19sn5EmX__HAtKoGXkgpA8yxvcEEwnq7Wz--HBZpS49NVwAXfIjw6rULIzk2Pw-r4iPY6AcQV8dB_KGwi37MOyCoh-dg5ZYis_e1srWbUv5Stf3sSf71fxUjCbpS_17NmgZw) A refined study would have to be carried out to find the precise position of the trucks, but it can be easily observed that (here for 25m spans - reminder) the trucks must be separated to obtain a maximum effect: ![](https://lh5.googleusercontent.com/HsOPwbeObs6NV18j9_lRfRca6IJwsGwjIbEo239wE5V-oYOBg2Smu60NwORb6jHuoTafjCEiWA5i25qrnB7l1uG-2TdAaUw-RUGaRUweFl8gHRtozW8KSZ_ui2UAYAM58szG--SGBdOItOXD2CI49w) Application: we run two convoys on the bridge, the first one with the two trucks very close to each other, as drawn in the codes, and the second one with a distance of about 28.80m (determined graphically). The results: ![](https://lh5.googleusercontent.com/lERlMfH0v2VspYqCAp56ir_c3nmlsz-qlmg_3z4XutwSNWPme8OHmb_UG5AIjInHNZ0pWCoLEo4raM8cCVxA3MRY9jIKoNQbC2Q55fbBGqicFvDz5Vw8OHxCqKfVYo7VttueIRX8HV1hfCLAEWezzw) Trucks very close to one another, envelope, and unfavorable position. ![](https://lh3.googleusercontent.com/_PFc5jtuFzluNiVfZAd4fFJYREg69sCX0Z5le7wWwSdo5k-JwfTW7CN2YywC3qLdgr9xiuSAWerL3fvlcYLZd11b4i7GsDeKUf0c3ktB2jjca4ab_EXEqbo6h3rIVEy3lP4U4Gfk1LNVnBaEwhgKrw) Separate trucks, envelope, and unfavorable position. The difference concerning the reaction moments is about 13%. However, the load case used to obtain the maximum reaction bending moment is not the one to be used for the spans. Practically speaking, one quickly realizes that finding the loaded lengths and/or positions and the spacings of trucks, for all sections and all values of interest, is incredibly difficult by hand. Thus, using a software becomes evident - again for Executive desing level calculations. For the other phases, simplified calculations, with a certain margin on justifications and quantities remains possible by studying certain judiciously chosen sections of the structure, but this is beyond the scope of this document. --- Set of load cases and results for distributed loads. Span 1, span 2, and spans 1+2: ![](https://lh5.googleusercontent.com/5HPD_SUmW46jV_mMqOL3FF7CJ5ilVCIqacNBT1NPgB6Pi_lC9EOUg5lyvjouHfgzmEEgz4m1zEd5jfABGglHs57v_TJ3yhoH4b4R03ieEoiMGJsbIBYzrzEe1jmm2ojiYmz1Vt5BXKG3xoggyXs9vQ) Loading according to the IL: ![](https://lh3.googleusercontent.com/Sc8InSAZcSKIFbFX5hm2NqGA6FbhvoD1M2bIesVWB_uxi2Z0zzhcnA6yQfIMLXLBdeWHkR90pESS41N_vqK9DkPp6NgDhzKcZv6JosevCNJfRESHhOOVo9y0bEOkaT31992lRqI6anRpUdYvqOF57A) ![](https://lh5.googleusercontent.com/BzmZQ40JC5yXTirY67-QeZFokYOCpEJ4N3sR88aI5iMitdwtHEQ8NBj8Qbk5SiOgXoY5BhmaB4gc4lUbKYXjXDhuBJ4HSGsWN0J2km7Gxgw2Q9ZPWsV1tEkKLJDBa1W1zESnvZ-_ANbTs97FMkoCag) **C.11.7 Thrust modeling and land abutment** Generally, the actions generated by the soil (thrust for example), water pressures, or seismic actions are modeled by loads. The reactions (pressures on the ground, which can go up to a plastic threshold, the abutment, ...) are represented by linear or non-linear springs. Linear seismic approaches are allowed if the foundation uplift is limited to 30% of the foundation surface. Be careful: no reaction forces are applied on a face blocked by springs... we let the springs do the work. Note: a displacement approach is also possible to model the thrust loads and can lead to a reduction of the overall loading (see AFPS / AFTES Guide. GUIDE "Conception et protection parasismiques des ouvrages souterrains"). # C12. More about solid elements #### **C12. More about solid elements** The principles stated for 2D modeling remain applicable in 3D, in particular, the use of isoparametric elements (parallelepipeds rather than tetrahedrons) is preferable, which requires a heavy and rigorous preparation of the basic geometry. Automatic meshers should be used with caution. Example of a bridge deck modeled using solid FE: ![](https://lh4.googleusercontent.com/Tr_jY2_b066Y_RKTt5F2jibK0tZGkyTcdIbcx2uBEg19S8HmgLS-GlSwHJI4NdhT1xvIhUTIiaNmUi0ycLhnOxpr-jlSMg5SSEP1LBlRtDQ4aYJg8zdONdbJGjSg7d0rfPfMxJa9EsNu93vQfQyPQQ) ![](https://lh3.googleusercontent.com/n8LjXHaJw7PFAmBIV6aQlIB9u7mt9NictNb-NZ8GZ5XgMneBJjTQaVKpshsd4WpTv-F5PMJwx2vaZ06hDLkn7D_1S9rhecVW6dYuei5yLFQTaBZCgCbb_H5Ulpb5svgNN-JYZwc4i-30T3sb58a-9g) (Taken from Part 3 - [**Example C - Modeling of girder grids**](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-c-beam-grillage-modeling "Example C - Beam Grillage Modeling")). # C13. More about non-linear calculations #### **C13. More about non-linear calculations** This paragraph deals with non-linearities related to the laws of materials and the so-called geometric non-linearities. It is common to associate nonlinear calculations with complex structures such as cable-stayed and suspended bridges, yet this subject appears in the daily life of any structural engineer, for example in the case of: - a partial detachment of foundation footings, - the inability of certain bars to work in compression (see § C.2.7 about bracing), - a buckling calculation in reinforced concrete, - cases beyond the field of beam theory (for example, the calculation of stresses in a bridge bracing under its own weight). In general, for all non-linear calculations, it is important to perform a linear calculation before accounting for non-linearity to understand the behavior of the structure and the specific effect of non-linearity. **C.13.1 Theoretical Geometry and Imperfections** Most standards require that non-linear calculations incorporate an initial imperfection in the geometry of the structure or the elements implantation. Some software can directly integrate this imperfection. For others, it will be necessary either to apply a load case that creates the initial imperfection, or to define the geometry with the defect. It can be observed that in a finite element calculation, the use of triangular elements always allows us to consider the pre-deformation of a flat surface. **C.13.2 Ropes and cables** The ropes and cables are essentially non-linear elements since they operate only in traction and because of the chain effect, an "apparent" Young's modulus must be considered. This modulus is a function of the tension, length, density, and gross Young's modulus of the cable. In earlier phases of the project, it is not imperative to take these effects into account. It is possible to model the ropes using a bar, ideally bi-articulated, making sure to neglect the dead weight of the bar or to apply it manually directly to the edges. It should then be verified in the analysis that these bars are not compressed. **C.13.3 Zones with material non-linearity** A first linear calculation is used to identify the areas where non-linear behavior will appear. The calculation will continue by successive iterations, progressively integrating the non-linearities. **C.13.4 Buckling and large displacement calculations** - Buckling - calculation of critical coefficients Most of the software can determine the critical buckling loads of the compressed bars (i.e. the buckling lengths of the bars composing a structure) from a modal calculation, in small or even large displacements. The calculations must be performed for each combination. Many software also allow to carry out the normative verifications from this calculation of critical loads (or simply by manually entering the buckling lengths). The calculation of critical coefficients is based on the search for αi values such as the determinant Det(\[Ko\]+αi \[Kσ\])=0, where Ko is the stiffness matrix associated with small displacements and \[Kσ\] the stiffness matrix associated with initial stresses. The objective here is not to develop all the possibilities offered by the software, but to insist (once again) on the fact that the modeler must understand what a given software does and what is the impact of the modification of the calculation parameters. A simple parameter may be the required subdivision of the bars to obtain the right results, as shown in the example below. Illustration on the braced gantry in Chapter C.2. [Link to the example of the calculation of critical buckling coefficients.](https://cloud.afgc.asso.fr/s/2zbHzFaPSqG7G94)![](https://lh3.googleusercontent.com/fwEDZXirK3BT0HyuXhOKRpP1-CxcE7JAGzMXfi3AusQvC1zI_9xbdY97eTL-kaxRZCMd3i_HpGoirws2cKiGx2Fa1KwMVJTbOh-Afdx_h-OhENjbbmEl8sYCoO8V8Nd7xsmNpdg0PqZWoS8ZHTZVjQ) This small example confirms that it is necessary to master what the tool does. Moreover, when more challenging calculations are being performed (not linear elastic, or first-order), one should always refer to simple examples from the literature. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/x4IHYj9V1zf5dxkL-embedded-image-84xddajb.png) *Modal displacements* - Calculations in large displacements: These calculations require updating the stiffness matrices at each iteration, whether in reinforced concrete or steel structures. What was highlighted here before for the calculation of critical buckling coefficients with respect to the control of the software parameters, remains perfectly applicable. We refer to two interesting articles on the subject: \- Calcul au flambement des arcs - Comparaison entre un calcul approché et un calcul en grands déplacements du Bulletin Ouvrages d'art n°32“ - [Lien vers l'article](https://cloud.afgc.asso.fr/s/fBfZLqFAN7qzFGY). \- Instabilité par flambement des arcs (CTICM) - [Lien vers l'article](https://metaletech.com/wp-content/uploads/2020/04/flambement-arcs.pdf). # C14. More about prestressed concrete #### **C14. More about prestressed concrete** The proper modeling of prestressing requires using specific software that can manage the cable layouts, the calculation of tensions (calculation of losses), and consider the phasing and creep laws. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/bgUBptZ3nkZOmGch-embedded-image-leo1w9gw.png) *Example of complex cabling* However, it is always possible to perform a prestressing calculation or to verify a complex calculation to model the prestressing in a simplified way. Beams (and shells) must be described at their center of gravity to ensure the correct positioning of the ropes in the cross-section. The next two sub-sections present respectively the simplified modeling of a rope within a concrete section and a rope outside of a concrete section. It assumes that the rope path is known and in constant tension (after instantaneous or long-term losses, for example). It is useful to specify that the modeling of prestressing losses would follow the same logic but with a sign opposite to the action of the initial prestressing. **C.14.1 Cable inside of a concrete section** ![](https://lh5.googleusercontent.com/L769A4y6XEMzbAtM8xdgiTB2cXQMfymINXEFdtfbgwMTPQoK7HHVezdJcYWnXPjbstfa4lze4DuzaGA55FBymkgcacML-k_uldDSjImQxXWZEpmQ1yYRW0lQ_QABOmH-xF2dhujwOAAdxxZ-Sa1lAg) The external forces method makes it possible to understand the effects of ropes by modeling them as concentrated forces at the ends and as pressures (thrusts) along the rope. End anchors or embedded anchors, we will have: ![](https://lh5.googleusercontent.com/CWL-I-FlIO9t5Sbm0QiDocI2rdpw0vJMK6GsL1pxZF_GvXuG5ZSkaDp5NeuZZFJ2YnOcMr83drc_gAWhhtYQ5wxsVdUetiEz0vLzAAH4PgserzxPnjdRAvyCbjhhPFySG1RdZIiuUvxO_ZkrQePJYw) - a horizontal force H_{A} = P.cos(α), - a vertical force V_{A} = P.sin(α), - a bending moment M_{A} = H_{A}.e. (with the sign convention adapted to the software) Along the beam, a cable exerts radial thrusts of pi≈P/Ri, which in the general case can be assumed to be vertical. This is the thrust exerted by the totality of the cables. They are applied as classical distributed loads. Straight segments do not produce thrust (R=∞). ![](https://lh4.googleusercontent.com/KSjrYAziyfOkC00iiStZr6gdGsSwyGcgGojsLQZJUN1spHFmREbs8V1CJg-033_RR0gV_vsZufM4kR8KF4GR5bkoLWzWTQCfz0vGqY069YNhwcMvZJde_4r-uKwseyYoTn6T_X3Pdx4BuoBat2dxNg) H_{A} and P are frequently confused, as the cos(α) is often close to 1.00. --- **Example of a simplified manual definition of a rope.** We analyze in this example a two-span beam of 25m each. The section is symmetrical and 1.25m tall (to set the limits of the cable). **Input data of the cable.** One must ensure that the cable remains inside the beam (in this case the limit is set as 10cm away from the upper and lower faces) and that the connections at the inflection points have the same slope. ![](https://lh6.googleusercontent.com/NAJZrwVJcFESBS4Z2_sj6c1Un1XN9chKwAw1UZyIjxor0QBxcVPzD4p621gSipWQ6DCznbg4zrr0I6-9LQkKHIqBSaNvJSYQOdjRJDDZukx2ZK5wJyw10WpwMreeh9YBjyR4DpMyykm3sybsFqIXlw) ![](https://lh5.googleusercontent.com/bks2OntqRwIskvviQnJ5zoMtMABRwZ6a0ZlKBxtidj-PKYq1HMm9fPIBSb32HN25TRjY-wBwCEwlq53a7dXWcGgceeTLUoUBQLO1QEs71YhCy1PxRyjQAAJsiQ2hNfu9vKjVMT33QkouaQ0RTQw-Hw) Converted to loading on the beam: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/O8ro9rPCIvhBEsF8-embedded-image-t5zumg5p.png) The resulting shear efforts, i.e. the shear efforts considering the hyperstaticity of the system: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/qHx7bt2t5CKa0VhF-embedded-image-hlueverk.png) The bending moment: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/RgZ76NOLunbgYiyQ-embedded-image-o86fo4nu.png) For control purposes, we can: - always return to an isostatic system (hereby removing the central support), - calculate the isostatic bending moment at the middle of the span (or in any section), by summing the forces on the left or the right. The differences cannot be greater than the %, - in this case, verify that the results are symmetrical since the structure and the prestressing are symmetrical. “Isostatic" shear effort diagram: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/t07Mg68ACSec825z-embedded-image-odkbruri.png) “Isostatic" bending moment diagram (the curve divided by HA is the rope path): ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/qkggsJL0Q8hP2eaG-embedded-image-qrrrixim.png) It should be ensured that the support reactions in the "isostatic" prestressed load case are equal to zero: ![](https://lh5.googleusercontent.com/GQwXIwGxgm9T0HA5XCqaKHdDUzOwRoLhfvvHxt3XTx5xpXYehR2Q7htk6SvjNG-2bdGmROoZ3A7rm9kOEwLJ3Yk4xWM_CogyZkNLWBeom6bclDMUSjG-p_d8KQx4VdUQgI1pnnH__DWWfaB1hecMUw) **Calculation using specific software:** For this example, a software capable of modeling directly the prestressing ropes was used. The comparison of the results is available in the document. [Example of prestressing and eccentricity.](https://cloud.afgc.asso.fr/s/CnNKt5sF2smWZr6) **C.14.2 Cable outside the concrete section: forces at anchors and deflectors** Just as before, assuming a uniform tension for the entire cable, the external forces method allows apprehending the effects of a prestressing rope by modeling it as a sequence of concentrated forces. ![](https://lh4.googleusercontent.com/4CNQAXequrCUDG6qAd_iwJ6CaaeWMqNG06OlHtfBAjepXfEHp2ApkJBhSE0u1u5I7k40TNJVoIJcZyikXJ3cjqSe6CvLBf1njJF14uKz22liI-nEMHbrB4NAKjsWXIf3db3sooGGycLtQk_KXZeatA) At the anchor A, the rope applies to node n1 of the model the loads (H_{A}, V_{A}, M_{A}), M_{A} being the moment produced by H_{A} at node 1. At each deflection point, the rope applies the force FS to the bar n1-n2. This is done for all the deflections along the rope up to the last anchor. **C.14.3 Modelling prestressed slabs** The study of prestressed slabs is carried out according to the same principles used for beams but applied to shell elements. The use of specific software is desirable, maybe even essential. It will be necessary to make sure that the elements are modeled at their center of gravity, and that the sum of the support reactions of the prestressed load case is zero. **C.14.4 Tensioning cables (side, order)** Be aware that the forces brought by the prestressing, after losses due to friction and anchor recoil, are strongly dependent on the tensioning method (from one side only, from both sides). For exceedingly long ropes, the error can be significant. Also, for highly prestressed structures, the order of tensioning might have an impact and it is important to analyze the structure at certain intermediate phases of tensioning. # C15. More about phased calculations #### **C15. More about phased calculations** The reader may also refer to [**Part 1 - D.3 Construction Phases**](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d3-the-different-construction-phases "D3. The different construction phases "). Structural phasing can lead to modification: - resistant sections, - support conditions, - internal continuity conditions of the structure. It can concern both elevation and linear structures, longitudinally or transversely, and of course, a combination of all these cases is possible. **C.15.1 How to make a phased calculation with non-phased software?** **Case A - Modification of the net cross-section** This is the case for the implementation of self-supporting collaborative pre-slabs. During the implementation phase, it is the pre-slab that must resist the weight of the structure (pre-slab weight + compression slab). Then, it is the complex \[pre-slab + compression slab\] which will take up the loads later implemented (superstructure, overloads, ...). ![](https://lh5.googleusercontent.com/uMKAOSIHEqqIZ3l1ziL_MjEv1AXec4z5IoRE1nQOTH3pvqZ2VgV7ajaLcXU8LDE22glEtUnVsq9yGDQhfzLBNQaAQIdnLBS-3HvZ2OOPGgHc1kmRfR6p0t7Yk-V4rYE1orcdAfU-qE3K5vLu93BlpA) At the SLS (Service Limit State), there is an accumulation of stresses in the tensioned reinforcement, but there is no direct accumulation of compressive stresses in the concrete. At the ULS (Unlimited Limit State), the verification must be conducted for the concreting phase and the service phase, but without considering the phasing. **Case B - Modification of support conditions** This is the case for a structure with temporary supports. It can be associated with a modification of the resisting structure (example: supported collaborative pre-slabs). ![](https://lh5.googleusercontent.com/uDtGDRSO-BtRlwvGmNkdkLKgc9pURGz5fhUSArqtUWg-veXysE2qx-5D0VRr0BFvvZaPf6SaEAYQa6HH2IYPi5JKjW-JIv5PeDTWeDCvMf3otlwtcV19okbfFB-GFiGalxReBk1wkwzOLKN6mNVI7A) Accumulation of the loadings *![](https://lh3.googleusercontent.com/1enZIXlVPgVib9BrAYVe_wJT_YMhvEzZnMWqNSJEIDQSbJziQBogdRJTKKKh271M4kOrnMJSG8lpAAG5NW3UBUJQBGdSmNFylJj9rp7yHD0mhGrHNIWEaCWVigJ6SR4j14IOQMu8VOfWrwIDFub_EA)* *Phase 1: Loading the structure with a temporary support* *![](https://lh3.googleusercontent.com/_75cTbtL-a9gvXpa47mCqDHRIfqRIvatNEMRm8ExUzvXXJa87CbeVRk6xu7xLJrTezDlbDxX2Ddr9MXqeadEfvUY4nWA7kBwCNpYDghliaaa5pbv6vuv-sztnoNA0BVvSCXAIl8RPZlEkwMN8cSJrg)* *Phase 2: Removal of the temporary support* *![](https://lh3.googleusercontent.com/x2EgfyMMxCjCSImj1mSytU7vcNRufYAFjb7NU588k15bhkPRIR8EqoHerzvAa7H_NSPiJNysEhzo_AUAe7t9KbRthPwzllqvyiCOfcwoa8V8-Sa1zuIutANGDIQEn6lGkk5cPKOv2YvYKtVs0J31bw)* *Phase 1 + Phase 2: The final stress is identical to a non-phased structure.* This method enables dealing with the installation and removal of temporary supports. It is always necessary to pay attention to the conditions of deformation of the structures during the installation of temporary supports (placing the temporary support in contact with a deformed structure). **Case C - Modification of structural continuity** This is the case for a structure that is clamped during construction. The stresses generated by the loads associated with a static diagram are calculated, then the stresses are summed up (if there has been no evolution of the net cross-section) or the stresses are accumulated (if there has been an evolution of the net cross-section). ![](https://lh4.googleusercontent.com/sqHouAgye-3VdExGlGKSWtqZSfZgWoEmmsvPFcicHYg78YOdi5Uvny88Vwrzzp9kuR1VAEY8EhWwYpYeXUi9t_sf-4QcEjcoVHeXxCIbnDPvDbyf6O6X6oh1tZ8NiNbXWyveeogtY7VsqCcHiCwy5Q) Accumulation of the loadings Example: **Phase 1: Self-weight sustained by isostatic spans** **Phase 2: Accidental loads sustained by a continuous structure** Particular attention should be paid to the evolution of materials over time. In the case of reinforced or prestressed concrete or mixed concrete-steel structures, creep (quantifiable by the difference between instantaneous and delayed deformation) must be considered. In the above example, before clamping, the deformation of the structure corresponds to a quasi-instantaneous deformation. After clamping, the concrete creeps and tries to increase its deformation under long-term load, but the structure is now continuous. The clamping of the creep deformations will here generate a moment of continuity on the support that stretches the upper fiber. Creep behavior can be considered approximately (see the CEREMA documents on the subject) or with the help of an FE calculation with so-called scientific creep. **C.15.2 Pushing of a concrete bridge and launching of a steel bridge** The one thing these two models have in common is that during their installation phases, they will witness a shift in the position of the support nodes according to the advancement of the pushing or launching phenomena. Potentially, any node of the structure can be, at a given moment, a support node. Software that accept a pseudo-language of programming may, in this case, have an advantage in creating incremental loops to simulate the advancement (by incrementing the numbers of support nodes). Whenever possible, having bars of the same length facilitates the regular motion of the supports. Modeling the cutwaters, in both cases, does not pose any problem: they are steel bars, usually I-beams, embedded at the extremity of the final structure. **Pushed concrete bridges**: The calculation is almost a classical phased calculation. The sections casted over concrete beams behind the bridge are modeled using bars resting on non-linear Z-shaped narrowed supports (possible lifting). The bars with their casting dates and the prestressing, temporary or definitive are activated throughout time. Finally, the cutwater and part of the prestressing are deactivated. **Launched steel frame**: models can represent classical bi or multi-beams, but also boxes. The main differences with the pushed concrete bridge model lie in the facts: - that the structure is very flexible, - that in the design phase, the added sections (of the order of 30m in length) rest on punctual supports, generally two supports per section, instead of a continuous ground beam, - that the structure has a camber, determined beforehand by the calculation of the framework on its final supports. The junction of the steel sections must be made by taking the necessary measures to guarantee the continuity of the rotations of the edges of the sections. The two possible types of modeling to describe the phenomenon are detailed below. During modeling, when a section is added to the rear of the already reassembled construction frame, the set of bars must be deactivated and reactivated after the new section is added. Otherwise, there is no continuity of rotation at the connection (figure below) and the structure would not be compatible with the 3rd bullet point above. ![](https://lh4.googleusercontent.com/2j_XJ_TLd_yR273ytmzpBJjLybNvEjExO7J7kmKwYYK-ftlXDRpzpP-ZEa_hWle72iUXzkW8LVTuQpKhb-aYsU5i17tGgBbheusXVF9CohwsQ6KSuXJLQR5OVlg1DJJzjK7TBdOgZrYGJc05RMDlVQ) Modeling can also be done by classical phasing, provided that a prior "presentation" of the joints is carried out, which consists of finding the altimetric offset of the two supports 1 and 2 that enables having the same rotation and the same altimetry at each end E1 and E2, schematically (following figures) : ![](https://lh3.googleusercontent.com/9BVtWqWUpZeGy7d7UNi2yOrWKG41ClJBliUqGYKRsqP6eKBCEKlYf7DqZAcN_Qx5yKskxjtfDRhMGjJrTEDVybXv9TG7iWNb4LiSv92siLQ06kb4h7JQwhNzQjQZs30OEP-yca0DfMvKp9Hzj_JfsQ) *Vertical translation for the Z-correspondence of the lips* *![](https://lh3.googleusercontent.com/GiypD5TdOfondwDH4rf4xYYCNaT7Fe4IZuN_jiXzCOPh7mNEGXhmlMewT7c8chGlopIBekMIf27V9b56gO24LxoIo6XvAxJtVP1w5rfe48savIayRpaaL6pJlqaNStzSlSp4ZBJ4KeCuCC-H8DnZXA)* *Displacement of supports 1 and 2 to generate a rotation of the section* Once these operations are performed in the model, continuity is ensured. For the launching, practice consists of modeling the neutral axes of the framework and the cutwater according to a geometry algebraically accumulating the shape of the intrados (rectilinear or parabolic, for example), the longitudinal profile, and the counter-axis, at an arbitrarily chosen altitude. During the assembling of the structure, especially during the launching process, the nodes located in front of the provisional supports are given a difference in elevation corresponding to the altimetric offset between the geometry described above and the altitude of the provisional supports. It will be verified that the structure is in contact with the launching supports thanks to the sign of the support reaction. A support in tension means that the structure is no longer in contact and that the support must be released. Finally, for landings, there are always two cases to be studied, one right before and the other just after. **C.15.3 Phasing Affecting the Straight Sections** Since the construction phasing of a structure has an impact on the stress distribution on the straight sections of the structure, it must be considered. This is the case for structures built with transverse phasing, where only certain parts of the structure see the first loads: such as for composite bridges with coated girders, or ribbed girders, or cast slabs in a second phase, and for compound slabs ... **C.15.4 Expanding a Structure - Delayed Connections** To expand a structure, when a new structure (metallic or concrete) is connected to an older structure, the modeling of the transverse phasing and the apprehension of the relative stiffness of the different elements is essential to correctly determine the deformations of the structure and especially the connecting forces between the structures. The case of delayed connections between several new structures is similar: the consideration of creep and shrinkage is essential for a good dimensioning of the forces developing in the elements. **C.15.5 Cast-in-place or prefabricated structure - Deflection - Effect on the calculation** *Please refer to § 2.1 and 2.2 of the Cerema Guide "Conception des ponts à haubans".* # C16. More about dynamic and seismic calculations #### **C16. More about dynamic and seismic calculations** The dynamic solicitations generate inertial and kinematic forces in the structure. If Eurocode 8 is used for the design, a detailed explanation of the permissible simplifications is provided for the modeling and calculations of the structure, according to its uniformity. This notion of uniformity is explained in §4.2.3 of EN1998-1. For bridges, the guide "Ponts courants en zone sismique" also provides uniformity criteria and admissible simplifications for the calculations. Depending on the refinement of the model and the objectives sought, several points should be considered. **C.16.1 Defining the general X and Y axes** Defining the general X and Y axes warrants particular attention. Indeed, seismic results can be erroneous if these axes are not close to the main axes of inertia of the structure. 2 examples illustrating the subject can be visualized below. --- **Example: Corner block of a stadium** ![](https://lh4.googleusercontent.com/jlmXKS41AExXH1C_jkyX_dxtkRp5IooBEtVNNkqszF7pecl1ZLciMkLw9rDIFuhZ5-_5kNKtesRjv6eexJnyt0vM-Hc6oojx4cjP694AXj--zHgGqMT_LWm788rXQvVVron63KpwhdssP1q9nOwVIQ) *Overview of the corner block model* ![](https://lh6.googleusercontent.com/bJ3TcHaKOVGiGrdmwxMLYPP2kWG34dht3d7yjgKgM1JrTW0yXWzQbWOoM-KQ4WFkazZDCl_lqeENpaRIUdvWg2MF0JcA9DDk2ITAUr_gbGFmyKvyEA8pz1c53La8ulBQiMGaQCArcdeYf3ELI1mVHw) It is necessary to adopt for the corner blocks different reference axes (X, Y) from those of the general project (XG, YG). The X-axis must be radial in the direction of the 1st vibration mode. ![](https://lh4.googleusercontent.com/7gggjB1IG2KG7ouWMi1zAW4vcEE2BgCjQEszxg1DW25WWmiT_BMa_GwLLyJoomygvJ5vLMZUJeshQ53h8hKbjJI6-IR0z_Cfg_-uak9nawWj1GxXAFdo6STgATzkDK4NIarxsD8MY3z-XHUcJd_uTA) The study of the eigenmodes then shows that the fundamental modes of a classical building with well-defined modes are retrieved according to the X and Y directions as well as a torsion mode. This would not be the case if the general axes XG and YG were adopted because each mode would activate masses in both directions, which would disturb the Complete quadratic combinations (CQC) and Newmark combinations. ![](https://lh3.googleusercontent.com/Mr44ZZXbnhJ_QvG7aFuSTQ8weU1Q8V3RAb76mj-tHgEcWOi_W0zksAqy5JSUGpkdaWdpICMSq15osIipccTbVuV41_R7VCufUAOgzPEI6nKbSSZGFTmwHGVAV0ykJfbf56Tn0qJ1UStBskToi7Zp8Q) ![](https://lh3.googleusercontent.com/BimSpdWitl7i4PGsT48lujIiQqtj86JjLi9UcoEU1d-PiMJbZUmg1MdfDAMVrxwYt2sS6JvJc0LehlM3NCsTi_hIps0-j1vcc4eicU4xMhKC662wvDQhR_W6hyHxW_aFYnTLxXDkDxrri1jaAQPceg) --- **Example: Earthquake on a curved bridge** In the example below, two seismic calculations were performed for this TGV viaduct with an in-plan curvature. The first computation depends on the general X and Y axes oriented according to the left abutment and the second with the axes oriented according to the right abutment. ![](https://lh4.googleusercontent.com/8X6Ao6wJ0sex-SBSrD7SPd8dfqn9qq5CNTirdIC4haHUPGfRtkty318eTMVftC7Y95aZ8nVCut-2uemditbSNBVzMlLLf_BviOxAIjNxkQCqWL1iem7ctHb4U3LhjabQXr6J-4RCSA0bvKVUzaxgOA) It is possible to switch from one model to another by changing the coordinates of the model nodes. The comparison of the efforts at the base of the supports highlights very different results between the 2 models. ![](https://lh4.googleusercontent.com/zPkO-lPvWO4P_zIcBRxxynMuNmilRLPWSk1GUQym3skgK0kD8ip2l2aedF6jtz0mYKzo6jzubxKX-CJVXTRwWTcGy-gTzhIJPkfNrpNkrujm_wG396Inu1EONY9RzablaAas-jOYnNiGVCn_WqnIpA) *Graph n° foot support/effort (kN)* Therefore, it is advised to carry out seismic calculations for bridges on straight planar alignments if the curvature allows it (refer to the CEREMA guides). Otherwise, several calculations must be conducted by varying the axes for each support studied, it is a complex solution that should be avoided when possible. --- **C.16.2 Modeling of non-structural or secondary elements** See [C.4 Modeling of non-structural elements or equipment.](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c4-modeling-the-non-structural-elements-or-equipment "C4. Modeling the non-structural elements or equipment") Non-structural elements and equipment do not need to be modeled if their mass is small enough relative to the mass of the building. However, one must ensure that their stiffness do not influence the behavior of the structure. Otherwise, they must be considered. For more information, please refer to §2.4.5.2 of the ASN guide and the AFPS technical book 36 of the AFPS concerning the dimensioning of non-structural elements under seismic conditions. When the mass of these non-structural elements is not negligible, it must be correctly defined in space. For example, the offset of the bridges’ lateral elements’ masses with respect to the center of the sections should be well defined so that the torsion modes are considered. The distribution of the masses on the floors can generate many local modes during a modal analysis and make the model difficult to operate. In this case, it is recommended to apply punctual masses and to redo a local study if necessary. **C.16.3 Transformation of loads into masses** Most software calculate the weight of the structure directly or have an option to do so based on the density or volumetric weight of the materials. For seismic and dynamic calculations, the weights, forces, and pressures must be converted into masses following the normative ponderation factors (it is the case for equipment and superstructures or part of the operational loads). To reduce the number of eigenmodes that are not useful for a global calculation, one can focus on options that transform the distributed masses into masses at the nodes or introduce manually the masses at the nodes. **C.16.4 Pay attention to the units** The accuracy of seismic or dynamic calculations is particularly sensitive to the coherence of the units. Inertial forces involve the acceleration of gravity g, whose unit (generally defined by default) must be consistent with all others.Trivial, but it is always useful to remember that the unit of mass is ... the kilogram.
Be careful when using old standards or regulations because they may use units such as kgf (kilogram-force). In general, **it is advised to use exclusively the international system units, at the very least to control the results**. Taking the simple example of the self-weight calculation. For most software, the action of gravity is defined by the application of vertical acceleration applied to the whole structure. Internally, the software will calculate the mass of the structure by first calculating for each element its volume multiplied by the density of its material. If one wishes to obtain the self-weight in N and the geometrical dimensions and density have been defined respectively in mm and kg/mm3, the acceleration will have to be defined in ... m/s²: ![](https://lh3.googleusercontent.com/yZh-0_Wim8qOTrYIvBtBM1Pvcng7OLJiN200gdpWmRmmGx3tr_4eKHmbtbd48JhSD_7UK1NPCvIF1IwjVGRmYjKXSxkLMDaktxixp_sA9GPBVgFLV02F9dAG2M0BZ-cHVtO9-toJ8YKx1iIH_s98Zw) For example, the mass equivalent to an operational accidental load of 20KN is equal to 20,000(N)/ 9.81(m/s2) = 2038 Kg or 2,038 tons. **C.16.5 Materials** The material laws as well as the partial coefficients depend on the type of analysis performed. Taking concrete as an example, the instantaneous Young's modulus will be preferred. To consider the cracking state of the elements, the EI module can be modified: - either by a minor coefficient applied to Young's modulus E, - or by modifying the net cross-section or the inertia of the section directly. The applied reference frame can specify the Poisson's ratio to apply according to the type of calculation. it can be modified to consider the state of cracking, for exemple, equal to zero in the case of a cracked element or under ALS (Accidental Limit State) earthquake. **C.16.6 Modeling of bracing elements of steel structures** Bracing elements ensure the lateral stability of the structure. It is important to transcribe their actual behavior. For St. Andrew's Crosses, for instance, the bars only work in tension because they buckle instantaneously in compression. Therefore, they should not be modeled in their entirety if a linear calculation is planned. Otherwise, the capacity of the bracing would be overestimated by a factor of about 2. See [C.2 Modelling of the main elements](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c2-modeling-of-the-main-elements "C2. Modeling of the main elements") **C.16.7 Boundary Conditions** Depending on the models, the dynamic soil-structure interaction may need to be considered. If the springs are modeled this way, it is necessary to ensure that the structure do not uplift excessively to remain within the validity range of a linear study. For earthquake studies, the engineer can calculate stiffnesses by referring to the following documents: - "Ponts en zone sismique" published by CEREMA, which proposes in chapter 4.3.3.2 fairly simple calculation formulas, - Seismic Design-Building - V. Davidovici §4.3.4.4 Modelling of the ground by a system of damped springs - Eurocode Collection - Afnor Editions, - Gazetas formulas: which can be consulted in Appendix D of "Fondations et procédés d’amélioration du sol de Davidovici" (or other references). All these documents determine the stiffnesses from the shear moduli and Poisson's coefficients of the soils, but also from the characteristic dimensions of the foundation. These stiffnesses depend on the vibration frequencies of the studied structure. **The case of foundation slabs:** Modeling a foundation slab under dynamic loading is more complex because the springs will have to represent at the same time the vertical, horizontal, and rotational stiffnesses, as determined by the soil-structure interaction study. One can refer to more specific documents for this type of study. Several forms of modeling are possible: - using a punctual spring in the center of the invert affected by the 6 stiffnesses (and 6 dampings), with rigid connections on all the nodes of the foundation slab, Advantage: an accurate representation of the SSI in dynamic calculations. Disadvantage: it is not possible to determine the stresses in the foundation slab because of the presence of the rigid connections that artificially stiffen it. It is then necessary to carry out a local calculation of the foundation slab subjected to the soil pressures deduced from the forces in the central spring. More specifically, in the case of a foundation slab with large dimensions compared to its thickness, this method is not adapted. ![](https://lh5.googleusercontent.com/RoUjktBLXHNRcVpiVV_TEVifmnS1y7mD9tMGto0JWNq4aQHsrfbZX9dbKLvMF9LDhzA9YhVKS7Tjeiru7NrxwlB36yeRQBD6EfUzz2Eg_tOkPcxZ1CEV-kt7axI-D_Kjm00j5RVWGa4Q-Q5Vbt3PHA) - using springs placed uniformly under the foundation slab (as for the static study); In this case, each node of the invert is connected to 3 springs, one in each direction X, Y, Z. The horizontal springs according to X or Y will be deducted directly from the global translational stiffnesses, whereas the stiffnesses of the vertical springs will represent either the global vertical stiffness or the global rotational stiffness in a given direction. This approach implies 3 computational models to analyze the 3 directions of the earthquake. Advantage: simpler model, allowing to calculate the forces in the foundation slab. Disadvantage: one of the 2 vertical or rotational stiffnesses is not represented in each of the calculation models. The torsional stiffness is not incorporated. - putting in place a spring mattress, This type of modeling is mainly used in complex structures, a mattress of springs assigned to each node of the foundation slab allows to represent all the global stiffnesses. Advantage: the SSI is modeled in detail. Disadvantage: the modeling is complex and can only be applied using specific software with a complete understanding of the causes. ![](https://lh4.googleusercontent.com/6Ht4Su_PT8LsBmQrAPYTm6mrXLuShzNbPkRdNg_OfMrP5ICVDLAavn_r8vHiyMCZDCy6FfVXTBVQOJXjRuOk3ujYX1Q5HuR2SJfynvWHVqUX721UzF3RYvugRvq-Fhz582FFPOTsuBCtqrPVZ9SGMA) *Figure: Diagram of the spring mattress, Tractebel image* **C.16.8 Spectral modal analysis** **Truncation - number of modes** The theoretical concept of truncation is defined in the 1st part of this guide. In practice, concerning the number of modes to be used for the calculation, we advise: - not to exceed 100 modes for classical works, - to go up to the cut-off frequency (generally 33 Hz), - to use a pseudo mode for the participating mass that is not being considered (EN 1998-2/§4.2.1.2), - not to be limited to the modes with the most participating masses, because the antisymmetric modes have classically a very low number of participating mass but induce non-zero forces, - to reflect on the relevance of retaining or not local modes in the analysis. **Behavioral coefficients** Since the coefficient, or rather the behavioral coefficients, can be different in each direction, they are incorporated in the definition of the calculation spectra. It is important to check that the calculated displacements are indeed re-multiplied by this same coefficient. **Modes signature** At the end of the combination of spectral responses, the sign of the efforts is lost (all values are positive). This can generate operating difficulties when one wishes to calculate a torsor or when one wishes to study concomitant forces (see D 7.4.5). To reallocate a sign to the different calculated quantities, there are several possible approaches, including those described below: 1. Attribution of the sign of one of the modes. For structures having a predominant mode in each direction, it is possible to allocate the sign of the predominant mode to the calculated quantities. This is interesting for the overall behavior of the structure and is very efficient as long as the participation of this mode is greater than 60% of the modal mass of the structure. On the other hand, for elements responding on higher local modes, this may not be appropriate (see the example of thick floors in industrial sites), 2. Attribution of the sign following a uniform acceleration analysis. For each direction, a unit acceleration is applied, and the sign obtained is kept, 3. Ellipsis method analysis. When the justification of a structural element must consider several stress components, it is possible to establish the range of concomitance of these quantities, so as not to introduce conservatism in the calculation. **C.16.9 Damping** Within the framework of a structural study with a calculation spectrum including a behavioral coefficient, the latter already considers damping. Thus, it is not useful to introduce another one. For dimensioning with an elastic response spectrum, the damping of the materials must be taken into account. When setting up the data, it is important to ensure that the material damping included or taken by default by the software is consistent with the codes and the analyses carried out. For example, it is necessary to distinguish reinforced concrete from prestressed concrete, or welded structures from bolted structures in the definition of material damping. **C.16.10 Time discretization and integration scheme** The resolution of a dynamic solicitation requires the implementation of a specific integration method. Part 1 Chapter 2 provides details on these methods and guidance for choosing the time step and mesh size according to the problem. It is recommended to consult engineers specialized in this type of study. # Chapter D. Analysis and processing of the results #### **Chapter D. Analysis and processing of the results** [D.1 General information about numerical calculations](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d1-general-information-on-numerical-calculations "D1. General information on numerical calculations") [D.2 Load combinations](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d2-load-combinations "D2. Load combinations ") [D.3 Results processing ](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d3-data-processing "D3. Data processing") [D.4 Validation rules: the behavior of concrete elements](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d4-normative-verifications-the-behavior-of-reinforced-concrete-elements "D4. Normative verifications: the behavior of reinforced concrete elements") [D.5 Understanding and analyzing the peaks (case study about concrete)](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d5-understanding-and-analyzing-the-peaks-case-study-about-concrete "D5. Understanding and analyzing the peaks (case study about concrete)") [D.6 Understanding and analyzing the peaks (case study about steel assembly)](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d6-understanding-and-analyzing-the-peaks-case-study-about-steel-assembly "D6. Understanding and analyzing the peaks (case study about steel assembly)") [D.7 Further information specific to dynamic calculations](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d7-further-information-specific-to-dynamic-calculations "D7. Further information specific to dynamic calculations") # D1. General information on numerical calculations #### **D1. General information on numerical calculations** **D.1.1 Calculation time** Computation time (in the broadest sense: solving the system of equations and storing the results) is an essential point of reflection to be associated with Finite Element modeling. It must remain compatible with the budget and timeframe associated with the project. The search for an optimized computation time is even one of the key elements when considering the economy of a project. The calculation time is influenced by different factors. - The finite element model: - Number of degrees of freedom, - Formulation of the elements, number of integration points. One can optimize the computation time by using simplified models, sub-models, sub-structures, symmetries, or locally adapted mesh sizes. However, be careful with explicit calculations because the time step is set based on the dimension of the smallest element. - The computing capacity: - RAM: random access memory (temporary storage), - the operating system (32 or 64 bits), - is the calculation done locally (on the user's workstation)? on a local server? on an external server? Model and results copy times, or the time it takes to launch other calculations on the same server can be long, - the capacity and number of processors: the "CPU time" (Central Processing Unit) usually provided by the software should be checked. Optimizing a given computing system can consist of performing the calculation in batch (launching the calculation in command lines without the interface), or parallelizing the calculations (on several processor cores), and/or performing further calculations if the software allows it. - The type of analysis: - Linear/non-linear and the associated algorithms, - Numerical integration scheme (direct integration/modal-based projection, implicit/explicit scheme) and the choice of the solver for dynamic calculations. The type of analysis is specific to the problem and the desired accuracy of the results. Therefore, the modeler oversees the optimization. However, it is emphasized that in the case of a transient calculation, the duration of the calculation (in terms of loading and response of the structure) should not be overestimated so as not to add unnecessary calculation time (machine time). - The anticipation of "post-processing": - for some software, it is possible to select (and keep) only the quantities of interest chosen by the user, as well as the instants (in the case of transient or phase calculations): the machine time to write the results is then reduced, - the number of saved/reused modes in the case of a modal analysis can generally be modified (definition of variable filters depending on the software), - the real-time visualization of results can be used to stop a calculation in progress (but it generally leads to an increase in calculation times), - the analysis of the results can be performed using post-processors independent of the Finite Element Calculation software to reduce the operating time. The automation of the calculations and post-processing (after validation of the first calculation round and using appropriate verifications ) is interesting when the user has to perform the same calculation several times on different models or similar calculations on the same model. **The acceptability of the calculation time must be assessed because the model will run many times and will become more complex as the study phases progress.** **D.1.2 Convergence of the software – The case of direct elastic calculations** In direct elastic calculations (linear static calculation and spectral modal calculation), there are very few reasons for the software not to converge: - either the structure is unstable, - or the inversion of the stiffness matrix is impossible because there are stiffness differences between the elements that are too large. All error messages, at this stage, are related to these two cases. Due to the boundary conditions in place, the displacements, translation(s), and/or rotation(s) of certain nodes of the structure are imposed (a blockage is a zero imposed displacement). However, the set of these blocked displacements may appear insufficient to prevent an overall movement of the structure. It is advised, by choosing an appropriate reference frame, to analyze the effects of all the blockages on the overall movements of the structure and to add one or more restraints to ensure the stability of the structure. At the end of the calculations, it must be verified that the reactions due to these additional blockages are null or negligible: effort for a blockage in displacement, moment for a blockage in rotation. Some software, for specific geometries of structures, ignore the problem of instability. In this case, the stresses and deformations are correct, but some displacements are somewhat unreasonable. Another instability issue often encountered is related to the connection between different types of structural elements. This is specified in [paragraph C.6.3](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c6-connections-links-assembly "C6. Connections - links – assembly").It should be noted that software error messages are sometimes not very explicit about the global, local, and/or numerical nature of the instabilities. Furthermore, some software programs allow the calculation to be completed despite a warning or error message. This can help understanding or visualizing where the problem comes from, but the results are not satisfactory in this context. In the end, it is necessary to have a model that runs without errors.
![](https://lh3.googleusercontent.com/9keNCdpaVa2nNP1dzcqayP6l5AFb5e5xcaM5ibMxUZDQjFj-0CmK3q8e_FVcvR1UFg83EvtN-QiGeSZJwXJ_Rqx9YyB6lWzpjiCYVWNXsbO3U5NgQPMIpE-2uCxnoGSUKmY-hpJMNwwWuIjiuuh2zQ) These problems of global and local instabilities can be detected by performing simple calculations: - either linear static calculations by applying a global acceleration (10 m/s² for example) to the structure. Three load cases can be created according to the 3 main directions, - or a modal calculation (determination of the first eigenfrequencies). If the structure presents global instabilities, the static calculation is unlikely to succeed whereas the modal calculation will present rigid modes. If the structure presents discontinuities, they will be highlighted by the shape of the deformation or the eigenmodes. Be careful, taking into account the shear stress deformations leads to failures in the deformed shape. **D.1.3 Convergence of the software - Case of iterative calculations** For non-linear calculations, the convergence of a Finite Elements calculation is obtained with a function interpolating the solution for each of the finite elements (principle of discretization). The convergence criteria are either given by the user or taken as default values by the software. The finite element calculation consists of a series of iterations and stops either when the maximum number of iterations has been reached or when certain deviation measures between two successive iterations are below the predefined thresholds (this is called the convergence criteria). On the other hand, a calculation that has stopped does not mean that it did not converge towards a valid solution. For example, deformation criteria that are too loose compared to reality, or a maximum number of iterations that are too low, can output a result that is not realistic. **D.1.4 Model Convergence** A model is considered to have converged when a small change in the size and geometry of the meshes does not significantly disturb the results. To be rigorous, it is advised to carry out a sensitivity study of the mesh to the post-processed quantities. Thus, carrying out the same analysis on different meshes (reduction of the mesh size, for example), should - if not provide similar results (acceptable tolerance) - converge towards an acceptable solution to the user. It is important not to focus on peak values and to bear in mind that several successive refinements of meshes can lead to divergent results. It is also advised to analyze the software's warning messages ("Warning" on mesh size or shape) to assess whether they are likely to alter the results. # D2. Load combinations #### **D2. Load combinations** **D.2.1 Combinations and envelopes** Recall that using a load combination consists of accumulating the structural effects of different loadings by assigning weighting coefficients to the different loadings as defined in the standards. Strictly speaking, the codes require all combinations to be verified. In the case of a building, the number of these combinations remains small, so the software can calculate all of them. However, for more complex cases, and particularly in the case of rolling loads, the theoretical number of combinations becomes unmanageable. In such cases, force envelopes are used. An envelope contains several load cases and only records the extreme values of the individual components (with the concomitant components). According to the codes, some loadings applied to the structure should not be accumulated because both occurring at once is not a reasonable assumption. It is then useful to incorporate these non-cumulative loadings into an envelope that will highlight, for each effect studied, the most unfavorable loading among a group of non-cumulative loadings. Thus, for bridges, the envelopes of thermal, wind, and road loadings are generally considered. Remember that accumulating unit cases calculated by a non-linear approach (NL) has no physical meaning. However, some software allow non-linear calculations on "combinations". In this case, the software will create a new case (the "combination") from the unit load cases and perform the NL calculation on this sum of loads. If the software does not allow it, it will be necessary to create combinations by manually grouping the unit loads. In this case, it is, once again, fundamental to understand what the software does. --- **Illustration of the above text using an example** A secondary gallery of a tunnel is considered. The structure is fully supported by non-linear springs – since the ground does not take up traction, the springs are blocked by the software if there is a soil-structure separation. *![](https://lh3.googleusercontent.com/xgBN7TgVUygQ1m6EOClOGUz4G6vctV5mhHjaIOURrkO9j-OLl0Ne0H5735cK83oP29NPo6epd31ylZrTtMSlgvCwwJ8Fs-gDenx21moYYfhsFec2nDWLdpR7_SijJ8FQdmVOasvnPHpZaYZkYchz4w)* *Illustration of the structure* The following two unit cases are defined: - self-weight + earth weight and thrust, - hydrostatic pressure. *![](https://lh4.googleusercontent.com/5OAFCVcNzDuGR-oDO2bEef9Rb2n3IYTOE0-zwR0amguMc4aSqyk4PuubraqvMf6La4cx7-MPfcy-vF1iYdU_wwPZxaze03sCpKr-qms0w1JSzr8os-Mq8P_pHm1z72weWJSqIDuBAgLw55VRVA-w9w)* *Gravity loads (left) and water pressure loads (right)* The following results show that although the software can conduct non-linear calculations using all the unit cases, the combination of the two cases is recalculated integrally and independently... ![](https://lh4.googleusercontent.com/orhgUX2RttZh4oNDafl2sANgW_dsTKDaf9jAHpBvEzIKS-Ho1rhv68nRCTArtZjCWblHGUpBYS77sTMs_m0j2E2VovR9siRFjWZ9vPR_3lydD-WckONu7xdiPiygwvqA19aoiiKhKgi8SIV66u_Vww) *Results of the unit cases: bending moments - gravity loads (left) and water pressure loads (right)* ![](https://lh4.googleusercontent.com/YwTbinFj0jBMbYcsAmdz4sBJNojYRZ_ztVt_dTi8PNEHxqMVfmmqt5Bc7UEJYccqAv56ZuVtg9WRpEev0_GwE9QQSdlncqPd1uuj0SDOfhyPImgUfwaAlWy8O27dyeRta3jb1shmZ4tT3nLW6eJKhQ) *Results of the combination of the two cases: bending moments - software combination (left) and cumulative loads in a new case created manually from the unit cases (right) - identical results* ... since the accumulation of the unit cases does not lead to the results of the combination. The diagram of the **pressures on the soil** speaks for itself: the water pressure forces the vault to rest on the ground "upwards" at the top (right figure) ... *![](https://lh6.googleusercontent.com/4v6ABmSPlAhcOLpQLwzTgUNtRGyBv8RjF_bb_GJdpG5Wc3xj5Iy01yj-xMhy9J77mhCtjhgew8CU4TJovrB59wUiYPG2k0BirNAEHmumqxM0uKYMjFOcz5N3JGsewp9oSeXnGH5uqvWpopU2XIZR-A)* *Soil pressures under gravity loads (left) and water pressure loads (right)* ... but once accumulated in the case of gravity loads, the top of the vault no longer pushes upwards, which can be seen on the results of the combination made by the software: *![](https://lh4.googleusercontent.com/TbiTH1Ryq7ByJTy1CTg-0_pKmJmVc9vnzyHcZX0JRfHUHuD-myVuViWia9yqRZ7BqscxMxyiE4dR0Joh-M0_qVKB1NBftChRP9e7becims9f4jdpBVJizxXxEhHsKKvlfIk2yzQtfnnOzM4WVmBzhQ)* *Soil pressures from the combination of gravity loads and pressures* Note: without springs on the arch, the second case would not converge. --- **D.2.2 Be careful when using the envelope results** When using envelopes, one must record in a database the displacements, extreme stress values, strains, or reaction forces at the supports. Most calculation software offer the possibility of storing the extreme values of stresses and strains, either alone or together with the values of concomitant stresses and strains. Before using the results of the envelopes for further post-processing, one should clearly understand whether the stresses and strains are concomitant. For example, if one wants to reconstruct the most unfavorable stress state of a section, it should be verified that the extreme stresses selected for the upper and lower fibers are indeed concomitant. Also, it is important to base the analysis of the results not only on the most unfavorable stresses and their concomitances but also on the concomitant stresses that generate the most unfavorable stress states. Thus, a maximum normal stress associated with a small concomitant moment can generate less unfavorable effects than a slightly smaller normal stress associated with a larger moment. To verify a section, it is acceptable in upstream phases to perform the verification with all the extreme stresses in the same torsor. However, in the execution phase, for optimization reasons, it is advised to recover the torsors of concomitant stresses. **D.2.3 Beware of automatic combinations!** The combinations of loadings are used differently for building or other civil engineering structures. For buildings, elementary loads induce a very large number of possible positions, all of which must be explored to determine the maximum effects on each structural element. This multiplicity of loads and configurations leads very naturally to the use of automatic combination modules. In general, the automatic combination modules proposed by most software should be used with great precautions because it is a frequent source of errors. Some modules are black-box modules and not all software are allowed to know what are the elementary load cases used for the envelope combinations. Moreover, the verification and coding of the combinations is a tedious exercise for which it is difficult to detect the error. One of the most effective methods to prevent errors related to combinations and envelopes is to dissect the design stresses and strains. For some key stresses or strains (maximum bending moment, extreme stresses), it is a matter of finding the participation of each design elementary load in the overall stress or strain. Thus, one can verify that there are no errors in the accumulated values and coefficients and that the "logical" load cases are design loads. For buildings, the same exercise can be done with the reaction forces at the supports. # D3. Data processing #### **D3. Data processing** **D.3.1 Stresses/Deformations or Internal forces** It is important to define what you are looking for before starting the calculations, and this depends on the type of study: - for structures modeled as beam elements, we will prefer processing internal forces, - for civil engineering buildings, the stress approach allows us to understand the overall behavior of the structure by identifying different zones. On the other hand, when the objective is to obtain reinforcement results (quantity or internal forces), it is necessary to process the internal forces and to carry out the corresponding calculations in a second step. **D.3.2 Values at nodes, Gauss point values or values at the center** See also [A.2 What is a finite element?](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/a2-what-is-a-finite-element "A2. What is a finite element?") Generally, the software calculates the values of stresses and strains at the Gauss points, whose position is defined in the software's finite element manual. It can then infer the value at the center of the element. It extrapolates to each node and, since a node is usually linked to several elements, it computes the average of the values obtained for each element. In regular zones, and with a proper mesh such as shown in [paragraph C.3](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/c3-fe-and-meshing "C3. FE and meshing"), the values at the center, at the nodes, or the Gauss points are very close. The issue arises close to the peaks, where it is necessary to reflect on the most representative values. **Types of values displayed** Most software calculates the stresses at the integration points (or Gauss points). But there are two ways to visualize them: - at the elements – This method consists of directly plotting the average value on each element; an average of the values calculated at the integration points of the element. The plotted stresses then present discontinuities, which are accentuated when the discretization is not well adapted to the zone of interest. The results displayed in the center of the elements are reliable. - or at the nodes - This second method consists of displaying the mean values at the nodes. For each node, the calculated value is the weighted average of the stresses from the selected elements adjacent to the node. This treatment, called smoothing (\*), is intended to display a continuous field, which may seem more relevant. ![](https://lh4.googleusercontent.com/E9ccDDSM6rG5LSk8sxhXbqCNOLEPJEstVhxaG_tQM9GOfPIhsaXEp2a9kByEpiW5Z9CE-xr1F2M-PyjHN_Sbs1gGwE8g3hUNrYN4BZbaafgFJ46wd2m276N4dTQdJbXs7wM56qS92O7y5A3SblBdRg) *Stress field - Principle of calculation of the displayed values* (\*) Do not confuse this smoothing action with the smoothing described in paragraphs D.5 and D.6, which consists of computing average forces over a given length. In the figure below, the stresses calculated at the integration points have been extrapolated to the nodes before averaging. This is what some software packages do by default. We can illustrate it using the example of the Br wheel ([**Example D - Simple case: modeling of a Br wheel**](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-d-simple-example-modeling-of-a-br-wheel "Example D - Simple example: modeling of a Br wheel")). The software used does not give access to the values at the Gauss points. *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/piltGf8JWQw9lCOi-embedded-image-mavdnzzr.png)* *Mapping of transverse bending moments - values at the center of the slabs - overview (28.52kN.m/m is an extreme calculation value)* *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/LM5RsuBkfM8y7h9p-embedded-image-h6hsqms9.png)* *Values at node 3 - they are different depending on the finite element* *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/tIRw8fSGwMJbRUeq-embedded-image-3mimzijv.png)* *Values at the center of the elements - Zoom* Each software documentation should provide information on how it displays the solicitations and the options available. By default, software can propose that the linear part of the result of the integration point is extrapolated to the node while the non-linear part (plastic deformation for example) is copied. And an option in the same software allows the linear and non-linear parts to be copied to the nodes. We will see later in [**paragraph D.5**](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/d5-understanding-and-analyzing-the-peaks-case-study-about-concrete "D5. Understanding and analyzing the peaks (case study about concrete)") the important variations that can be linked to smoothing the results at the nodes or elements. **D.3.3 Stress Analysis - Identification of Sensitive Zones** To follow up on the above details, displaying the stresses at the elements allows better visualization of areas of high discontinuity. For steel structures, software usually display the equivalent Von Mises stress, which gives an idea about the zones of high stress and/or with a high-stress gradient. One can also display the internal energy of deformation of each element. In reinforced concrete structures, either the stresses are displayed, or the reinforcement mapping, which allows visualizing the highly stressed areas. # D4. Normative verifications: the behavior of reinforced concrete elements #### **D4. Normative verifications: the behavior of reinforced concrete elements** ##### **D.4.1 Reinforcement mapping – reinforced concrete normative verification / connecting struts** Calculations of reinforcement mapping are carried out by the current software generally by using the method of Capra Maury (Annals of ITCBTP - Institut des Techniques de la Construction du bâtiment et des Travaux Publics - of December 1978) or the method of Wood and Armer (“The reinforcement of slabs according to a predetermined field of moments" Concrete February 1968, August 1968). These methods render it possible to determine the necessity of reinforcement in the 4 directions Axi, Ayi, Axs, Ays on the lower and upper faces of an element according to the 2 directions of reinforcement considered orthogonal, X and Y. A good approach to the calculation of these mappings can be made from Wood's method by simplifying: Either an element subjected to the following stress components: - Nxx, Nyy, Nxy membrane stresses (positive if traction) - Mxx, Myy, Mxy bending stresses The first step is to calculate the following intermediate stresses: - Nwx = Nxx + |Nxy| - Nwy = Nyy + |Nxy| - Mwx = Mxx + |Mxy| if Mxx is positive, Mwx = Mxx - |Mxy| otherwise - Mwy = Myy+ |Mxy| if Myy is positive, Mwy = Myy- |Mxy| otherwise ##### **D.4.2 Bending elements: slabs** The slabs work mainly subjected to the bending moments Mxx, Myy, Mxy. The membrane efforts Nxx, Nyy, Nxy are often negligible. The Mxy bending moments can be important, they are null in the zones where the principal bending moments are aligned with the principal axes (often confused with the directions of the reinforcement) and therefore in the middle of the span and on continuous supports. They should not be neglected especially in the corners of the slabs and in the case of concentrated loads. The calculations of passive reinforcement carried out in the determination of mappings are according to the rules brought by the Eurocode, because they are adapted to the study of a rectangular section subjected to combined loading (N, M), they can thus be carried out in SLS and the ULS. The calculation of the reinforcement in SLS considering the crack openings is more delicate and requires the use of well-tested software. Indeed, the presence of MXY bending moments requires steel calculations on several facets because cracking does not necessarily occur according to the direction of the reinforcement. As the behavior of slabs in bending is similar to that of beams, it is necessary to redistribute the bending moment diagrams to have a truss-like behavior. The reinforcement areas Ax are calculated directly from the efforts (Nwx, Mwx) and the reinforcements Ay from (Nwy, Mwy). --- **Example: 5m square slab** The slab is hinged on 3 sides and clamped on the 4th, it is subjected to a uniform permanent load of 50kN/m², a thickness of 20cm, and a concrete cover of 3cm. ![](https://lh3.googleusercontent.com/U1KCPpBPLVzuAc_BSiLkWDemHUF7mDlGraW5EpZHfRwtNis6w0cCWzEab-NvQ2gvYvhBCozhEc8gDXTadnOjmh8ylT1-7TaWrOc0tlW2qzZ0Q9RQF5RLR0iTDr1xAqo9HiqkKOPEtO6tfMJIFKAwOw) ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/sKePxw1gPAE2sTe1-embedded-image-lrnrvc1a.png) *Horizontal bending moments M_{YY} | Bending moments M_{XY}* Ay reinforcement is calculated manually with fyd=200MPa (SLS). ![](https://lh6.googleusercontent.com/Bd4Ies4SAvASzx1e0Fnv8Kgdj4jWaif8Cqt0xLZHainzxIXuTChW_BrczJOuRgnock--l5VtD5Tv4CEN-1_rU2AzH8bn8q3TRyKrA_eGPDGU3dkgezv30Rd5olDBUsBa6CWpdHclzuP2yipcsV2WUg) Ay manual = 10 x (M_{YY} + M_{XY})/(0.9 x 0.17 x 200) cm² Values that can be compared with the reinforcement areas calculated by the software: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/Be6Jv67bfZLbaPnx-embedded-image-b1zauhuz.png) *Reinforcement Ays software / Reinforcement Ayi software* There is a good agreement between the reinforcement calculated manually and the one determined by the software (CAPRA MAURY method). It can be deduced that the Mxy bending moments are cumulated with the M_{xx} and M_{yy }bending moments. --- ##### **D.4.3 Elements submitted to shear forces in their plane: concrete walls** The bracing walls of a building are subjected to normal stresses and shear forces in their plane. We have the examples of "large dimension walls of lightly reinforced concrete" studied in EC8-1 chapter 5.4.3.5. or transfer slabs of buildings subjected to horizontal forces (inclined columns). For these elements, the components Mxx, Myy, Mxy, Vxz, and Vyz are very low or even null. They are only subjected to membrane efforts Nxx, Nyy, Nxy: - Nxx and Nyy being the tensile/compression stresses along x and y axes - Nxy the shear in the plane of the wall. Taking into consideration the previous calculations of reinforcement distribution, this gives: - Nwx = Nxx + |Nxy| - Nwy= Nyy + | Nxy| Hence the reinforcement: - Ax = (Nxx + |Nxy|)/fyd - Ay = (Nyy + |Nxy|)/fyd - Ax and Ay being the sum of the reinforcement in X and Y (2 faces included) - and fyd is the design stress of the rebars These formulas lead to the observation that if the normal stresses are zero (Nxx=Nyy=0), then the reinforcements Ax and Ay are shear reinforcements and their values are equal to Ax= |Nxy|/fyd and Ay= |Nxy|/fyd. Hence, shear efforts require reinforcement in both directions, as opposed to the classical shear verifications performed according to EC2. This is because the strength of the concrete is not accounted for. Therefore, the shear reinforcements calculated by the mappings are "higher" than those usually calculated using EC2. Article 5.4.3.5.2 of EC8-1 concerning the study of "Poorly reinforced large dimension concrete walls" was consulted so that no shear reinforcement is required Ved is lower than Vrdc. Thus, it is recommended in these cases to use reinforcement maps only to consider local effects, and to perform calculations of the main reinforcement by taking cross-sections at the base of the walls and to determine the reinforcement from the resulting torsors at the level of these cross-sections. --- **Example of a sail:** Let us study an isolated concrete wall, 5m high, 4m wide, and 20cm thick. It is clamped at the bottom and subjected to a seismic horizontal load of 2000kN at the top. To avoid peak efforts, the horizontal load is linearized over the width of the concrete wall (500kN/m). The resulting membrane forces Nxx, Nyy, and Nxy are illustrated below. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/rUetMBDlNB6a6qEV-embedded-image-cyrxna4z.png) Stresses Nxx (horizontal) (kN/m) – Stresses Nyy (vertical) (kN/m) ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/4RiU4x0xU8WyvldZ-embedded-image-lfkal5bz.png) ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/XUGttYszNmMGYbAZ-embedded-image-txklioth.png) *Stresses Nxy (shear) - Reinforcement mapping (cm²/m²) for one layer* The steel sections are calculated manually and compared with the map values. ![](https://lh4.googleusercontent.com/nOw44XoZ1Tzl3dQHrZcehNALF2c-Ywk5h9Js59D8qH9k26bH-u3gTiS-WTsC9yOuC72I9mcpVYZyxGsd3wi0puzAtdk2IomHig4-2CFZexDLZitr4t9Qu1u2dSdlAN1PkFbZYvDwJ7BUePlffI5K6Q) This table shows that, on one hand, the manual calculation provides a good approximation of the required reinforcement section and, on the other hand, that the shear efforts Nxy are added to the two membrane efforts Nxx and Nyy, which does not reflect the real behavior of reinforced concrete walls. Normative verifications of a reinforced concrete wall: The reinforced concrete wall is recalculated according to EC2. At a cross-section at the base of the wall, the resulting efforts are equal to: - M-flection = 2000 x 5 = 10 000kN.m - Vu = 2000kN (ALS) Hence the bending reinforcement: A-tension = 10 000 /(0.9 x 3.9 x 50) = 57 cm^{2} or 29cm^{2} per layer. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/btTr75Qpok4RZW3Y-embedded-image-gjgd4rsl.png) Vrdc = 997kN is lower than Vu = 2000kN so, 11cm²/m of shear reinforcement must be distributed (6cm²/m per layer) considering cot(θ)=1 or 5 cm²/m with cot(θ)=2.5. Comparing the 2 methods: The bending reinforcement is more important using reinforcement mappings, (36+23+15) cm²/m x 0.5 m= 37cm² compared to 29cm² using the normative verifications (30% greater). For the shear efforts, 7cm²/m must be distributed using the reinforcement mappings whereas the normative verifications allow distributing only 2.5cm²/m considering cot(θ) = 2.5. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/3DzBDKbvDpAZIyym-embedded-image-kmwwdnsl.png) *Summary of the comparison between the calculation of a reinforced concrete wall either by the reinforcement mappings or by the normative verifications for reinforced concrete (EC2).* ##### **D.4.4 Cross-section method** Most software allow to “cut” the elements to calculate the resulting torsors in their centers. Let us do a study case on the base of a reinforced concrete wall: ![](https://lh5.googleusercontent.com/Dq9yKay1SkIim6Y34fcT66DU-Catd0TwBKPmKqxCDOi-cwQWJtQBajSyKarDKM_LVzKm3DOTCZIdvAanpL5tpGb9j_RSOwinZpptuYY8vmGzqq4im9dptTnoFN9UbXwxjRhw3M2LZfEiSsSHVu9s3A) The horizontal cross-section at point 0 at the base of the wall allows obtaining the resulting torsor consisting of the normal efforts, the shear efforts, and the bending moments (in-plane or out-of-plane), by the integration of the stresses. The reinforcement can then be determined by using a beam type calculation, for which one must be sure to stay within the definition range of a beam element. The use of cross-sections is above all very useful for the engineer to quantify the stress paths in a structure. ##### **D.4.5 Scope of validity of steel mapping** **D.4.5.1 Mapping and cuts** Reinforcement mapping is the result of a numerical calculation carried out for each element independently, therefore without considering the overall reinforced concrete behavior of the structure. Note: The cross-section method is the only one that respects the behavior of the reinforced concrete walls and is considered normative. The usual additional verifications must be applied: redistribution of bending moment diagram, verification of the connecting struts, lapping, and minimal reinforcement ... is still to be done. Therefore, the engineer needs to validate the obtained results with other normative methods. Example of a wall-beam calculated with the reinforcement mapping: The example of a beam on two supports is studied here. The beam is modeled as a tall wall-beam, to show on a simple case the inconsistencies of the reinforcement mappings. Let the isostatic beam with a 10 m span, 3 m high, and a uniform load of 200 kN/m². This beam is modeled in plate elements working in their plane with a mesh size of 0.5 x 0.5 m². ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/1BvX6eXw2hWuc6wH-embedded-image-wbuate9z.png) *Visualization of horizontal efforts Fxx* Calculation of reinforcement with reinforcement mappings: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/e7DB1K8reo5OTKmX-embedded-image-we2rx8np.png) The bending capacity is equal to F0 x d0 = 2 layers x 0.5 m x (24 x 2.75 + 16 x 2.25 + 8 x 1.75) = 116cm².m. The resulting reinforcement is equal to Ax = 116 cm².m / 2.9 m = 40 cm². Calculation of the reinforcement with the cross-section method: This second method consists of “cutting” the beam in the middle (A-A). ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/4dcpbAFRjgttjCLq-embedded-image-6ndruggg.png) The software integrates the efforts Fxx along the height of the cross-section to deduce the resulting torsor in the middle of the cross-section. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/0hmglEgADQhkSYgV-embedded-image-oql6spjs.png) The bending moment at the center is equal to 3358kN.m, (we then find the classical bending moment using Strength of Materials, Mu=1.35ql2/8 = 3375 kN.m), hence the reinforcement calculated according to the rules of reinforced concrete: A = 3358/(0.9 x 2.9 x 43) = 30 cm². Conclusion and comparison between the two methods: ![](https://lh4.googleusercontent.com/fWZEujWhh9qOosr69tZzUM2-0BC_EBvRy-BqOVeFOAl1pzV_0a2-GXwWkOhJWELgs5fdMD9ToKXduX8-YU5YGBYVI4mMNBHBqs-o2PhRdiZIuMvrbSBaiQ93tdi9asb44iI-6Kkq1UClz5AgQR923w) *Reinforcement resulting from the reinforcement mappings / Reinforcement resulting from the cross-section method (Reinforced concrete calculation).***Conclusion**: This example shows the limitations of steel mapping since it does not respect the deformation rule for reinforced concrete. The cut-off method makes it possible to optimize the reinforcement.
**D.4.5.2 Strut-and-tie method: Finite element contribution** **Case of a wall-beam** The Eurocode 2 strongly encourages the use of the strut-and-tie method, in this case, finite elements can help the engineer to define the operating scheme of the connecting struts as well as their inclinations. Let us consider the example of the following wall-beam: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/u344fICMnJ0tlS5S-embedded-image-rrf3wvws.png) As the span of 3m50 is smaller than 3 times the height of the beam, the classical rules for beams do not apply (EC2-5.3.1), this wall-beam is calculated using the strut-and-tie method. As this example is quite simple, we can manually define the strut behavior: ![](https://lh5.googleusercontent.com/OQ03oUS5zZslijc8a6m40a1ld7yfzQOUr2B90itx06Dh0gdMCxiLjLAqYCg7AX_j3g7W3FPrTfkSV5xdvTQf8Pp8aQY3GZcfv4uJOMgox2LUuWR01TaISoM_v2IyF2vXgoUHOqaCPD6fkSFwH56hNg) The usual rules estimate the height of the connecting strut Z in 1.90m, we obtain tg(Θ) = 2.18, i.e. a tie with H=515KN, or a theoretical reinforcement area A=11.8cm² (ULS calculation). In more complex cases, the engineer will have to define a strut-and-tie behavior which may be difficult. The finite elements then bring precious help for the engineer, we propose to follow the following method: **Representative isolated model:** It consists of creating an isolated representative model of the problem. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/9bRo3KKffT60GqxV-embedded-image-4v3sl4sv.png) *Isolated representative model* **The principal stresses:** We will also refer to part 1, chapter E.3.3. What to remember: There are 2 principal stresses, the min S1, the max S2, they are represented as perpendicular arrows, the length of each arrow depends on the intensity of the stress. The S1 stresses show the negative compressions and S2 positive tensions. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/tDnIgZ1vSffGxpzO-embedded-image-5z9tufuh.png) *Principal stresses S2 (compressions)* ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/XbG0SN80SC3kVFWN-embedded-image-e6lzydlf.png) *Principal stresses S1 (tractions)* In our case, the long blue arrows show compressed zones, the red ones show tensioned zones.**Nota bene**: when the 2 arrows S1 and S2 are almost equal, i.e. when the representation is a cross, then the zone is in pure shear.
**Definition of strut-and-tie behavior:** ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/zVGr8VqaRv0EiBUJ-embedded-image-obsufyka.png) The visualization of the compressive stresses at the base allows to visualize the direction of the connecting struts, its angle is of the order tg(Θ)= 2. Hence, a tie with 562kN from which a reinforcement area A = 13cm² with some uncertainty due to the graphical method. **Reinforcement mapping:** The reinforcement mapping directly reinforces the lower tie: ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/MovTStN9urM3fMHt-embedded-image-4lwe0xjv.png) The reinforcement area along 1m summed results in 5.07cm² per layer, i.e. 10cm² in total. This more precise value can be retained. **Balance sheet** This approach makes it possible to identify the stress path and to set up a model of a suitable connecting strut (compatible with the stress path). *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/CVCmCU717yq03efJ-embedded-image-vkentq50.png)* *Load path in a wall-beam with multiple openings, S1 stresses* *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/gkHZmTmQTThtatyr-embedded-image-vnhbgsu4.png)* *Load path in a wall-beam with multiple openings, S2 stresses*The reader might refer to §8 "Strut-and-tie modeling" of the FIB Bulletin nº45 for details on modeling this type of approach and to [SETRA Bulletin Ouvrage d'Art nº14, pages 23 to 32](https://cloud.afgc.asso.fr/s/NkLf5KTRem5YqCB).
# D5. Understanding and analyzing the peaks (case study about concrete) #### **D5. Understanding and analyzing the peaks (case study about concrete)** The smoothing referred to in this chapter concerns the clipping of stresses or strains or the distribution of reinforcement, by averaging it, over a certain length (or width) of the calculated element. ##### **D.5.1 Stress concentration and peak stress (forces) - Different types of stress visualization** **D.5.1.1 Stress and strain peaks** Contrary to common ideas, stress and strain peaks did not appear with finite element software, but have always been part of the stress of structural engineers, they are inherent to the inclusion of point forces in the calculation of slabs. Let us consider, for example, the study of an infinite isostatic slab subjected to a load concentrated in its center. --- A possible approach to calculate the forces in the center of a slab is the use of Pücher’s charts. ![](https://lh4.googleusercontent.com/00GNZ9heeKe5VnzjzAqCYiPNlKGhv3v7k5xLPmbCkScLhXipk9rnW09aubGTD47x-IXy0wbXk2-GGwLFZAZS6IIygQX0wEixVMID0W9XXF4rX_82AOQi2svoo0Uq1u230tj7FjNAtEkichfyvfwc1A) ![](https://lh4.googleusercontent.com/yMza2ZnmT5Mv65HAg8sFmX5mUJJkPRKDtSXd-y-kqH4nVPl6_WhsNntRD0dvpmUDR36tGBArcTfHux8x8zwiUd2AaoDHyTSMmCM0t226k_D_Z5YjyvKnJMQqyojoPmNeVfYXIz-M6Jiw-JLHi4LiiQ) The chart above (surfaces of influence) shows a peak of moments in the center: the line of influence increases rapidly as the load approaches the middle of the span: the values 3 / 4 / 5 then 6 and 7 narrow to an value which is infinite, but corresponds to a surface tending toward 0. Pücher arbitrarily truncated the representation to the value of 8. Let us consider a slab with a span of 3 m articulated on its sides, subjected to a concentrated load of 10 KN in its center. According to the chart, the theoretical moment at the load is infinite, which is not satisfactory for the engineer who has to dimension the reinforcement. In reality, point loads do not exist, especially since the common practice is to diffuse the loads to the layer of a slab. We are then led to calculate integrals to obtain the value of the moment in the slab (for more details, please refer to Pücher’s original publications). By distributing the load over a 20×20 cm² square, the integration of the surfaces shows that the maximum moment is equal to 3.0 KN.m. Another example of the use of Pücher’s charts is given in the example of modeling a Br wheel. It should not be forgotten that the calculations are generally carried out with raw sections (formwork) and elastic materials (linear behavior). In reality, the cracking of reinforced concrete will lead to a redistribution of forces that tends to reduce these peak effects. This type of calculation is not (to date) current practice. It is therefore necessary to know how to correct simply, often manually, the results of a linear calculation. Examples of correcting the results of a linear calculation are given below. **D.5.1.2 Finite Element Peak Studies** What happens when this same slab is calculated using finite elements? ![](https://lh5.googleusercontent.com/5DCGb-YTvYbp9_pmpAa1VniFrywDPTSAhtE9OeObDjQVjpGolQkszlBZsPMaJA41TDMpRndXCX2KsUk7QoWIyFBImTRqkaMLnJF70C-TQWhAyJtiPaj17yJKqwhNFpafb_1BfqV-Oq0apCM1lQo4lQ) Slab of 3 m articulated span subjected to a concentrated load of 10 KN at its center (node stresses) *![](https://lh4.googleusercontent.com/BeXFIcMUrbPqlB2xwjZB1BVh4wUjVC4M6VQoirf8LBqYvy1tN9eXIpvrsg_ekfnuUeLU-I2pNvCXfNSEb73zB-7BokAcMMhsbXhhFEVkyL0m1d-O_BIBIAcUPEyXmGW2YNjLuzdVCTH8hZe4_TX7gg)* *Same in 3D* We note the appearance of a peak whose maximum value is not infinite, but equal to 2.96 KN.m. We saw that the software calculates the efforts at the elements' integration points, then extrapolates the results to the center and then to the nodes of the elements. A node is generally common to 4 elements, so there are 4 results per node (one for each element). What will the chosen result be? The maximum value? The average value? Indeed, finite element software does not propose a single result for each calculation, but several results depending on the options chosen by the engineer: the software is able to draw up maps of results from the forces on the nodes, or from the forces at the center of the elements, they can be smoothed, not smoothed, etc. The engineer must choose the visualization options carefully, as the results vary greatly depending on the option chosen. This is what we propose to show with the example below. The previous figure shows the moments calculated on the nodes of the elements whose maximum value is 2.96 KN.m, it is very close to the value of 3.0 KN.m calculated manually. We take the same example by displaying the calculated moments in the center of the elements (instead of the nodes); the central peak is smaller: 1.92 KN.m for 2.96 KN.m previously. This result is also far from the manually calculated value of 3.0 KN.m. ![](https://lh4.googleusercontent.com/-iYEcSTVzjsZAxZYVBaqww1m37x1wFWO7zVrFHWwTqGvNr9UZ7HMSiajxS-67wI8quC0ZXD8n1BaDfsXbJZWHKfnf1oHTAq6XYhtZ4W532KJC_9774ZxyKADwf4J5TWM1DieOu1v3p3Ivi7me1dpJA) Slab of 3 m articulated span subjected to a concentrated load of 10 KN distributed over 20×20 cm² in its center (forces in the center of the elements). The representation below of the curve of moments on a section in the middle of the slab allows to understand these differences. 1. **Node efforts** Below is the curve of Myy moments calculated by smoothing on the nodes. ![](https://lh4.googleusercontent.com/gNxcMNw9Uv6qkkD2PWfNauG-jQmfwejpUQ9TcCXKlmJpvqs4hNQ0EHYP4ok_RheG9mZYhwHKsWvFROKb48i7FZfL6kLahRqpZAa_gZvEv_pkDxgx0N6KlbG05UC3b5BUUCQX7JFC9EVWz5XAIYJHhA) The forces are calculated in the integration points of the elements and then extrapolated to the nodes. The maximum moment is 2.96 KN.m in the center of the slab according to the manual calculation. 2. **Unsmoothed efforts on the elements** ![](https://lh3.googleusercontent.com/YwA-HPbnQTmgROpUazC7uGyEgt7DHH9vPQbec5GlZAvKmM57sM617wIKTWRFFyXFh5Cqmceqw2xU_2PagyDZ_6qzSZwowzYuzIytBURpfUeTJec982m2Ye7T7BrkK9NRrzQtfHp7lAmwSWOW-hax3g) The forces are calculated in the integration points and then averaged to obtain the force at the center of the element. The maximum value is 1.92 kN.m , average of the central elements. We do not find here the manually calculated value of 3.0 kN.m, but a "smoothed" value on the elements surrounding the peak. From this example, we will note that the forces at the nodes give results that are consistent with those calculated manually, which is not the case for the forces calculated at the center of the elements. 3. **Smoothed efforts on the elements** ![](https://lh4.googleusercontent.com/hNry23k32MGnFsiOQPLnTU1l9mIWYpZxjMKQeOHRNJixhBDXNpJttoIJGtmjd7wrgbv_zU1BiHHTWkIONKg0RELhYxOBd0r0U15DkjfcGXZIeIFb0oFgrYLlebeGhoeqoUXuLHI1trSoT108R4tjrw) The forces are calculated in the center of the elements and then smoothed between them. This curve gives the impression of a curve which is extrapolated on the nodes, whereas the extrapolations are carried out only on the results at the centers of the elements, the resulting curve is without physical meaning and therefore "false". On the other hand, in another case, this option of smoothing the efforts at the center could be useful if we want to know the efforts in the plane of the walls. ![](https://lh5.googleusercontent.com/3c9p2_RvnLZWuyBOmrUMetSxiFWmst6bPWJAJE3whzXuDAusnNsWNx6HBfHlLljOMcHievq67lnSou3ymGaHsZvieTe8Md6-b3xXkrey7-SoFbMdaaA_-5Bd3-oQ5_OewWQJlaJJ6eTQB_quHzcpgw) To be valid, the width of the mesh should be equal to the thickness of the wall.The visualizations of the finite element results at the peaks give very different results depending on the options chosen by the engineer. These results cannot be taken as they are, but must be analyzed and interpreted by the engineer.
--- The figure below shows the values obtained with a point force of 10 kN at the center of the slab. The moment value increases to 5.2 kN.m and the pace of the moment curve shows a clear peak. ![](https://lh4.googleusercontent.com/qLXbqEQOgubvdxKCzaBweCitrkn1dyP75r7FO_jnuJ8x6Y3i7jLrSXmfSnrtto154WsHEZumLNxrNH2n5pp7IYOvFyseauVOjp0RUB7H60Tni_jDMXMT3Ln6mFqX2w_oTLeAhjC0GzZo6Kkp_Gsm2Q) Later in this chapter, we will see that point forces (which have no physical meaning) lead to effort peaks and that it is better to avoid using them in order to obtain accurate local results. --- **D.5.2 Peak analysis method** The reinforcement specifications often show peaks of steel which have very important consequences in the dimensioning of the reinforcement. The user is often unaware of these peaks: should they be taken into account by considering that they are structural, or should they be ignored by assimilating them to numerical calculation problems? ![](https://lh6.googleusercontent.com/aSH39orZmu6Q5YAjF29z4GjLV74WAkauIEj9z10I2FdqiiZlsVvzH8FxXKKVGrHo75qD8O1GGtKkqcCy0z5TMkEce8Il38qgyDVh8tzo2r6dwM-kQJczeDDCfWEMcMivs1grnciocnxSeJJjmX5FZQ) *Example: the peaks shown above at the fixed end of this cantilever beam are of course structural.* The answer to this problem lies in understanding the functioning of the structure and the path of forces at the peak level, an analysis that is indispensable to solve peaks (limit the maximum demandclipping, linearization of reinforcement). This can be difficult in the case of complex models, but is always essential. Three types of analyses are possible:**Analyses** | **Objective** |
1: Geometrical analysis | Identifying the singularities of the modeling at the peak to determine its geometric origin. |
2: Steel sections analysis Axi, Axs, Ayi, Ays | Making a first distinction between membrane, shear and bending forces |
3: Analysis of the efforts generating the peak | Detecting the "faulty" component(s) and quantifying efforts |
Tip: Avoid modeling distributed forces by a point resultant for the calculation of forces in slabs or one-way joist slab!
**Make sure that the mesh size is in correct proportions with both the thickness of the plate and the impact area of the smallest load.** In addition, to illustrate the different results that can be obtained for an extremely simple case, the Working Group calculated the forces generated by a Br wheel of installment 62 Title II, using several software programs and several smoothing approaches. The study is available in part 3 or directly below: example of modeling a Br wheel. --- **Punching** It has already been evoked, several times, the fact that finite elements did not deal with certain subjects such as the shifting of moment curves, the limiting of maximum demandclipping of shear forces close to the supports or the punching checks. Except in special cases, therefore, the checks related to punching still have to be done manually. We will illustrate this on the example of the load on the one-way joist slab bridge shown above. The modeler might be tempted to reason about the shear stresses averaged over the punched surface from the FE calculation. We refer to the Limit state design (LSD), also known as Load And Resistance Factor Design (LRFD), which has the advantage of being simple. The comparison stress is simply the load divided by the perimeter of the impact which is diffused at the average layer and by the thickness of the slab. Let τ=100 kN/(4\*0.25 m)/0.25 m=400 kPa (the slab is 25 cm thick). The FE calculation, on the other hand, results in smoothed stresses (here in the most unfavorable zone, not strictly on the load diffusion perimeter!) of the order of: - τ=5.33 kN (integral over 0.125 m, read below)/0.125 m/0.25 m= 171 KPa; - τ=5.42 kN (integral over 0.125 m, read below)/0.125 m/0.25 m= 173 KPa. We are far from the 400 KPa that the regulatory approach to the BAEL gives - taking into account FE values would not be safe. But these are two different approaches: shear in the slab is used to calculate the shear reinforcement and punching is another type of verification. ![](https://lh6.googleusercontent.com/VwIvM8sN5d2WyDunBA9CWlmxmI8ZGAglyoBhB_XDSpXInGIkuQqrzAvdChCy7j2AanmxOe8KtGPeK7DNpJYo8MGZIcGdeuFjOhVaHxF6rxGaPD0mLsm68V2ClCS8U9GLkfUdb-9XrE9AxGTindPd9A) ![](https://lh3.googleusercontent.com/RhZlRf0MqBUddLtzaqAnljJyho7nY28uBYfwI_-BUaCb62RIMCkIwDaa8WFN9DkTP_RTIAS2mSdo3zUE5amtaasJxsCd7KJR4qhquTmijMfaKFqDivNgHZwC2Q5oydBcRcQBwWMx107FDpsY0l6NsQ)For the calculation of reinforced concrete structures, it should be noted that the peaks are caused by point forces or supports.
--- **3. Peaks caused by mesh size problems** The geometrical marking of the peak often makes it possible to detect the causes. **Example of an inconsistency of results related to modeling**: a graphical construction can make us think that an edge is common to two shells, whereas in reality there is an extremely small shift that leads to aberrant results. To illustrate this case, we extend the slab of an example above by another rectangular element that we consider to be strictly in the same plane as the previous one. The results should alert us that some peaks appear: ![](https://lh5.googleusercontent.com/kElPJIPkw6RYBAjoTEi_n1zqwmOA0IelLoM2vCVJ8KzLxL14739BeKXWsHzu22_loq3_SbBMjM6Vh02Noe14Fg3t58fBKshPDrWDKJgs1LxU22CuA-dhgnda6fpDVu9oZo3mVH3qaAZtgZHaLTQ4gQ) By zooming, we can see, on the right side, that the connection is only made on a few points (corresponding to a geometrical tolerance of the software) while on the left side there a very small shift (and which is caused in this case!) but which prevents the connection. You can see in the figure below that not all the nodes on the common edge are connected: this should alert us. ![](https://lh5.googleusercontent.com/dlnoSalhENK3CFOLjq1u45Sp2LXBExDU3nFl5oBaJrKJSVr7yv7bGx7sxReFoaEdkauUJxGG0TxviO3hBIoBUYu1BqIH-qVyBxuvZ0QnvmsqVSYaN3OpserObDcQQkAW4IvwiAyXhaF02_hVnls3TQ) ![](https://lh3.googleusercontent.com/UweGomDMCEHAV8Ed9Jv0BYMH1obpSHYjYoNv5dRW8r_-uQ_gFC3KIgIDsqYJ0eRY92KQeLucEDaRN5gArgJdeJFEE4nJtNJxuEYFt5e_yFY87y2bWjdaE93etUxlUAN4hhXTQ9u4yUnx_0hAZijzEg) The observation of the deformation should also alert us:![](https://lh4.googleusercontent.com/LCU_CAnrai7uRwGPLLWR6gnt5ZyZM_r3MnfIvCZ14xdVTM7mVbmYvKflzn-slCSmhHc2hF7aE8uKe7cxAuX9yuduHypEjgJnsTAIjhLJhzcivCKa5GsQHt49hpNMbKDevsiTIrFM5eK67WtfPmiDew) In case of difficulties, the user can himself or herself create beforehand the nodes of the joined edge, if necessary with bar elements that will be deleted once the mesh is reliable and fixed. Although this approach may seem tedious at first glance, the time saved can be well worth it. We must remain cautious about the use of automatic corrections proposed by some software (in this case the linking of nodes through kinematic links) which can lead to local stress peaks. In this case, it is better to erase some shells and start again some parts of the model. See also § C.3.7. **D.5.2.2 Second Analysis: Study of steel sections perpendicular to the peak.** To help us locate the origin of the peak, we can analyze the steels details on each face, in both reinforcement directions. Indeed, the analysis of the steel sections of Axi, Axs, Ayi and Ays perpendicular to the peak quickly provides important information: - high NXX and NYY membrane stresses are detected by large and equal steel sections on both sides. If all 4 steel sections are equal, the element works in shear in the NXY plane; - high bending moments MXX and MYY can be detected by important steel sections on one fiber and very weak ones on the other one. To illustrate this, the table below summarizes the consequences on the reinforcement of each stress component: ![](https://lh5.googleusercontent.com/D5IAoPvGg4d5DvAt1ID_6pSzN57DKOvgLRTiItNVx8B683W2yTm929h-OZI3mWwG1-IfI5TU2JoX0u46CbhQvNRr8MwEgWcyxNwWU_ATZ6IQmiMwdS7xExb1l50tvac7nrM8XPdXgcTSYG6vOlG3mg) The code X indicates an important value of the steel section, the code 0 a low value. From there, the analysis described below is carried out. **D.5.2.3 Third Analysis: Effort analysis perpendicular to the peak** If the two previous analyses are not enough to explain the peak, it is then necessary to study the effort components in detail to determine their intensities and identify cases of dimensional loads. This analysis, which is often long and delicate in the case of complex modeling, can be greatly simplified for simple modeling by carrying out effort mapping or local cuts. **D.5.3 Peak Resolution: determination of final reinforcement** After having understood the functioning of the structure and mastered the effort paths, the engineer has all the elements to solve the peak and deduce the strictly necessary reinforcement. **D.5.3.1 Cases where maximum limitingclipping or smoothing are not possible** In some cases, the study of the effort path shows that the peaks are real and cannot be limitedclipped. This is the case of lintels which show very important peaks at their ends, which is logical because they are fixed end beams that must be calculated according to the mechanics of materials rules and reinforced concrete (fixed end beam subjected to constant shear). **D.5.3.2 Limiting Clipping moments on supports** Article 9.5.3.2.2 of EC2-1 allows to limitingclipping of the moments in the plane of the supports (walls). 1. **Beam resting on a column - example 1** Consider the example of a slab with 2 spans of 6 m which are uniformly loaded by 25 kN/m². ![](https://lh4.googleusercontent.com/6R7JxLIYKf8rfOgITXMOSimoImghxMwpwdicF1okx8MUudve6zNIlYws260uE6Cc06S6Rpx0kZaxY1VpUah_HIpuDsiDVaravInK2-3xfVA-Hu_XdzhlMXagRsSe5_PI2GU2T22wdtd-1W9CbvfIyA) Theoretical moments are -11.2 kN.m on supports and 6.3 kN.m in span. ![](https://lh5.googleusercontent.com/ncT7yHOypy-6xZafiLVQTjHfDqyi5CprNC3DzHg8-1wTNvounYPHXAQB6QTlqjuECl0bB9WoR0PfdZj64pTZ3fEmHBObds6ZXDV5nZVxiWLC8IaUE6ERInp9OSteS06LVUCFMwJcAQ5qnhAS8LFjDw) The FE software shows a peak of -12.1 kN.m on the support, which is real. Limiting Clipping at the plane of the wall: To obtain the moment at the plane of the wall (thickness = 20 cm), the user has several solutions: - either making cuts at the support level; - or not visualizing the support area (but this requires an adaptation of the mesh); ![](https://lh6.googleusercontent.com/rY6ATq1z7n7sOGKJsYvfRs2x4xgpJ1taxV4MPgXbUQHxti28l9dAF46FKI-K6lgVbeDKH5wcAbdah1n0vgO-UrM0QfVFtzIyjFzqtf7c6mlbVvDjwxdWdGGpBmNSwk_EloI228uxas1hvpzxRkDPDg) Moment Clipping at the plane of the supports = -10.6 kN.m - or adapting the mesh in order to make the width of the supported mesh equal to the thickness of the wall, as shown below. The moment in the center of the mesh will then represent the moment at the plane of the support. ![](https://lh4.googleusercontent.com/-SPj0LbhqA6t5VO8FNgM8hjHslcgyA3ojjm8O805pDagmFAJ3exDUsbVjXPfct17a8naIBVaOzsjE20iyjSycnSYyy0LEThswuNmI3P9qdkHdnoBj9_i39E_MyFmS5p8k3MNdd7DzipfzW-XQBdQlw) The same type of reflection and approach is to be carried out in order to reduce the transverse shear effort, if necessary. 2. **Beam resting on a column - example 2** The example below shows two ways of modeling a simple column-beam structure to highlight the effects of the real dimensions of the structures. The principle is as follows, for an out-of-plane width of 1 m: ![](https://lh3.googleusercontent.com/waHlOG8VagKczCuTzlqowafcSTaubuBMgv3ekalreGzWBzzD-lGm2rmF1q3y07JgE-W0wpHlyLPJ76I4wn6a2DEHSiV1QeLpAYIwpzfr31Y_CKw67jaKLrDrFVwXpWediGbCGLwp0fPe9JG8FD5uzg) Firstly, a wireframe model is used to calculate the moments at the central support (truncated view): ![](https://lh5.googleusercontent.com/1KH-FA2Ikul6ICgPNTiYW_nXRl_Gfk4QgnV1fBnLEvWyobERDuSKQcLY7g5RK76TOsI1uyHOjJkjBKj8AbxW5mmcHIBjhUiXbqhsIhsIQ6j2yttmlmspGifZ1HN3NWTojJdfWYhmeokGjCUS6NXlEA) The moment on the central support is 82.09 kN.m, giving an extreme upper and lower fiber stress of 6M/(bh²)=(6\*82.09)/(1.0\*0.5²) = 1970 kPa = 1.97 MPa. The stress in the plane is (6\*70.00)/(1.0\*0.5²) = 1680 kPa = 1.68 MPa. Below is the result (in stresses) of the same calculation performed on a model with plates, locked in out-of-plane displacement. This model allows to represent the behavior in section, with the real thickness of the elements. (truncated view). ![](https://lh6.googleusercontent.com/lqw1JviNTDzL3RK6YAi0MMkc2vwqdrgD4ZfMrORowqd9c3jDhkXBtqmOEIA6BP1nIcQaQ1lTIZYLHaxBOseEjY7LyZgvhc1Iy2cIV6bHxTHtI1jSPKjJKtR0QlzRRewhsAxhNN5mLh8FoPngYpXWiQ) The stress obtained in the upper fiber is 1.58 MPa. (The lower fiber stress is not representative because it is calculated in a singular area that constitutes the right angle). This model highlights the legitimacy of limiting clipping in practice. **D.5.4 Reinforcement smoothing** The following method, derived from a common practice in the field of **nuclear civil engineering**, provides simple rules for smoothing the reinforcement. Its application is nevertheless subject to the engineer's judgment. In particular, in the case of floors of ordinary buildings or bridge slabs, these values are probably too favorable and it seems possible to reduce the size of the smoothing to half of the values below, therefore limiting this size to 2h (h being the thickness of the slab). In this context, the smoothing of the longitudinal and shear reinforcement sections must be carried out: - between adjacent elements (and not successive in relation to the reinforcement direction); the smoothing is done perpendicularly to the reinforcement direction; - over a reasonable distance (engineer's judgement) and less than a value that is correlated to the plate thickness and the plate span. The current common practice is to average the results of three elements: the element for which the maximum is observed and the two adjacent elements, limiting the width over which redistribution takes place to 4 times the slab thickness (see table below). E.g.: if the size of the elements is 1 m, averaging over three elements is the same as averaging over a width of 3 m. For a 0.5 m slab, this width is limited to 4 times the thickness of the slab (2m) which leads to averaging over only two elements. The distribution width should also be limited according to the slab span or the wall height, because the smaller the span (or the height), the smaller the distribution width should be. **Proposed rules for smoothing the longitudinal reinforcement peaks of slabs (resulting from N, M forces)** They are presented in the following table. They are valid for a slab subjected essentially to membrane forces and bending moments due to out-of-plane distributed loads, and with a sufficiently fine mesh size that has: - an odd number of elements in both span directions; - at least 5 elements according to the small span (7 elements if possible); - a mesh size equal to the thickness of the loadbearing elements.**Width over which longitudinal and transverse reinforcement sections can be smoothened** | **Limitation of the distribution width as a function of the plate thickness h** | **Limitation of the distribution width according to the plate span L** |
Zone where efforts can be redistributed in both directions | 4h | 0.5L |
Zone where the redistribution of efforts can only be done in one direction (at the edge of the shaft) | 2h | 0.25L |
**Width over which longitudinal and transverse reinforcement sections can be smoothened** | **Limitation of the distribution width according to the plate thickness h** | **Limitation of the distribution width according to the plate span L** |
Effort can only be redistributed in one direction (at the shaft edge). | 2 h | 0.25 L |
**Numerical application**: Illustration of chapter D.6 - Peaks in angles, mesh incidence and fillet incidence. [Link to the file](https://cloud.afgc.asso.fr/s/Ta7XtSjMZEFCbMm).
![](https://lh5.googleusercontent.com/wb_JyckwtvqW4qxCEfyy16hkFfKtJIHcNoeoiWnuoUXgOjLC3kQCmL8SXnzpc1Jbx0IoZrHjtsIniHmQWTvFFMLEKrOeyc5dyvCAw4IggyqyI1GHTNm4eEnNSJ_yUvh3_c6uyHyGnpsY) --- ##### **Illustration of Chapter D.6 - Peaks in angles, mesh incidence and fillet incidence.** *Authors: D. Guth (Arcadis) - P. Mangin (CTICM) - v0 – Jun 25th ,2020* 1. **Input data** The modeled structure is a simple flat angle bracket made of 10 mm thick steel (dimensions in m on the view): ![](https://lh4.googleusercontent.com/BPtXZGVY-JUosziv8x3OlvVdhZp_IN3aWCicMF2INXNqAnx8KGyXZL70TB9qVkr-hNxIf_YtzLNVs9veRI_g3pckrJsiFflT8wsQ97pPK8a93uRgJcvCNDAxdI4crGoFUAr96jgnrDbZ) We apply a load of 100 kN/m to the upper horizontal edge. We do not take into account warping phenomena - this is a "simple" mechanics of materials model. We start with a mesh size of 10 x 10 mm² and refine the mesh in the peak areas, as shown in D.6. - "If the stress peaks are due to singularities (reflex angle, interface between two different materials, point forces), they can be neglected ... if the state of stress near the singularity is not part of the objectives of the FE study. Otherwise, it is necessary to improve the modeling (replace the reflex angle by a connecting fillet, replace the zone of discontinuity between behavior laws of different materials by a transition zone in which the parameters vary continuously, replace a point force by a contact pressure on a non-zero surface). - If these stress peaks appear in areas outside the proximity of a singularity, we should successively refine the mesh of these areas to know the most realistic level of stress.” 2. **Results** We will also find that the more refined the mesh is, the more the extreme stress will increase. **2.1) Calculation without fillets (right angle) - successive mesh refinements** Mesh =10x10 mm² to start - each successive view represents a x2 mesh refinement, at the angle where the peak appears. ![](https://lh5.googleusercontent.com/1xnhWOU4XT4cjvGTLeHe6PkCV5Ry9blrVoKOVbmRockrWF9Y39K21DipNjFq0QW-Mch_iOj1--X_PSzYmMrjJW8M7Z6zvQEoIzKjYLvbj7010dEo2pR6maUVcFRtsCb2Wea7qHZUkf_W) Zoom - Von Mises stress in the angle: ![](https://lh4.googleusercontent.com/CAzrAGW-h-7vAu6Ji1-uhvZ1GfalbwVKgDC_iV1ONXkzPm0rBkbbGU0HJgDxMt_XFetfV7hWbtfqCtRHO9l1BPbTgsqWULA04YDk-rGZuY4FxZXPDDjDypnkcQM3zDgc82pOfk4mY2vu) Refinement x2: ![](https://lh3.googleusercontent.com/z6XXXfCNCKkARhrvdFrCYlRZ1AToL4GMNmdmIoGihR0gP-YCUj4bq751-h5VJZlLkI0MBZDqdl6rCrQ3UuA_30-27uiixeNqdKX10Xy28Yrp3ptOKMUaHvgLFUgQju9-FyTqEmTvPH2U) Refinement x2: ![](https://lh6.googleusercontent.com/gRbkojtIvazylgK1VxX3Zrqcc-Ez_64T7ncacXJZIl1KFA559IcccgCpZJtqXe1OfHu5dWXyuQ28FX_PC_7lff_2tksijaXnrH8w266kqFX3NvNzefhZZAgwSIPDXjSzszWs7Pta19YC) Refinement x2: ![](https://lh6.googleusercontent.com/2Gkua3I9v11y3GJEW-kJPiMACryhgMCQ-50CZ-yUdBKmzjgM-ufaDY-loS4zGV51Ez0hqQO5Q-_u3O3xiCqKIZ3oYHidBBwjLQGnt1QuT2tsgOx4dP5UMK6fowo_xa7FP89Jqyj6Nu8E) ![](https://lh4.googleusercontent.com/JMty7duK8wiMdQZly0Ypy2fM3Z9YR_j17a11p63yO3fijOpH0pvSSI2cenPGg5OAVUTgRqXQpS1Mm_d4RAY-CxECUKWcIwPsc0rUUzSNOK6Ynk-Ps3-H5s2CZt0-RqePk8H8eM2B9buw) Refinement x2: ![](https://lh4.googleusercontent.com/cerQYXV64ppgbD8SvwDxPUSV_ewJE5zGgdIxe4AKlth3ES26V8ZTUG3cnm4KKURX_rh06osbbHojPcRoiD8Qy-0VOlXkqCgm19KLWOpnjFOf7rArEoQdqZyObe8C9keMTiTWvuBHnH_e) Let us set an arbitrary elastic limit of the material at 460 MPa: we present below the extent of the zone having a stress above this elastic limit - about 10 mm long ![](https://lh4.googleusercontent.com/xRt7pzNRrVysL1qiDvKWr-L-DIzloXvPOZWe11Br6C2Ix9fhKPrx2Pvdgji4g2kk4hd38AeC_yyJTaOWnZZNfKlzgz13AEuBaOSCnu9mPxEvMauCabMMMRBnPe1EVj3BSiViYjDcLyPY) The curve below gives the evolution of the stress peak according to the mesh thinness. ![](https://lh4.googleusercontent.com/BifKEj9EwssJ7f940-bMEzFpRVeE7M9KoBcF9XCyKkU3w8VvoJRbFNFzI5ggN7twJuJOuf91Ob5uAkWFlyctMNRTdwnbDxQjEDoR3Lur5r5OFW9MVcOrTr-YBX_IP_PSD3pn4s03S6b4) This curve reflects the fact that at a singularity, the stress peaks will increase singularly (literally)with the mesh thinness. If this zone is of no interest with respect to the study's objectives, we admit the presence of a stress peak at the singularity. It should be noted that if this zone is not of interest, it is not necessary to refine the mesh of this zone. Nevertheless, it is always disturbing to display iso-stress with a stress peak at 753 MPa. If the recipients of the calculation note have some experience, they will admit this singularity. Some may ask for an elasto-plastic calculation, if the value of the stress peak is too excessive (of the order of 2x the elastic limit of the material). For information, for an S460 steel, an elastic stress peak at 750 MPa should not produce excessive plastic deformation (we would remain below 5%, the limit value recommended by Eurocode EN 1993-1-5). If this area is relevant to the objectives, it is necessary to model the connecting fillet. **2.2) Fillets Implementation r=50 mm** The Wiki indicates that the minimum fillet must have a radius greater than or equal to 2 times the thickness of the part - here r=50 mm> 2x10 mm - ok. Note. - The fillet consists of a succession of straight segments. - The mesh at both ends of the fillet shows FE that do not have an optimal aspect ratio, due to the connection angle that tends towards 0. Base mesh 10x10 mm²: ![](https://lh4.googleusercontent.com/iPzQvxQJMwm2-PnE9sNm9qLPeEW7Moc1xJ4OWOps4Df02etr1U9QCd9wYthJYomL9WIH_X14MIzkP1GzGmzDBpXIIIGCrXw2Czxkr8SfgjBdQkEEQjG7dVyXfmdocijYTSO-XfF1Rvwv) Refinement x2: ![](https://lh4.googleusercontent.com/9_bvsEe_piGqTuDUYR7Tz3MjfQieGxFSl1MNVk_NZAb3QBp9aQ0DOs7CA4HCIsXF1RItY1eu4wu1HTN3p2bTfEw6yzAgP9wA0O5mxUBiHMYaQOhg69Krd0qtfZ1iMqY3irbWTFBMYHGl) Refinement x2: ![](https://lh3.googleusercontent.com/S1nl1eKvumsYwZheXAUXhqJ33DfeL8ngCIyo2XxUG0MJAQ-3BtFNA40O_QKYhdJPxkqvINc_kpbWLOrA6jWJepKmQ7e_HGGss_551OwCQQUZGNi9RL6-5tHNuUBD7okW2gkU8SyCfS1m) It can be seen that the increase rate of the peak value is lower at each refinement than in the previous paragraph. Arbitrary filtering at 460 MPa does not show an overflow area: ![](https://lh4.googleusercontent.com/cO205bxDx0wMw0USA5HCMTzVA-Szrv0wl7JkpCCCTUZwCbxtWzhjkI4i1UcPXw1VvVo16z5YiRU4uIrrNla6CGmH_BTUnbKlwzOiS3LAxmXUScUxQ22h8-Hw_ScB4KLixzV1TGRCJFUq) Let us assume that we have an elastic limit at 440 MPa, filtering at 440 MPa: ![](https://lh5.googleusercontent.com/6eFJyqYZVhOhnEiYnqIVF14kHiCidnyPm3VPLwQlTcJw1Nhw6Yygt_Ou3aIYSaoccZLkOhAXIM27M4n1Xd1jbkezunM0BA7UEGOsCtS5IS_KlhBYSQ_T7shCjD4i5Zsn0l4LRVwRnx_M) ![](https://lh5.googleusercontent.com/E8_nV9877bs-ixH94rzu01k1sFfp654UUu6P9zrEUiqLaN20q627i2x-VsZiME-Gs5UMY5FSo5YdyRBsOwqPd3_rDw1FVrBDohGrUkiJDRD5nvdIIrfDx5D6EoZ40tOPewIBn-NXdAGT) (dimensions in mm) If the material’s elastic limit is 440 MPa, a stress peak at 459 MPa is perfectly acceptable for an SLS analysis (for a Fatigue analysis this would not be the case but this is another approach). At this stage, there is no need to further refine the mesh. We can see that the value of the peak stress tends towards a realistic value. ![](https://lh6.googleusercontent.com/2zoIS-0fmKgmnX1fQkMHpXOm9-RTVKBpS2gBkHBZPk7B24aQz55zAMqDqC_ecSTQyjBdRKYMPl6FwBidAXVH5sas0vIsWr5T8PzK_Bt2JycJ8jybvFVny4iTd8vli99nM4UFPqQU23b5) 3. **Results** The curve below gives the evolution of the stress peak as a function of the mesh thinness and according to whether or not the connecting fillet is taken into account in the modeling. ![](https://lh5.googleusercontent.com/ag709OpzQA5AuPUibYWHR9lWpxJMPiQuTfgsIAOtoriZ2rBAmZssH8dVvJh0smpWizsXXJC0aLLRKI-cE95gu4U-ByPIb2P9evcLamkvti68BOe9RkO-e0PfOmvmAVd_fHnkiC61dmEN) # D7. Further information specific to dynamic calculations #### **D7. Further information specific to dynamic calculations** **D.7.1 Total mass verification** In the case of dynamic studies, one of the fundamental parameters is the mass of the structure which is used to determine its eigenfrequencies. It is therefore very important to make sure that the entire mass of the structure is actually entered into the model. Indeed, in the case of using a model that has already been used for static calculations, it may happen that some permanent or variable loads, such as equipment, have been entered as loads (point loads, linear loads, surface loads, etc.) and not as a mass. Therefore, it can happen that the software doesn’t consider these loads as masses but only as overloads, and does not take them into account in its mass calculation. This may result in a reduction of the seismic forces. It is therefore always necessary to make sure that the total mass of the structure is indeed the desired one. This information is generally available in the results of modal analysis or, even better, can be obtained by performing three static calculations, by applying a unit acceleration field in the 3 directions (X,Y,Z): only the elements with mass will therefore be taken into account, and the sum of the reactions will therefore make it possible to know the mass actually taken into account in the model, in each direction. **D.7.2 Verification of the participating masses** It should be verified that the modal analysis carried out takes into account enough eigenmodes. For this, it must be verified that the participating modal masses in the studied direction and cumulated for the different calculated modes, represent at least 90% of the total mass that can be set in motion, calculated from the unit cases of acceleration, otherwise the standards authorize the taking into account of a pseudo mode (per direction).Trap: Some software indicates cumulative modal mass % which may be based on a wrong hypothesis of mobilized total mass: in fact, the parts of masses blocked in movement by supports will not be counted by the software, which will therefore overestimate the mobilized modal mass %. A trick to overcome this is to define elastic supports with high stiffness rather than fixed supports: the total mass will then be exact.
In general, it is preferable not to model mass associated with fixed supports. --- **Example of the study of a skewer model with 5 degrees of freedom:** ![](https://lh6.googleusercontent.com/XXM9utkjuTM-DVlZHEt3Lzn21WSlMPYFklbhbZopvo2pRJWMcvy41cIzy--jrAuylUE5ZkGthU6szZ1I8fbJPPIeFwXQuM6GfM6SlHSUiNypDHd_j9GGHHsZ81RwPSPUhB9w_GaeJ5aO5Ox2tpnl7w) Three cases are studied: - Case 1: Similar masses and stiffnesses at all levels; - Case 2: Case 1 but with a stiffness 100 times higher in the height of the first floor; - Case 3: Case 1 but with a stiffness 100 times higher in the height of the first 2 floors. ![](https://lh4.googleusercontent.com/mF2fwV98XyiaXh5X-rEfsyr-TEdfkfuXVdyXZaQNKuGeOMbNUULkRccuwyv9EZ9hIDYJGBcZUJWgxjpEdv7bTE07MsKjpi1STL7gu9JpThbp4jopp5GuA6VfUGPXw65SfnzhZ-URsikm_C3KOZU2xw) Assuming that all periods correspond to the spectrum plateau (identical spectral value for all periods):**Case 1** | **Case 2** | **Case 3** | |
Mode number | Base effort | Base effort | Base effort |
Difference if we choose 1 mode instead of 5 | 99.5 % V | 96.0 % V | 83.2 % V |
Trap: Symmetrical and anti-symmetrical modes.
**Example of beam vibration** Depending on the type of calculation being carried out, modes that do not provide a % modal mass supplement in a given direction should not necessarily be considered irrelevant. Simple case of the beam on two supports - the masses are mobilized only vertically. The table of modal results shows that all even modes do not add any additional % modal mass. ![](https://lh3.googleusercontent.com/NyaIhhPfnl1AsVAGNARJu6PMWRhGk2tNKPc16AVfYGRbbgYkagRHyCuMCmMCCS76DOZCOGl0UtxaBLyKzD2OOnhMKjrn13UMqyGMBYiKBrjJBSKD0ltROQYWLL5QQzQux3LdQHInwyVQ_D5mmgXFzA) Looking at the modal deformations, we realize that these are modes with anti-symmetric deformations: *![](https://lh5.googleusercontent.com/S225IW4NQmyrxoCT5fF3KOqnlu2HP2XPCLqcyf00Uw_gkp-VKmNvSyMa4128wJEgyPPdEfyKXfRfEIS0i2v_OxCssSZFG805piUBsvhNfPoqOyLpLJJuB2Bogp64iW_pyyE50sPYF3USKFOLMb8mNw)* *Modal deformation - mode 1* *![](https://lh5.googleusercontent.com/SNVmscLEDmNTnQK9nKxJtXuudo-2iJL3sbdlJr2RMrLZQJNds_tKwChCDRZP50hbQZ616dAf00_zPHIvFIE6VES3aRbkkzUsziUSmJzF2tJfxlJWILXnKg8hcVHk9KGkk82-2yZG5DaJhELA0NQhtg)* *Modal deformation - mode 2* In the case of a spectral seismic calculation, these modes do not actually add anything new, whereas in the case of a beam or bridge vibration calculation, these modes have all their interest. It is indeed admitted that pedestrians, in their movements, can have actions in opposition and in the direction of the modal deformation. A harmonic calculation is indeed carried out from the loads positioned as below: ![](https://lh4.googleusercontent.com/7-B6h0xVryRO0PF29TAmlnkO1fPR_GhHIQIdJK0EsTi1oNt0peA9yewF6HuquNFDIBrwxQcvJ9bwtEhvoNBiXJ7b2e4qJ7CY7EH2rJDfaWnQ_RfR1H0E8m9AgnNlJW5RWaxZT_EDWUDI6_FPG8AR8A) We will usefully refer to the SETRA (operating society for transport and automobile repairs)/CEREMA (center for studies and expertise on risks, environment, mobility and development) guide on pedestrian footbridges for more information. Spectral analysis: finally, we give below the forces at the middle node of this beam, calculated by a spectral seismic analysis - it can be seen that even modes do not actually make any contribution. ![](https://lh3.googleusercontent.com/5PvBkVTXfXgw63LQ3TwztFKCBdXJjntORdpm7XuH83W_iRlko_vEYDqO22FZW8sxS1zAlrqdVhRUMLxW5s5dSZKXq0NA2TdEPHphhdxZF6il-l1j5ZVgyaVAuT4P9GJ7cjfUrv75T3y0OUQUmmeP9g) ---Trap: Torsional modes
**Example of a building in torsion** Generally, common buildings have a torsional mode. On the example below, we can observe: - The 1st mode: with a preponderant mode according to UY (longitudinal), ![](https://lh3.googleusercontent.com/FkKEV_QzpPcw5rDu0lMAZA-GLDXLMIY2yAvdda3_N9nobZAVW5LpifmCQ7k4cidIOOdlaVr1c1rBu9dbvbY9JUVEF2NfiYkjykMgjpr7JOWRtSU2uxGnN0ROr4gfFD2r54pu70IAwfpeD1WiYsczZQ) - The 2nd mode: with a preponderant mode according to UX (transverse), ![](https://lh6.googleusercontent.com/GA0_VfVA-d6uPbc3lErMdTiBSXH28tzHzXIup2OFwgp8pmU6Vcm9_tsbghCVgAR0pNVi5CHw2Mv-ig-OfxVR2UEiRoFFos8Ahip2Zc-gkdOPDN5pvS90kispHKOjf27t30oXjmaHyCWHSFjwFhVSBw) - The 3rd mode: with little modal participation while it significantly affects the structure. It is a torsional mode. ![](https://lh6.googleusercontent.com/zRf9I7r8aPDNWARcOh3u_Sm617oIiatpraoIZTN9ny8sRGk3ooHD7TW07XCimT_8JiW-a3TsUDWR1bMe4-HOdnxMKXJOIRBuOhDxhpbPv8P1s9uOV11OSMbs9TXfnMYwH-i0ynjgVpKQ-04pi23Trg)**Modes** | **Modal deformation** | **Modal mass following UX (%)** | **Modal mass following UY (%)** |
1 | Following UY | 0 | 77.36 |
2 | Following UX | 74.11 | 0 |
3 | Torsion | 0.45 | 0 |
Beware of graphic amplification factors, which can be misleading on local displacements (impose a factor of 1 to verify possible inconsistencies).
In linear elasticity, the displacement rough estimates must be satisfactory. Their amplitude must be small in relation to the dimensions of the structure. *b) Vertical loads calculation* Static equilibrium must be verified. The results of the loads applied in the model can be calculated manually and compared with the components of the sum of the support reactions displayed by the software. The distribution and direction of the reactions on the different supports must be analyzed in relation to the blocked degrees of freedom. The presence of a null reaction for a blocked degree of freedom must be analyzed. This will generally be a symmetry effect. **E.2.3 Tests on connections and assemblies** *a) Null or non-zero support reactions* The support reactions must correspond to the static diagram. The sign must also be verified and allows the detection of referential errors for load cases. *b) Modeling an assembly* The general calculation does not eliminate the need for a local (and manual) analysis, for example with a load close to an assembly to verify that the force transfers are made in the expected way. **E.2.4 Sensitivity tests on specific modeling points** We must question when modeling produces an effect (global or local) that varies a lot as input data changes. This would be a case of model instability. # E3. Traceability and group work #### **E3. Traceability and group work** While there are projects where a single engineer will do all the calculations, from start to finish and at all phases, most of the time the work is divided among several people. This requires the implementation of a particular methodology, described below. And even when the engineer is alone, these elements are part of the global quality approach and allow to remember the work done. **E.3.1 Transmission / traceability / archiving** For the project success, it is essential that any model can be passed on to another person with the skills required to operate it without wasting time trying to understand what has been carried out. To allow the transmission of the FE model, and without redefining the classic notions of quality (files storage in a well-defined folder, explicit filename in relation to the valid version of the model), it is necessary to trace precisely what has been modeled (in a modeling note if possible, but failing that in a simplified text that can easily be found), which will list at least the following data: - the software used; - the type of elements used; - the material properties considered; - the support modeling principle; - the representation by sketch of the main principles of geometric modeling (in particular simplifications made); - the principle for numbering nodes and elements; - applied loads; - the calculations performed; - the combinations made. If the models are modified as the projects progress, it is necessary to make a point of noting the changes made at each stage so that the effects of this or that modification on the results obtained can be traced and the intermediate models used can be saved. These should be stored and identified. We should be wary of names which at time t seem to mean something and which 6 months later are no longer understandable ("test\_support\_2\_z\_flexibility", for example). In case of software operating by lines of code, see the following paragraph. **E.3.2 Operating and commented code** In the case of a model imported directly in the interface, the user does not have access to the entire process of creation of the model. On the other hand, in the case of FE programs operating by lines of code, it will be advantageous to take advantage of the options that outline the entire model construction process. This makes it possible to retrieve all the reasoning and to understand how the software created the different parts of the structure and loads step by step. It is necessary to make maximum use of the commenting options to explain each line of code or group of lines of code, to quickly find the specific data you are looking for in the model, and for a person who is not familiar with the language of the software to at least be able to identify the main modeling principles. **E.3.3 Reflection about BIM** BIM (Building Information Modeling) is currently a new work method applied to the various construction trades. This approach aims to interconnect the different trades to create a single model from multiple files. The connection of calculation models to geometric models is beginning to be developed by software companies. Nevertheless, it is important to be vigilant and not to take for granted all the options presented as automatic. Indeed, FE modeling is based on an engineer's approach, to model only what is useful and necessary, whereas geometric modeling aims to provide additional information that is useless for mechanical dimensioning. The geometric model is created to present 3D plans and views of a structure, as well as the interfaces between the structure and the equipment, and to detect possible volume conflicts. It is not created to ensure that element connections are mechanically correct. It does not distinguish between main structural elements and secondary (non-structural) elements that should not be taken into account. It does not integrate any of the simplifications described above which are important to understand the functioning of the structure (for example the shifting of the neutral axis of successive elements or the reprocessing to obtain the nodes). Thus, the use of FE models derived automatically from geometric models does not necessarily save time compared to the conventional method, given the need for exhaustive control of the EF model, on the one hand, and the time required to rework the FE model to make it conform to the desired objectives, on the other hand. This is true at the time of writing, but companies are making improvements to their products every day, which could render the previous text obsolete. The BIM implementation, whose objective is to facilitate exchanges with other professions, should in no way cause us to lose sight of the fact that FE modeling is another profession, based on the added value of the engineer's viewpoint. In any case, the use of BIM to obtain a computationally compatible model forces to rethink the traditional modeling sequence (engineer/projector), to redefine the responsibilities towards the information ... which leads to define specific processes for the project. --- **Example of a structure whose calculation model comes directly from the BIM model:** *![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/csOPCT2xmvQHtnFM-embedded-image-a4na1lhu.png)* *BIM model* ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/CfSjCt4hf7rZYX59-embedded-image-e2g9feyb.png) *FE model from the BIM model* # Chapter F. How to properly present the finite element calculation note? #### **Chapter F. How to properly present the finite element calculation note?** This paragraph introduces the fundamental elements that must be present in a note to provide a clear description of a FE computational model. [F. How to properly present the finite element calculation note?](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/f-how-to-properly-present-the-finite-element-calculation-note "F. How to properly present the finite element calculation note?") # F. How to properly present the finite element calculation note? #### **F. How to properly present the finite element calculation note?** This paragraph provides the minimum elements that must be included in a note in order to provide a clear description of a finite element calculation model. First of all, the modeling note cannot be the first note of the project. It is either preceded or accompanied by the general assumptions note. The general assumptions note provides essential information about materials, foundation stiffnesses, load cases and combinations, and all the justifications that will have to be carried out on the structure. Ideally, the two notes are written in parallel. Often, points that would have their rightful place in the hypothesis note or in the modeling note are deferred to a later note. This way of doing things is harmful insofar as the clarifications arrive afterwards with a very long note containing the results and sometimes even the justifications ... generating tensions with the Project Manager in charge of the verifications (or the controller) when the latter will require to complete the work or even redo it and, above all, wasting time for all the parties involved. It is fundamental to understand that there is a real leverage effect involved and that it is better to spend some time detailing and fixing the elements at the beginning and have them validated. This will greatly improve the process. Let us not forget that in a basic verification mission, the general hypothesis note is the only one that will be subject to an in-depth examination by the Project Manager. **F.1 Note introduction - Description of the object of the calculation** a) The EF calculation note must begin with a brief reminder of the object under study. Excerpts from blueprints are always welcome. b) The study phase should also be mentioned. If the study phase is advanced, it is interesting to remind how the subject has been treated in the previous phases. Sometimes a simpler model was developed in the previous phase, sometimes a manual calculation was done. In both cases, the note should compare the results of the simplified model and the more complete model. c) It is advisable to specify the calculation objectives, i.e. the justifications that one intends to carry out with this model: global stability, internal efforts, deformations... The model is not an objective in itself, it is merely a tool to obtain a result. d) It is not mandatory to use a single model for all project justifications. Specify what will not be covered by the current model but by another sub-model. e) The modeling note must declare all documentary references used: blueprints with their index, market parts, calculation or geotechnical notes. f) In case of a model update, the changes made must be explicitly traced. g) The note must describe the principle of the results exploitation, the direct software outputs and the possible post-processing that are contemplated. **F.2 Geometrical description of the model** a) The physical boundaries of the study should be very clearly defined: which elements are modeled and which are not. Some secondary structures often do not need to be modeled (stairs or walkways, equipment). Some main structures can be simplified such as bridge abutments or piles, which can be represented by supports with their flexibility. In case of a succession of structures, the modeling boundaries must be described with the way to take into account the interaction with adjacent non-modeled structures. b) Hypotheses for geometric simplification, choice of nodes and sections must be set out in detail. The provision of a complete listing of the calculation file cannot satisfy this request. Drawings are required. Hand sketches, which the engineer uses when coding, can advantageously be provided. They help understanding the modeling logic. c) If there is an exchange between the drawing software and the finite elements software, it is interesting to indicate it. d) All the units used must be explained: distances, forces, stresses and masses. By default, the SI system is preferred. e) Define the global coordinate system for the model and recall the efforts sign convention for all support reactions. f) The same applies to the finite elements: the local coordinate system and the sign conventions adopted by the software for stresses and strains should be indicated. g) Images and graphic outputs are interesting to visualize the model, but they should be accompanied by the corresponding descriptions. A modeling note consisting of a series of screenshots is not acceptable. **F.3 Finite elements description** a) As discussed in [Chapter B](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/chapter-b-structural-dynamics "Chapter B. Structural Dynamics"), the software choice depends on many criteria. It is necessary to explain, even briefly, why the software used is appropriate. If it has computational limitations, do not hesitate to write it down and explain how these limitations will be overcome. b) Description of FE properties: this part is often missing in the description, yet some software has a wide variety of element types that do not have the same functionality. In particular, for plate models, the elements take or do not take into account membrane effects, which may change the results; this is also the case in 1D for shear strain in beams. c) Describe the number of nodes, the size of the elements, the mesh type. If a mesh refinement test has been performed (as recommended in paragraph d), report it. d) For a bar model, a table of the mechanical properties of the bars must be provided. e) The link between the global coordinate system and the local coordinate system should be illustrated with screenshots. Most software programs have quite explicit ways of displaying the coordinate systems. Note that it is often possible and useful to force the coordinate systems in order to facilitate the results analysis. f) It is interesting to give the number of elements as well as the number of degrees of freedom of the model. **F.4 Mechanical description of the model** a) The properties of the materials must be fully explained: density, Young's modulus, Poisson's ratio, static behavior law, shrinkage, creep or relaxation laws... b) Boundary conditions must be correctly described. The static diagram must be recalled, along with how the supports are modeled. If a stiffness matrix is introduced, explain how it has been calibrated from geotechnical parameters. c) If supporting devices are present, specify whether they are modeled by bars with special characteristics or by special connections in the model. d) Non-structural elements (equipment) must be listed and it must be specified which ones are modeled or, conversely, taken into account as loads. As indicated in c), this choice depends on the stiffness and mass of these non-structural elements. e) The way in which efforts and loads are introduced is not evident. It must be specified whether the software does automatic load placement, incremental load positioning or whether load cases are entered manually. f) In the case of a force to be introduced on a cut, it is necessary to illustrate how this force diffuses in the model (spider connecting the edges of the cut). g) In general, and in particular for seismic or dynamic calculations, it is necessary to detail how the masses are introduced into the model. If the mass of the elements is generated automatically by the software, in the assembly areas, there are volumes counted twice; it is therefore necessary to be able to correct the densities. Non-structural elements modeled by load cases are not recognized as masses and have to be added. A manual verification of the global mass of the model is always useful and reassuring. **F.5 Demonstration of the self-monitoring approach** Self-monitoring is a fundamental element of the modeling quality. This self-monitoring process must be visible to the person who is going to verify the calculation note. a) Tests and elements of verification of the mesh validity must be mentioned. b) All the model validation tests that have been conducted contribute to win the controller's trust. It is not a question of providing a large amount of information and data, but just indicating the tests that have been conducted. c) On the other hand, the verification tests for the vertical load calculations are absolutely essential. They must at least include the structural self weight, the self weight of the equipment, a uniformly distributed load and cases of thermal loads. d) This also includes global mass verification for dynamic and seismic models. **F.6 Description of effort recovery and post-processing** a) It is necessary to describe in which form the efforts or displacements of the model are recovered (listings, graph and chart reading, screen display). b) In cases where the results are expressed in a local coordinate system and a change of coordinate system is necessary afterward, the risk of error is frequent. The validity of the baseline change must be demonstrated. c) In general, the process of post-processing the efforts, with the associated tests, should be described. d) For combinations and envelopes, it is necessary to say whether they are made by post-processing or directly by the software. In the second case, it is necessary to indicate if the combinations are formed manually or if they are automatic (source of error). In any case, it must be specified whether the combinations and envelopes generate concomitant forces or not. **F.7 Results report** The results are often presented in the form of tables, sometimes cumbersome to understand. a) As said before, the system of units must be defined and the units must be systematically indicated in the table columns. b) It is necessary to recall the vertical loads calculation for elementary load cases. c) The dimensioning values in the tables must be highlighted (highlighted, circled or put in bold or red, etc.). d) Result listings should not be in the body of the text. They make the document more difficult to understand and lead to unnecessary printing. They will be placed in an appendix. **F.8 Specific complements for volume elements** a) The choice of cross-sections must be consistent with the expected results and must be consistent with the critical plans of the structure. b) In the same way as for surface elements, the software offers a wide variety of volume elements, with different codes. Some elements are very specific to certain materials and certain types of calculation. It is necessary to refer to the software's manual to choose the "simplest" element, unless there is a very particular need. c) It is advisable to give priority to results in the form of steel mapping highlighting the dimensioning points and specifying whether the values are smoothed or at nodes, for example. d) In the case of forces integration on a cross-section, it is useful to explain the method chosen. **F.9 Specific complements for non-linear calculations** a) It is necessary to provide the behavior law used, which may be different from the standard law of the software. b) It is interesting to present, in the calculation note, the evolution of a remarkable magnitude (displacement of a point, specific effort, etc.) during the increase of the load, to visualize the plasticity. **F.10 Specific complements for dynamic calculations** a) If a spectrum automatically provided by the software is used, it must be demonstrated that it has been verified to be consistent with the expected spectrum. b) It is necessary to define the selected damping (which is not the same in dynamics and seismic) and/or the behavior coefficients for seismic calculations. c) The participating masses and mode participation coefficients must be given mode by mode, and modal combinations and modal sign conventions must be specified, if applicable. d) Modal deformations should be presented for the most representative modes. The modes shape is an important element in verifying the global structural behavior. e) For a calculation by time steps, as for the non-linear calculation, it is interesting to present the temporal evolution of the representative quantities (displacements, accelerations, etc.). # PART 3 – EXAMPLES AND COMPLETE CASE STUDIES # EXAMPLES AND COMPLETE CASE STUDIES This part contains modeling examples for simple and more complex objects. They are presented as a complete or partial study or even a comparison of different models of the same structure. If you happen to have an example that you wish to share with us of a complexity or paradox noticed on a part of a model, please send it to the following address: [**elements.finis@afgc.fr**](mailto:elements.finis@afgc.fr). (It could be a note about a real project rendered anonymously.) **Example A – Modelling a complex high-rise building** [Example A – Modelling a complex high-rise building](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-a-modeling-a-complex-high-rise-building "Example A - Modeling a complex high-rise building") **Example B – Modelling of composite bridges** [Example B – Modelling of composite and steel bridges](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-b-mixed-and-steel-girders "Example B - Mixed and Steel Girders") **Example C – Modelling of beam grids** [Example C – Modelling of beam grids ](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-c-beam-grillage-modeling "Example C - Beam Grillage Modeling") **Example D – Simple example: modeling of a Br wheel** [Example D – Modelling of a Br wheel](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-d-simple-example-modeling-of-a-br-wheel "Example D - Simple example: modeling of a Br wheel") **Example E – Transverse bending of a prestressed concrete box girder** [Example E – Transverse bending of a prestressed concrete box girder ](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-e-transverse-bending-of-a-prestressed-concrete-box-girder "Example E - Transverse bending of a prestressed concrete box girder") **Example F – Dynamic calculations of tanks** [Example F – Dynamic calculations of tanks](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-f-dynamic-calculations-of-tanks "Example F – Dynamic calculations of tanks") **Example G – Cable-stayed bridges** [Example G – Cable-stayed bridges](https://wiki.afgc.asso.fr/books/finite-element-modeling-and-computations-in-the-field-of-civil-engineering/page/example-g-cable-stayed-bridges "Example G – Cable-stayed bridges") # Example A - Modeling a complex high-rise building #### **Example A - Modeling a complex high-rise building** - Franck DUBOIS - Structures Engineering - Thierry RICHARD - Structures Engineering ![](https://lh3.googleusercontent.com/4zW7ZebnniSBSdYfz5ZNdAzitu0N1kuHl-gkHFUo4Ae5tRYWBIx8S3FUPoizX-t5kRC68sNahAZyhZClp2-hLjntNFA7RbiP6kkBTDhMtA9M1uQAShqoxvrlyv_CJZ-aNHnNHAjXGS5Wu9-KyNlb-g) ##### **Part A: Presentation of the example** **Purpose of the example** This example focuses on the calculation of the general forces of a high-rise building using finite element global modeling. This calculation takes place at the beginning of the execution studies, its objective is firstly to determine the reinforcement of the foundations (diaphragm walls and drilled shafts) of the base in order to start the drilling of the diaphragm walls and drilled shafts. Then, in a second step, the modeling will be used to calculate the general forces in the walls and floors necessary to calculate the reinforcement of the different elements (walls, columns, floors). This example studies in particular the sensitive points of the modeling of this building: - soil-structure interaction; - seismic calculations; - non-linear calculations; - as well as phased calculations. Particular attention is paid to the management of the modeling, detailing its preparation, its integration in the general study, its organization and its validation. **Presentation of the project** This building is located in Monaco on a major urban site, in the middle of sloped soils. It is made up of 2 major areas: - a base buried in its rear area on 13 levels consisting of rear parking lots and dwellings including a school on the sea side; - a 25-storey tower sitting on part of the base. ![](https://lh6.googleusercontent.com/FEq7AiC9jDz5cMo6wmJZP6B3I5h21gvKYa_MxcOyViz92gKog1BrnZzKUOPMFJ3tuSFgorBqubDYOIwCMvld1RznioMqlHYbN4wS7MidE6XqpDtoKE7QvuHHZmHY32nQwiRxOCCHvOydGol4W2FEIw) *Figure 2: general view of the model (3D view).* ![](https://lh5.googleusercontent.com/kHCoFsfB7Eqmjo0t7riO0Ya__7PL5Yzwh8eMkA7B4z8SJSR3NSOFfVMKtCz8N-JUmZPuyJbpdAVM3N41uCkFyBSk6Y8UwhKaO5n2mxsVyR0RjVs662-cK2qEhfSRHEuM1Pg0F6xrFMmKXliXj2aLRA)![](https://lh5.googleusercontent.com/FZuB1GHSE9HQIY0rA-T0PV36z5Al5yoHiOpWsJrX_1a9dfbRyUQzJ0f6syCtoUPbWdvuvjBm9FSKYFSL4IP25-jPyzH_Q2_AD4ThC8lB-b72OPbwYuAJbcPyp5Rp7GuHCKOOFrcxyXPP7JB9f5SEiA) ![](https://lh3.googleusercontent.com/_tM6fi0MOl2CJ3d3ZwTKm9U4GT_JDbKvAudYJDwwrAXIjOa7_aQOGRVPff7WJEVto0j_cwUMM8YURWeLTJl2xg25a52Hrkq5989BiFEFSFSWYhaFeYf-cpEJK_ZhOEuAViTIAW5Ssf3m5XXOuPkj-w) --- ##### **Part B: Preparation and organization of the modeling** This is a very important step, because it will be very difficult to modify the model later on when it is advanced, so it is essential to have clarified all the characteristics of the calculation model before starting it. **A.1 Particularities and constraints of the project** They allow to identify the sensitive points of the modeling: - The large excavation area, the school area and the tower form a single monolithic block, there are no expansion joints. - The excavation is integrated in sloped terrains, its dimensions are significant (109m x 169m on 13 levels), its support consists of a peripheral diaphragm wall reinforced by buttresses and inner drilled shafts. - It is moreover asymmetrical with strong active earth pressure on the upstream zone and no passive earth pressure on the downstream zone. - Diaphragm wall panels rest on buttresses (no embedding) - The project is on an urban site in the middle of existing structures which are very close to the site - Presence of the high-rise building on part of the base - Taking into account a second tower (possibly built in the future) for the dimensioning of the base - Very tight work schedule **A.2 PRO file studies** The study of the calculation notes of the PRO file allows to quantify a rough estimate of the forces, and to identify the sensitive points. In our case, it clearly appears that the foundations are dimensioned by the earthquake cumulated to the earth pressure, in fact the foundations’ notes show very important shear rates in the diaphragm wall (5 Mpa) with reinforcement rates exceeding the usual uses. A resizing of the foundations will certainly be necessary. **A.3 Main modeling features** The first findings for the modeling are: - The size of the model will be very important because there is no expansion joint. - Taking into account the active earth pressure as well as seismic calculations are the key elements of the modeling. - The precision on deformations required due to the proximity of existing structures cannot be obtained through conventional structural modeling. It is therefore necessary to carry out simultaneously a "3D Geotechnical” finite element modeling which will be used solely to calculate the deformations. It will take into account on the one hand all the soils around the project and on the other hand the structure of the project itself. The active earth pressure applied to modeling will be derived from the "3D Geotechnical” model. - Asymmetric active earth pressures and their high intensities require consideration of passive earth pressure zones, and modeling of horizontal wall friction on the ground where possible. - The up and down excavation construction method without the use of tie rods, associated with active earth pressure asymmetry, has very important consequences on modeling. Indeed, during construction, the active earth pressures are taken up on the one hand by the peripheral diaphragm wall (which is classic), but also by the inner drilled shafts, which make the classical 2D calculations obsolete. It is therefore necessary to integrate the construction phases in the determination of the forces. **A.4 Input data:** It is necessary to list and validate all the input data that form the basis of the calculation: - The PRO architectural file - The PRO structural work file carried out by the project management (plans and calculation notes) - The overview of the reservations which appear in the PRO files and which unfortunately will evolve throughout the studies - The "2D" active earth pressure calculated by BET FONDATION in a first step, which will be used to develop the modeling - The "3D" active earth pressure that results from the 3D geotechnical modeling that takes place in parallel with the structural modeling. They will make it possible to correct the classic "2D" active earth pressure caused by the geometry of both the soils and structure (vault effects in particular) - Seismic active earth pressures that will be added to inertial seismic effects - Ground stiffness and friction in statics - Ground stiffness and friction in dynamics - Construction phases - Construction site methods **A.5 Output Data** They are quite simple as they are relative to the definition of the reinforcement of the diaphragm walls and drilled shafts, which are to be transmitted to BET Fondation so that it can carry out the reinforcement plans. **A.6 Interfaces between participants** The complexity of the input data and the ties between participants requires an interface flowchart to ensure consistency between the modeling and all other stakeholders. (see next page). **A.7 Assumptions Note and Modeling Methodology Note** The Assumptions Note describing the assumptions taken into account in the calculations (materials, definition of loads, etc.) must be accompanied by a Modeling Methodology Note describing how these assumptions are taken into account in the modeling (application of active earth pressure, calculation method, etc.). The Methodology Note sets out the principles implemented in the modeling and allows all project participants to validate them before modeling them. This avoids the long and laborious modifications that often occur when the model is finished. To simplify, this is equivalent to writing the modeling note before it is completed. ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/5s0nOOTVASvf46xc-embedded-image-s7a64emz.png)![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/HSKyzzjNyyZE87ZK-embedded-image-jimlzbdm.png) --- #### **Part C: Modeling** **A.1 Geometric modeling principle** **A.1.1 Breakdown into three independent parts** The modeling has been broken down into three independent parts, assembled during the final phase: *![](https://lh6.googleusercontent.com/g3s32uYO5dmcv2-ptoufPvKGKHUgbaWfvtspg6N42PwmDch78wcyLQnfyjbJHG_y7AIa-Frtg3maUsvBBJvAmpEQR31di1pimEuftABjY19Iqb9wXJ9kKiXiu0Xn5EgHBPuVoCEuTGQ6RglCVOgT2w)* *Partial modeling* *![](https://lh3.googleusercontent.com/hoNT35V_IUqdacKiJzEnfPcusRg0Nt1Jbaw7YxJzmz41myFg5gEDdb7saFHQlwbHyU7d6KgrD_68LCxQGmCf9j51XKHMkkRrzTqANY0wdbPyksu9seOT0HBYrb-fWafkOY7xZsM8ITcL6ms7o7ZHWQ)* *Complete model* **A.1.2 Coordinate system** The general reference frame is taken in the direction of the rear wall, which corresponds to the axes of the tower and overall to the directions of the active earth pressures, in order to make the seismic calculation coherent as it will be carried out according to the main axes of the tower. *![](https://lh4.googleusercontent.com/W-gnqnyzDp2FY5ZLxBuSPys7ZUxck205hNat1nJ97aEIjcu3GvloxiiUKHhBANKgMWKIDWOeX42yHK3HRmYDzhgwuJIebEWkBMDSJL78SiW5N56EJT5Twsrm5DdCI308JwLoY6AC6EXVt13wh7XVvg)* *Global reference frame* ![](https://lh3.googleusercontent.com/R1g2G-JsNZHEwN4ZCevRAdBlpo5h4XWkr_ayAUwoaKYlJZc8MlAEQb2rXYkMMry6SFaumlbIb0fDwlr3cJ-4OpbASh5ed2O2llLNIJZOkvdswsdJfS8ShUsKArGF51toHJmIgx3dPAOmsqSntHDP5Q) *Tower axes* **A.1.3 Using the BIM model** It could have been interesting to use the PRO file including a BIM model to generate the geometry of the model, but it soon appeared it was much simpler and more rigorous to study each level separately from the AutoCAD files to define the average lines of the panels. This helps understanding how the structure works and ensures the proper transfer of loads between levels or between the elements themselves. This manual step is important because it simplifies the modeling by removing local details that have no effect on the overall distribution of the forces, which will then be the subject of local studies. It mainly deals with the alignment of walls, slabs, the removal of small reservations, the removal of secondary walls, etc. **A.2 Modeling of the rear zone of the "large excavation" base** **A.2.1 Model features** *![](https://lh4.googleusercontent.com/pjKnHWOthtvGIaG870BHCRQtOoyE3Djh5FqwEoOxwpvAHnE_nPMN7hqYKKEaYj8Rz1qS_R9_thBb8mQk18w-xraRZIWWdHXvhyC1g04SXEyvdf-sKbsi4Ru5BAe6i7X4zzXbHRPW79HbaCqRLpVgAg)* *Model view of the rear area of the base: large excavation* It is the most delicate zone because it is subjected to earth pressure, and it is done from the top to the bottom with the following phasing: - Diaphragm walls and drilled shafts - Upper slab (tower support) - First level earthworks levelling - 1st floor concreting - Lower levels according to the same principle The active earth pressures asymmetry between upstream and downstream requires a partial active earth pressures resumption by the central drilled shafts during the levelling, such resumption not being calculable by conventional 2D methods – hence the need to proceed to a 3D phased calculation. The main features of this modeling are: - Modeling of the diaphragm wall in shell elements with the installation of springs at the junction between panels - Modeling of the buttresses into shell elements, with springs modeling the support of the diaphragm wall on these buttresses - Taking into account passive earth pressure zones in areas that do not affect the surrounding areas - Taking lateral earth pressure into account in areas that don’t affect the surrounding areas - Making 4 seismic calculations (+X -X +Y +Y directions) - Phased calculation of earthworks phases ![](https://lh5.googleusercontent.com/LNVnVMmFS3IPnoXG-M8Ri-3nqp7j9WrnrkrjNTlkFhCvg5uy3JTQTuUitkLVRctq1efGEGKcbWWldUPKfdikPkpzHGcFVEWnE_O4hEg3QzmBie01xseRvhYa06yvNzFMe53w75O_N83CsmAV5nTLlQ) View of the large excavation without the upper slabs **A.2.2 Soil modeling by springs** The connection of the diaphragm wall to the soil depends on the direction of the force: - Either the wall presses on the soil, the spring is then in passive earth pressure, and its stiffness is in passive earth pressure - Either the wall pulls on the soil, there is then a detachment, the stiffness of the spring is thus null (the wall is in fact in an active earth pressure state) ![](https://lh3.googleusercontent.com/HpU7xiO_K2pBsojb1Ce5Dr31B2cdhGxNsHNuHa5XSUbXBc-qHIKNGDfXkdXaHvq-Gsj41YUp0xpa5UbmwGHv-DlkHaeePlukJBlw19G6U0rcKAVRH0kAJHmYRHm7yDLnHdf8jR1u77vvLw9rF6PoVw) Active and passive earth pressures of walls framing a floor There are therefore active and passive earth pressure zones for each load case. We have considered 2 methods: - Either define manually by iterations the passive earth pressure zones for each load combination. - Or use non-linear springs working only under passive earth pressure. This non-linear second method was adopted, as the calculation times proved to be acceptable. Two laws of physics are used for soil modeling springs: ![](https://lh3.googleusercontent.com/nT8vCRL2ukufNgdHkrlG6YkIAUSMB3ic984hOGSbmqLq2K5HIpyYTyusqVO6jYlPMKxMLeVRFUU5G3T8vFt0YJruaYXEpfo8RW7z8shxTfF43khM13ZiKq0lTB6lCU8k-IobFYTGEN4Y-r3l3dX5qA) ![](https://lh4.googleusercontent.com/Jv8kjxXxZpQ87ThwyGZ2Wm_fvln1mKt2kKkOBSRxyah9j1YnALJrm1sZY2xeHShuhTvzUhS7tE541h0iSEZ5pm06HVHzIKBLxlYLGVxhPKUYyTKcXJt3CfjnNQKzhaMtjgx_TfcPqzsTH10znb5llQ) *Springs in passive earth pressure. Friction springs (passive earth pressure at the bottom of the excavation).* The friction springs are horizontal: there is no friction in the vertical direction. These springs are relative to frontal stiffnesses and friction stiffnesses, and they vary according to the soil layers. *![](https://lh4.googleusercontent.com/SmVftbp6Nkb-dwEiIu806pUGkNxHDFyvxMPYduOiBQKx-JSqIscM1OE3rUN4PQf2XvHxvlHQjZ_Tv4I9SNNH0aCifHHlWJMhDp3MHmvUZfYXRwrlwckbKkhFCXYbrUS_1qFQWNxiQySNFkWvkGFRbw)* *Example of soil spring location* **A.2.3 Connections between panels of molded walls** The connection between diaphragm wall panels and drilled shafts or between diaphragm wall and buttress is modeled by a gap between the elements: 0.20m between panels and 0.5m between wall and buttress. The 2 panels are then connected by a non-linear spring connection with the following behavior law: *![](https://lh4.googleusercontent.com/dGtDx7qDsVBoFzR0JKmgcCCugqMc97iu1F7Y23N3drWPeU4pSaVtbIFbFJTS_B8Za54h2UOWL2UPlXp5GT-9nvxDVQIcm_99WV-nYlVv0E-hM8dmNCUVIwTxiv8IX2iKEIJW6HcbBlTlN-3Eq56tiA)* *Connection between panels of the diaphragm wall* A friction coefficient of 0.7 is added to model friction in the panel contact plane with a limit of 0.7 x normal stress to the surface. **A.2.4 Connections between the buttresses and the diaphragm wall panels** They are carried out according to the same principle than for the connection between diaphragm wall panels. *![](https://lh3.googleusercontent.com/MxR22af6PlS2jJguoTn7dlbPLVXKn2Skb3qPa9vtvlmLR_UpMHKccJvgm-0HQbQRP4a2LVlG7GIgKh2Bqboz0Ig71Kqm81NpF2RA-0ZB4tMOOqv11MeIp1C7potC-CmMLhVLv72OawdU5_hVRBsL4Q)* *Connection between the buttresses and diaphragm wall panels* **A.2.5 Loading** **A.2.5.1 Weight loads** They are simple to describe: dead weight, additional permanent loads, and overloads. **A.2.5.2 Static active earth force** They are derived from 3D geotechnical modeling ![](https://lh4.googleusercontent.com/oBkuCVoopEY0GuGZ5GqBpyudnDtcG2a6m3iQbl3W7gZu4IvMWi3uMl7Zz4jvlC0WWgrdwjRD5XfoQqEXVr7199a1Z7GvWDwwDZ1nMuwgUfXpZzdi9BqFjXBWIRuyBptuRs4YFJIAl35OKF0yOgNMVA) **A.3 Modeling of the front area of the base (school and dwelling)** This modeling is much more conventional and traditional. It is made up of shell elements (floors and sails) and wire elements (posts and beams). The foundations are modeled entirely as for the rear area. This area is only subjected to weight loads. *![](https://lh6.googleusercontent.com/LWK0GU4_xPCnaw4G3vFfWbMIrM4zksRA6VGNOFAsO40d4kc_bLx-PuBBHkv_9BTMQBwJTGJV9OK2b_ccx_ud88qKZAhqOt27p4L90iwLSKxp7i8hfsId1Ff0pNwZv8q9NwSfuHlDh4KQY-UO_tD0gg)* *General view of the school zone model* It should be noted that the lengths of the lower levels exceed 100 ml, thus exceeding the regulatory lengths for taking into account the shrinkage effect. A calculation of this zone under the shrinkage effect will have to be carried out during the second phase of the study, in order to determine the longitudinal reinforcement of the walls and floors. For homogeneity with the large excavation, the piles of the foundations are modeled entirely with the installation of horizontal and vertical springs according to the soil layers. ![](https://lh4.googleusercontent.com/QnbELNCxWLWbVxxPA9gG-MuJFbfDwWlcJzaLV5Vli2eKMQRLwCffqUOnQOyu-AAVdpvIfI0iswrKwwJ_251XIsa3no0qDrzmDCFLBSDcpVHdVH_k_RiEtO58vTngftm14W-h4qtuF_B9DsXLzIKjJQ) **A.4 Modeling of the tower** ![](https://lh6.googleusercontent.com/U0FMJhrdjVjID-w3dOKiKCoYDC1LH5gwzl58n6vcNI0yGRP4wV9DJnvPupZXUVNb-AwwC4I98VLyVFk201zTCsKJa_EfPfiv7IMNIVSOGo3cH0Pe5ucIQcVttZCrqZd_NoM8IJUNBiylIRzikMRNlw) The modeling of the tower is conventional and traditional, consisting of shell elements for the sails and floors and wire elements for the beams and posts. The main problem is the large size of the number of elements due to the large number of levels. In the first step of this foundation calculation, the tower only interacts by its effects at its base (upper base level). The size of the meshes does not interact much, it will thus be large meshes. *![](https://lh3.googleusercontent.com/Isj3P2cG_qfDGEclSYKBjOuuU5wQnXKEv9THgnuCQ5NCr3mBVzW55FNcyjOR2Gx2HliE701elreiYB1TRRLqmR7PZmKdB2LkjSpniX7YvH2bvAahtx3CY2YYZIZxRO9nvbQUMKqxAXsmcRFuhBiJzA)* *View of a typical level of the tower* One of the peculiarities of the tower is the design of the slab edge which is very complex and variable at each level. There are no two identical slab edges. The layout of the slab edge had to be worked on in order to remove many points from the architect's original DWG file, which had very small distances between two points – even down to the millimeter. ![](https://lh5.googleusercontent.com/NyyldtFLe7ULZ4PJbzBZjiUX3nO-yt-_j9toCBYcayzP7IWB-kLPJV6EUPonzHdC78FYwaTlkN0awyD0bS_wbOTkr9atJ8qNJ-hE_tmtRVEBi5ieHr7JtttoFCB0Ikry_5nG8y0b5U8wwX_NCriAJQ) *Meshing of the slab before purge the useless points on the slab edge* This example shows the problems encountered during the automatic recovery of DWG or REVIT files. Although it does not initially study the effects of the wind, the modeling includes at each floor the definition of a "WIND" node positioned at the center of gravity of the floor and connected to the core walls by rigid links. These nodes will then be used to introduce the wind load torsors calculated in the wind report for each level of the tower. **A.5 Modeling of the optional second tower** This second tower is identical to the first one and may be built in the future. Whereas for the first tower the need to model it entirely by shell elements quickly appeared, for this optional second tower, we studied solutions limiting the model size. **A.5.1 Solution 1: modeling of the 2nd tower by its forces torsor at its base** This is the simplest solution which consists in calculating the resulting torsors at the base (O2 point below) for each load case and applying them directly to the general model. ![](https://lh5.googleusercontent.com/9qL_vzW6jrUe600nbmP3Rk6EjNDNagU4WMGRZ54CKwDmWVKMUz4hd0KNdvVIPrLhIMhIJje0dSuiATDgOgtV7kjpDPmrMjGtPUpxN15zpOdl_xCO8D1hJ0GSQHHtneK4uKj0MCoSsUvsqjH-dmTetg) The resulting seismic torsors of the 2nd tower are then calculated on a model of the tower alone which is embedded at its base. This method could not be implemented because it directly adds up the seismic forces of the two towers, thus generating inadmissible forces in the diaphragm wall. Indeed, it appeared during the PRO file that there was no seismic interference between the 2 towers. **A.5.2 Solution 2: modeling of the 2nd tower by a skewer model** We realized a skewer model of the isolated tower. This model consists of a vertical bar modeling the core whose characteristics are defined from test cases of the tower model by arranging horizontal loads at the head (according to X and Y), then by studying the equivalent inertias producing the same deformations. Given the asymmetries of the floors, it soon became clear that the conventional skewer modeling consisting in assigning masses at each level is not suitable, because torsion is then not taken into account. Each floor has been cut into 4 parts to which the corresponding masses are assigned. *![](https://lh3.googleusercontent.com/UQLJ7Bx6-RYPKCq7r2LxXT35eiWA-WYfNwMgkH6bVqHP-xwe063WsgaLtnYeM8mvivGH5z4j6fQLl6NJno3RV5UCk-bhY6cGe1kTDl8ljJJ4N1pdF3eA1C5sIILZx2U-dGKvGB07TzAfgs6RCKOZJg)* *Visualization of the skewer model* We then compared and validated the resulting torsors between the 2 calculation models under the CQC seismic cases, and compared the main modes. Mode 1: transverse according to X: ![](https://lh6.googleusercontent.com/2W1G9PeIpU90n6JCBkA9JLRqK02dKX1wmr-JLgEeNyT1VNC_ypG8YcWHw1Zok5BPbHOwmNDBee-irypWaXZZMxsizLQ0ml6qjbD8_l2cGM7qBE39sSkB7IvktUZLUy3MVDqTKWH9gv7S-QLVx7XecA) ![](https://lh6.googleusercontent.com/b5xoYa7hvznmC8lE2Z_44eY8bn89Bos6Hju5aC-pmHfFUAqWojeQwsgaOUF8NJCblV2dj9asWWuiE85a6dt6YSNLa0BJW_pDYVp_5axo2DM5k_fGEtmrizwXUc2cybKgBc61iNuiXM8uJBxgRFQGCw) f= 0.68 Hz with 56% of the mass f=0.63 Hz with 62 % of the mass Mode 2: Longitudinal Y: ![](https://lh5.googleusercontent.com/0XKgz9fxGlBBZj6S6U8lBJB7x26-49NbT-zn4XScHSoyPEwYhQUazM5VlEk250hby77k-6WlH6sVks9gce0ZhFXMY4lioK7nki1CufCwW-uNaeJF2Pyj-b08QLGz6vZRp95vO4zFDHwA11uKUqRenA) ![](https://lh4.googleusercontent.com/Rrz7PhC9h43FdXvhjcbGh1GBpeoBtaenFSvM2y2XBJri6q6_vPYwOHaCFN6jYTVl8riAR-dRqc_-cNZmFM7eXkiiM43977J8Fu1bvTpo7Q3orCg8d-cqbPZU2QsPX2yylFi6VLihlC7fvhOcjaIDnA) f= 0.77 Hz with 66% of the mass f=0.70 Hz with 62 % of the mass Torsion mode: ![](https://lh6.googleusercontent.com/-EndyXWPSPxaniUtLyWjzSAwi6ALtH3DP4p3RGOuH3Y32F9_hLkdS0qL7aFq-Ctt2vc-9mOhdFim79WSva48uNffgar5ZZQRp0UmvzU7q3PptWVG6oiXhtzAl-UVF-nIOh8pz0p8i6ql7NLLp_5zRQ) ![](https://lh6.googleusercontent.com/f747x50LDa4RQn7KMCwNGY72ToH9HoURFENABPjDcSNsJrIiGXwEZ3YqX2tkYw1b5Rxum5RC6Vnr2bFhnOajDZUDstkqRMe2w550LDAo2dibR-ObfFuh8lzHIO1K1_p0F_hUM_tp-yisqLURTFmHqQ) f=2.2 Hz f=1.3 Hz Vertical seismic mode: ![](https://lh6.googleusercontent.com/vVWAv6PTgiuojYMMgMnMBFFEjKU_EbGzVHUA5_xNHew70v1XceyDc5M4fx4p-lGGuZDb7WWktn7lWva4BcGCFYpQkWBcIEbAlMV7lfEZ_KsplkFRh8tFXqBVejw1PMuUoUdZbRYWR5JMWrCtfv3iBQ) ![](https://lh5.googleusercontent.com/9Qi1QZQI2C0OvGUFxO-N4w9-8RTK7jjQRcPjoJPzBZnq9l8i7Ar4hHNO3_yMqNi6N4nH2ZxNARgVR_B6GyBX6Osprs-0VYWBdDsw4c76sv4IT952xkaWw3wkbQkmSo_ugRoEua8C9Hl0669ZBAbp4w) f= 5.0 Hz with 73% of the mass f=5.5 Hz with 82 % of the mass The validated skewer model was implemented in the general modeling by having rigid joints between the base of the skewer, and the diaphragm walls and bearing drilled shafts of the large excavation. Compared to the first solution, a decrease in the forces in the diaphragm walls appeared. On the other hand, the rigid connection has generated very significant not admissible forces in the diaphragm wall, which do not appear in the connection of the first tower. Therefore, the first level of the second tower should be modeled in shells to obtain consistent results. This solution has therefore been abandoned in favor of the third solution. **A.5.3 Solution 3: modeling of the 2nd tower entirely by shells** It is the solution that we were trying to avoid that was used!!, the calculation times have increased while being reasonable. ![](https://lh6.googleusercontent.com/3NyAWiSttfPN5iRHmoEQD0Uv1omimiYZH1NhW5xDyMjlvhNl9zPbGNWWk-FZeCFXWCbAhC6oiYNYxfoARq66j3uW1TB0CTgezRezOeSJ7600kFD4lWjTzj9bVni7otFcgSbrq0JLFIXDBNth613EoQ) *Rear view of the model showing the anchoring of the 2nd tower in the diaphragm wall* **Part D: Global modeling calculations** **A.1 Global model features** The global model is meshed with elements of 1.50m size, except for the foundations (diaphragm wall, drilled shafts) with smaller meshes of 1m. In the end, the model includes 168,000 nodes. The total calculation with phasing and seismic calculations takes one night. **A.2 Phasing calculation** The calculation takes into account the 18 construction phases (earthworks) of the large excavation. Then the school zone and the tower are activated. Operating overloads can thus be applied to all floors of the model. **A.3 Seismic calculation** **A.3.1 Modal spectral calculation** 4 seismic calculations are performed in the directions +X, -X, +Y, and -Y, neutralizing the linear springs in tension in each case. These cases are then studied twice; with or without the 2nd tower. There are therefore 8 modal spectral analyses. ![](https://lh3.googleusercontent.com/Z2fiWHb8SdigxVQt_Ruxfih__2YLaclmEt8kzEkj2CMa4hmrhDbhOkkmPSwJTjvsOYmV7Gb0Wwc3RL7mDZ99XXTZr7gRD2jPiRg49zkgQRWhaNfKTSJYUl6Q4O40PB1kt2TSCLqPRC_U9d3duH2Xmg) Modal analyses are carried out on 100 modes, which allows to interest at least 70% of the participative mass. The residual mode is then added to reach 100% of the mass. The 2 calculations with or without the second tower are quite close, the 1st mode is 0.471Hz with 2 towers, and 0.582Hz with only one tower. *![](https://lh4.googleusercontent.com/fVGkmPtX1CpaK5xzW8_uXAR24suiz64UQR_yElNoYLxpUR49Ubk8YyEaH3YtpBZtn1Xw8FE53QC2CptAMwXT1Wjl1sUoIrbVnAd2ywfNGcNLGECcxdhZyxTk23OJZw4OHLhxCE2lbgvHoBf14Wbtlw)* *First modes visualization (with 2 towers)* **A.3.2 Seismic active earth pressure** Dynamic increments are applied in the 3 directions +X, -X, and -Y. They are added to the static active earth pressure. ![](https://lh3.googleusercontent.com/DHNogLRFxjk0Xfi87g02ttZ16evysNTLSiRCL4JZChwz8c_KaRhC6nBv1Re-9dzQIeoyqHgdMS9NLb2lccWkEE0cOUS9iDyU_I8xsDXPrRoCcUaDiDb-rE4EfMDmpgbneCf8SO5yOzHqpBNIzcLCFw) Cumulative dynamic increments with static active earth pressure The seismic active earth pressures are then added to the inertial seismic forces from modal/spectral studies. **A.4 A few results** *![](https://lh3.googleusercontent.com/V3OpPkjT0Ni2lDL8o2MJ_mqHp1UwTZPpycrxeiknTRW_lpHLQQzpRgqwM9YGD94RWPtpBrYiZr5Ov0bE5K_CxDLNtrdJYgTG36ZDWq4SV6voFj-UT-B2NcXoXwsIUiBz4onBb59zL-dNX6yZ8L3zng)* *Cumulative phasing deformations* *![](https://lh6.googleusercontent.com/iX5jQf17ah7RAgpV7SsvDnN1vzNZIZD9I38s1_4StC8n9LQdIrnPyS02o1NZ3qVZ_MG4n7UFNxyqvWFI02My_q1NZ8Iv_sXgp5XCgd1Ga6MuBvGySgOdMJeRXScSXFuxjc6fkFGOhipKdqKTSxCEqg)* *Deformations of dynamic increments* *![](https://lh4.googleusercontent.com/J79xlKlVbD0OHrjtlLYUPFRT9zvIZ96qgM0X2HgQx2FR56246shxN_r9Fnf1Akhzii1KEqjkedV71VDSgBUPVlLP0UzCc-JLu_PYpuacTaI6yFirZRkGTNka3HzDUGQ-GdOvznac3krncC3esTWmbA)* *Seismic CQC deformations +X direction* **A.5 Iron framework of the foundations: diaphragm walls, drilled shafts and buttresses** The global forces are calculated for the SLS and ULS limit states, and ULS seismic. Cuts are made over the entire height of each panel to deduce the global resulting forces. We visualize below the graphs of the forces in a buttress in the SLS state. *![](https://lh6.googleusercontent.com/C8NtuehFnI0LMIBHLVDBU1IPDfbLI5VOk363D3wbVciNZOIPU1GV3XxyaMtrSH8uWsNWHIkJI7W0h3wy97WMK7LsK3r77_7LGielaznwYK83NmTDUUSFWg-OaPvgWbgV4sIRz1Jxa5rH8PbwuwSepw)* *Normal stress in a buttress* *![](https://lh5.googleusercontent.com/IoTZxTQradOqaABJGWFRwhs3GR94SVYOQem1bQ-XDRCvTnaXCO-BtXsHf4aH5UDH2_mGA8dhfQucQowEnHxU-sorSBDsCfQ98JUBVWqpTl6FOoNpVkgcEiNoy_Wb1EU84-3v2BZU9ZWrffSK_mXekA)* *Bending moment on high inertia* *![](https://lh3.googleusercontent.com/fgwqkR6CBv20e1LtedjEbMb_F3R2vZAGoEraQgivuzfGZRy6Hu6eBmOnnol4h4UcCencdd7do8L0Z1wjN9F9Wn4eJVojRYlFGxtGI1Ct_HMj2ySs53Ok6DLAh-gsk4rLIhgpYM2IIFVDjwdVTDs42Q)* *Bending moment on low inertia* The iron framework is then calculated by applying the usual and regulatory rules related to reinforced concrete. --- ##### **Part E: Modeling validation** This is the fundamental question of complex modeling: how can we show the validity of the results? Several types of validation were carried out. **A.1 Comparison with PRO file studies** The main results were compared with those in the PRO file: - Mass balance - Torsor of support reactions for elementary load cases - Deformations under permanent loads and earthquakes - Specific modes - Etc. **A.2 Internal validations during modeling** They are carried out during the modeling and during the verification of the main results Moreover, they relate to: - Geometry visualization, local frames, thicknesses, etc. - Graphical visualization of the loads applied to the model, - Visualization of steel mapping to show any problematic zones identified by large steel sections - Visualization of the deformations of elementary load cases **A.3 Internal validations by a partner not involved in the modeling team** A person external to the modeling team checked several points: - Activation and deactivation of groups of elements (surface, wire, or spring elements) in the calculation phase - Behavioral laws according to input data - Behavior law assignment for all passive earth pressure or friction springs, depending on panel location and level. - Orientation of non-linear springs which only work in compression - Respect of the springs’ plastic zone during the different phases - Loading of elements **A.4 Modeling validation meeting** Outside the modeling team, it is absolutely impossible for other project participants (project managers, technical controllers, construction site, other technical design offices, etc.) to understand the details of this "black box" and to be able to validate the results of the model. A general meeting was therefore scheduled "live" in front of the modeling computer. Everyone was then able to request data visualizations, request additional results, understand the model structure, see all the parameters included in the calculation data, access intermediate results, etc. The aim of such a meeting is to answer all the questions raised by the participants directly with the modeling computer. --- ##### **Part F: Calculations of the structure’s iron framework** The modeling will be completed in a second phase by the calculation of wind and shrinkage forces. The mesh will be refined for the tower’s walls by adopting 3 meshes on the height (i.e. a 1m mesh). The walls will then be calculated directly from the results of the modeling by making cuts at their base. The bending forces of the floors will be calculated "manually", i.e. with local modeling, which will be added to the membrane forces (N and FXY) determined by the modeling in order to determine their iron frameworks. ![](https://lh6.googleusercontent.com/FvI1KM0Dign83dn5mLgNlTA5ZKyVGOMBHpSleH-sMFiW3YgVpxWAYs-bHt75kX2d2J_p4qbWPy8Rv7mAOw9cpMji-gFWU9EVzDx1bLO4aXTjxNg2Fe0UIensSN2jrGOFyRXkkW_GqWa1vonEcT2V9A) *FXY membrane forces to be taken into account in the slab calculation* # Example B - Mixed and Steel Girders #### **Example B. Mixed and Steel Girders** ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/KBl34y85n5SFZMPt-embedded-image-9pqhqhrh.jpeg)The subgroup responsible for these examples is still working on the subject. Some patience will be required.
--- **Mixed Structure** ![](https://wiki.afgc.asso.fr/uploads/images/gallery/2023-09/cGOMeyUcweV1e9J6-embedded-image-rghduae7.png) This subgroup has studied the same structure in three different ways: - A 2D wireframe approach (link) - Valentina Bruno (Setec tpi). - A 2D beam grillage model - Hugues Somja (INSA de Rennes). - A 3D model - Aymeric Perret du Cray (Setec tpi). --- **Orthotropic Deck Steel Structure** -**J\[m4\]** | **Software** | **J=∑ab3/3** | **J=∑ J\_Caquot** |
Beam | 0.0191936 | 0.0261760 | 0.0199764 |
Cross girder | 0.0069919 | 0.0078125 | 0.0069646 |
Beams y (m) | **Guyon-Massonnet method** | **FEM model** | |||
K | Point load Miso=P∙l4 | Distributed load Miso=q∙l28 | Point load | Distributed load | |
Edge | 0.405 | 150 kN.m | 112 kN.m | 169 kN.m | 99 kN.m |
-3.375 | 0.244 | 91 kN.m | 68 kN.m | 121 kN.m | 65 kN.m |
-2.250 | 0.188 | 70 kN.m | 52 kN.m | 107 kN.m | 52 kN.m |
-1.125 | 0.170 | 63 kN.m | 47 kN.m | 102 kN.m | 48 kN.m |
Center | 0.166 | 62 kN.m | 46 kN.m | 101 kN.m | 47 kN.m |
\[m4\] | J = Σab3/3 | J=Σ J\_Caquot | Software | FEM = G-M \[y=b; e=b\] | FEM = G-M \[y=3b/4; e=3b/4\] |
Kp | 0.0261760 | 0.0199764 | 0.0191936 | 0.0282102 | 0.0258026 |
**Beams** | **Moment - Bar model:** **beams of identical inertia = basic case** | **Moment - Bar model: variable inertia beams (edge) and end cross girders** | ||||
y(m) | Point load | Distributed load | Point load | Impact | Distributed load | Impact |
Edge | 169 kN.m | 99 kN.m | 154 kN.m | -9.81% | 86 kN.m | -15.24% |
-3.375 | 121 kN.m | 65 kN.m | 123 kN.m | 1.31% | 66 kN.m | 1.62% |
-2.250 | 107 kN.m | 52 kN.m | 107 kN.m | 0.60% | 53 kN.m | 1.15% |
-1.125 | 102 kN.m | 48 kN.m | 102 kN.m | 0.01% | 48 kN.m | 0.02% |
Center | 101 kN.m | 47 kN.m | 100 kN.m | -0.23% | 46 kN.m | -0.47% |
J\[m4\] | Software | J = Σab3/3 | J=ΣJ\_Caquot |
Beam | 0.0191936 | 0.0261760 | 0.0199764 |
Cross girder | 0.0069919 | 0.0078125 | 0.0069646 |
End cross girder | 0.0232905 | 0.0318938 | 0.0232925 |
Edge beam | J=ΣJ\_Caquot | 0.0242880 | 0.0181062 |
Max. span moment | Beams – y(m) | |||||
edge | -3.375 | -2.250 | -1.125 | Center | ||
Isostatic deck with a 70 degree skew | Point load | 147 kN.m | 120 kN.m | 107 kN.m | 101 kN.m | 99 kN.m |
Distributed load | 77 kN.m | 61 kN.m | 51 kN.m | 44 kN.m | 43 kN.m | |
Note | The influence of the skew is very small and the common cross girders (hollow core elements) are arranged skewed. | |||||
Isostatic deck with a 50 degree skew | Point load | 138 kN.m | 105 kN.m | 98 kN.m | 88 kN.m | 93 kN.m |
Distributed load | 72 kN.m | 54 kN.m | 43 kN.m | 38 kN.m | 37 kN.m | |
Note | The common cross girders are laid out straight. The end cross girder, on the obtuse angle side, is in flexion rather than torsion, therefore it reduces the span moments to its detriment. | |||||
Statically indeterminate deck (2 spans) with a 100 degree skew | Point load | 130 kN.m | 105 kN.m | 93 kN.m | 90 kN.m | 88 kN.m |
Distributed load | 65 kN.m | 51 kN.m | 41 kN.m | 37 kN.m | 38 kN.m | |
Note | There is no variation on the load distribution between beams caused by the deck being statically indeterminate | |||||
Statically indeterminate deck (2 spans) with a 50 degree skew | Point load | 132 kN.m | 97 kN.m | 91 kN.m | 82 kN.m | 87 kN.m |
Distributed load | 66 kN.m | 48 kN.m | 36 kN.m | 33 kN.m | 31 kN.m | |
Note | The fact that the deck is statically indeterminate causes little variation in the span moments. | |||||
Max. pile moment | Beams – y(m) | |||||
edge | -3.375 | -2.250 | -1.125 | Center | ||
Statically indeterminate deck (2 spans) with a 100 degree skew | Point load | -63 kN.m | -40 kN.m | -33 kN.m | -31 kN.m | -30 kN.m |
Distributed load | -70 kN.m | -46 kN.m | -41 kN.m | 39 kN.m | 38 kN.m | |
Note | No variation on the load distribution between beams caused by the deck being statically indeterminate | |||||
Statically indeterminate deck (2 spans) with a 50 degree skew | Point load | -84 kN.m | -53 kN.m | -31 kN.m | -28 kN.m | -27 kN.m |
Distributed load | -92 kN.m | -46 kN.m | -37 kN.m | -36 kN.m | -36 kN.m | |
Note | There is a concentration of moments close to the obtuse angle of the load. |
**N (t)** | **e (m)** | **M hanging beams (Ton\*m)** | **M model n°1** | **M model n°2** | **Difference %** | |
Distributed load | -32.30 | -0.69 | 3.35 | 25.64 | 23.71 | 8.1% |
Bc system | -25.17 | -0.69 | 6.93 | 24.30 | 23.20 | 4.7% |
Point load | -6.49 | -0.69 | 1.51 | 5.99 | 5.86 | 2.2% |
Model n°1 | Model n°2 | |||
MYY max (Ton\*m/ml) | MYY min (Ton\*m/ml) | MYY max (Ton\*m/ml) | MYY min (Ton\*m/ml) | |
Case n°1 distributed load | 0.91 | -0.40 | 0.92 | -0.43 |
Case n°2 Bc system | 2.75 | -1.89 | 2.82 | -1.91 |
Case n°3 point load | 1.11 | -1.59 | 1.14 | -1.62 |
Cross girders | In non-cracked | Ix/10 | Difference % |
Distributed load | 23.71 | 25.94 | 9.4% |
BC system | 23.20 | 23.98 | 3.4% |
Point load | 5.86 | 5.91 | 0.9% |
Hollow core element | In non-cracked | Ix/10 | Difference % |
Distributed load max | 0.92 | 0.97 | 5.4% |
Distributed load min | -0.43 | -0.52 | 20.9% |
BC system max | 2.82 | 2.88 | 2.1% |
BC system min | -1.91 | -2.01 | 5.2% |
Point load max | 1.14 | 1.21 | 6.1% |
Point load min | -1.64 | -1.75 | 6.7% |
Guyon-Massonnet coefficients -> to divide by 11 | ||||||||||||
Beam | 1 | 2 | 3 | 4 | 5 | 6 | 7 | 8 | 9 | 10 | 11 | |
Y= | -4.5 | -3.6 | -2.7 | -1.8 | -0.9 | 0 | 0.9 | 1.8 | 2.7 | 3.6 | 4.5 | |
Super distributed | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | |
Left cross beam | 3.287 | 2.523 | 1.860 | 1.317 | 0.893 | 0.577 | 0.348 | 0.186 | 0.072 | -0.013 | -0.081 | |
Right cross beam | -0.081 | -0.013 | 0.072 | 0.186 | 0.348 | 0.577 | 0.893 | 1.317 | 1.860 | 2.523 | 3.287 | |
∑ cross beams | 3.206 | 2.510 | 1.932 | 1.503 | 1.241 | 1.154 | 1.241 | 1.503 | 1.932 | 2.510 | 3.206 | |
q span | 2.407 | 2.089 | 1.751 | 1.407 | 1.087 | 0.812 | 0.586 | 0.406 | 0.262 | 0.144 | 0.042 | |
support | 1.347 | 1.412 | 1.459 | 1.445 | 1.322 | 1.136 | 0.933 | 0.738 | 0.560 | 0.401 | 0.257 |
Beam | 1 | 2 | 3 | 4 | 5 | 6 | 7 | 8 | 9 | 10 | 11 | |
Moment on support | ||||||||||||
Self weight | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 |
Superstructure | -2320.0 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 |
Cross beam | -391.0 | -114.0 | -89.2 | -68.7 | -53.4 | -44.1 | -41.0 | -44.1 | -53.4 | -68.7 | -89.2 | -114.0 |
Span | -2109.0 | -461.5 | -400.5 | -335.7 | -269.8 | -208.4 | -155.7 | -112.4 | -77.8 | -50.2 | -27.6 | -8.1 |
M= | -18389.0 | -1984.4 | -1898.6 | -1813.3 | -1732.1 | -1661.4 | -1605.6 | -1565.4 | -1540.2 | -1527.8 | -1525.7 | -1530.9 |
Moment Span 1 | ||||||||||||
Self weight | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 |
Superstructure | 1305.0 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 |
Cross beam | 220.0 | 64.1 | 50.2 | 38.6 | 30.1 | 24.8 | 23.1 | 24.8 | 30.1 | 38.6 | 50.2 | 64.1 |
Span | 1615.0 | 353.4 | 306.7 | 257.1 | 206.6 | 159.6 | 119.2 | 86.0 | 59.6 | 38.5 | 21.1 | 6.2 |
M= | 10774.0 | 1210.1 | 1149.5 | 1088.4 | 1029.3 | 977.0 | 934.9 | 903.5 | 882.3 | 869.7 | 864.0 | 862.9 |
Shear C0 | ||||||||||||
Self weight | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 |
Superstructure | 278.0 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 |
Cross beam | 47.0 | 13.7 | 10.7 | 8.3 | 6.4 | 5.3 | 4.9 | 5.3 | 6.4 | 8.3 | 10.7 | 13.7 |
Span | 295.0 | 64.6 | 56.6 | 47.0 | 37.7 | 29.2 | 21.8 | 15.7 | 10.9 | 7.0 | 3.9 | 1.1 |
V= | 2251.0 | 247.5 | 236.0 | 224.5 | 213.4 | 203.7 | 196.0 | 190.3 | 186.6 | 184.6 | 183.9 | 184.1 |
Shear P1, left | ||||||||||||
Self weight | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 |
Superstructure | -464.0 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 |
Cross beam | -78.8 | -22.7 | -17.8 | -13.7 | -10.7 | -8.8 | -8.2 | -8.8 | -10.7 | -13.7 | -17.8 | -22.7 |
Span | -422.0 | -92.3 | -80.1 | -67.2 | -54.0 | -41.7 | -31.2 | -22.5 | -15.6 | -10.1 | -5.5 | -1.6 |
V= | -3682.0 | -397.3 | -380.1 | -363.1 | -346.8 | -332.7 | -321.5 | -313.5 | -308.4 | -305.9 | -305.5 | -306.5 |
Abutment reaction C0 | ||||||||||||
Self weight | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 |
Superstructure | 278.0 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 |
Cross beam | 47.0 | 13.7 | 10.7 | 8.3 | 6.4 | 5.3 | 4.9 | 5.3 | 6.4 | 8.3 | 10.7 | 13.7 |
Span | 295.0 | 64.6 | 56.0 | 47.0 | 37.7 | 29.2 | 21.8 | 15.7 | 10.9 | 7.0 | 3.9 | 1.1 |
R= | 2251.0 | 247.5 | 236.0 | 224.5 | 213.4 | 203.7 | 196.0 | 190.3 | 186.6 | 184.6 | 183.9 | 184.1 |
Reaction pile P1 | ||||||||||||
Self weight | 479.0 | 479.0 | 479.0 | 479.0 | 479.0 | 479.0 | 479.0 | 479.0 | 479.0 | 479.0 | 479.0 | 479.0 |
Superstructure | 928.0 | 84.4 | 84.4 | 84.4 | 84.4 | 84.4 | 84.4 | 84.4 | 84.4 | 84.4 | 84.4 | 84.4 |
Cross beam | 156.0 | 45.5 | 35.6 | 27.4 | 21.3 | 17.6 | 16.4 | 17.6 | 21.3 | 27.4 | 35.6 | 45.5 |
Span | 844.0 | 184.7 | 160.3 | 134.3 | 108.0 | 83.4 | 62.3 | 45.0 | 31.2 | 20.1 | 11.0 | 3.2 |
R= | 7353.0 | 793.5 | 959.2 | 725.1 | 692.6 | 664.4 | 642.0 | 625.9 | 6158 | 610.9 | 610.0 | 612.1 |
SLS Max | |||||||
Support | GM | Grill1 | Grill2 | EF1 | EF2 | %1 | %2 |
101 | 247.5 | 366.5 | 373.8 | 361.3 | 365.8 | 3% | -33% |
111 | 793.5 | 1023.0 | 1028.3 | 1019.1 | 1015.3 | 1% | -22% |
201 | 236.0 | 199.3 | 197.4 | 223.6 | 215.0 | 13% | 13% |
211 | 759.2 | 763.4 | 758.9 | 804.2 | 786.4 | 6% | -2% |
301 | 224.5 | 238.4 | 238.7 | 224.7 | 223.2 | 7% | -3% |
311 | 725.1 | 751.5 | 748.6 | 743.5 | 743.5 | 1% | -3% |
401 | 213.4 | 196.3 | 195.0 | 196.2 | 197.3 | 1% | 9% |
411 | 692.6 | 652.6 | 650.7 | 645.5 | 651.3 | 1% | 7% |
501 | 203.7 | 185.3 | 183.2 | 181.3 | 183.5 | 2% | 11% |
511 | 664.4 | 611.1 | 608.4 | 598.7 | 607.1 | 2% | 10% |
601 | 196.0 | 177.0 | 175.2 | 173.8 | 176.1 | 2% | 12% |
611 | 642.0 | 587.7 | 585.2 | 575.7 | 584.7 | 2% | 10% |
701 | 190.3 | 173.1 | 171.7 | 169.7 | 172.0 | 2% | 11% |
711 | 625.9 | 575.7 | 573.8 | 564.2 | 572.9 | 2% | 9% |
801 | 186.6 | 170.7 | 170.0 | 168.3 | 170.1 | 1% | 10% |
811 | 615.8 | 569.9 | 569.0 | 561.4 | 568.8 | 2% | 9% |
901 | 184.6 | 173.7 | 173.4 | 170.0 | 170.3 | 2% | 7% |
911 | 610.9 | 576.5 | 576.1 | 569.6 | 572.4 | 1% | 6% |
1001 | 183.9 | 165.3 | 167.8 | 171.0 | 166.0 | 3% | 10% |
1011 | 610.0 | 564.2 | 568.3 | 592.6 | 583.5 | 5% | 6% |
1101 | 184.1 | 210.6 | 212.3 | 215.4 | 215.7 | 2% | -14% |
1111 | 612.1 | 691.0 | 693.1 | 690.9 | 681.8 | 2% | -11% |
max: | max: | ||||||
∑ | 9602 | 9623 | 9619 | 9621 | 9622 | 13% | 33% |
Guyon-Massonnet coefficients -> to divide by 11 | ||||||||||||
Beam | 1 | 2 | 3 | 4 | 5 | 6 | 7 | 8 | 9 | 10 | 11 | |
Y= | -4.5 | -3.6 | -2.7 | -1.8 | -0.9 | 0 | 0.9 | 1.8 | 2.7 | 3.6 | 4.5 | |
Distributed superstructure | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | 1.000 | |
Left cross beam | 3.287 | 2.523 | 1.860 | 1.317 | 0.893 | 0.577 | 0.348 | 0.186 | 0.072 | -0.013 | -0.081 | |
Right cross beam | -0.081 | -0.013 | 0.072 | 0.186 | 0.348 | 0.577 | 0.893 | 1.317 | 1.860 | 2.523 | 3.287 | |
->∑ cross beam | 3.206 | 2.510 | 1.932 | 1.503 | 1.241 | 1.154 | 1.241 | 1.503 | 1.932 | 2.510 | 3.206 | |
Q span | 2.407 | 2.089 | 1.751 | 1.407 | 1.087 | 0.812 | 0.586 | 0.406 | 0.262 | 0.144 | 0.042 | |
Support | 1.347 | 1.412 | 1.459 | 1.445 | 1.322 | 1.136 | 0.933 | 0.738 | 0.560 | 0.401 | 0.257 |
Beam | 1 | 2 | 3 | 4 | 5 | 6 | 7 | 8 | 9 | 10 | 11 | |
Moment on support | ||||||||||||
Self-weight | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 | -1198.0 |
Superstructure | -2320.0 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 | -210.9 |
Cross beam | -391.0 | -114.0 | -89.2 | -68.7 | -53.4 | -44.1 | -41.0 | -44.1 | -53.4 | -68.7 | -89.2 | -114.0 |
Span | -2109.0 | -461.5 | -400.5 | -335.7 | -269.8 | -208.4 | -155.7 | -112.4 | -77.8 | -50.2 | -27.6 | -8.1 |
M= | -18389.0 | -1984.4 | -1898.6 | -1813.3 | -1732.1 | -1661.4 | -1605.6 | -1565.4 | -1540.2 | -1527.8 | -1525.7 | -1530.9 |
Moment Span 1 | ||||||||||||
Self-weight | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 | 674.0 |
Superstructure | 1305.0 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 | 118.6 |
Cross beam | 220.0 | 64.1 | 50.2 | 38.6 | 30.1 | 24.8 | 23.1 | 24.8 | 30.1 | 38.6 | 50.2 | 64.1 |
Span | 1615.0 | 353.4 | 306.7 | 257.1 | 206.6 | 159.6 | 119.2 | 86.0 | 59.6 | 38.5 | 21.1 | 6.2 |
M= | 10774.0 | 1210.1 | 1149.5 | 1088.4 | 1029.3 | 977.0 | 934.9 | 903.5 | 882.3 | 869.7 | 864.0 | 862.9 |
Shear C0 | ||||||||||||
Self-weight | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 | 144.0 |
Superstructure | 278.0 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 | 25.3 |
Cross beam | 47.0 | 13.7 | 10.7 | 8.3 | 6.4 | 5.3 | 4.9 | 5.3 | 6.4 | 8.3 | 10.7 | 13.7 |
Span | 295.0 | 64.6 | 56.0 | 47.0 | 37.7 | 29.2 | 21.8 | 15.7 | 10.9 | 7.0 | 3.9 | 1.1 |
V= | 2251.0 | 247.5 | 236.0 | 224.5 | 213.4 | 203.7 | 196.0 | 190.3 | 186.6 | 184.6 | 183.9 | 184.1 |
Shear P1, left | ||||||||||||
Self-weight | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 | -240.0 |
Superstructure | -464.0 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 | -42.2 |
Cross beam | -78.0 | -22.7 | -17.8 | -13.7 | -10.7 | -8.8 | -8.2 | -8.8 | -10.7 | -13.7 | -17.8 | -22.7 |
Span | -422 | -92.3 | -80.1 | -67.2 | -54.0 | -41.7 | -31.2 | -22.5 | -15.6 | -10.1 | -5.5 | -1.6 |
V= | -3682.0 | -397.3 | -380.1 | -363.1 | -346.8 | -332.7 | -321.5 | -313.5 | -308.4 | -305.9 | -305.5 | -306.5 |
Mxx | Difference/BT1 | Myy | Difference/BT1 | ||
BT1 SETRA | 23.5 | 28.7 | Appendix 7 | ||
Distributed load - mesh 25x25 | |||||
Model R1, peak values | 24.2 | 2.7% | 29.0 | 1.0% | Appendix 1 |
Model R2, peak values | 23.2 | -1.3% | 28.5 | -0.6% | Appendix 3 |
Model R1, 25x25, manual smoothing for 2 hours | 23.3 | -0.7% | 28.0 | -2.4% | Appendix 1 |
Model R1, 25x25, automated smoothing for 2 hours | 23.4 | -0.3% | 28.1 | -2.3% | Appendix 2 |
Model R2, 25x25, automated smoothing for 2 hours | 22.1 | -6.2% | 27.5 | -4.5% | Appendix 3 |
Software S, quadrilateral-25x25, smoothing over 2 hours | 23.6 | 0.4% | 28.6 | -0.3% | Appendix 5 |
Software S, triangular-25x25 | 21.0 | -11.9% | 26.9 | -6.7% | Appendix 5 |
Software P, quadrilateral-25x25 | 21.6 | -9.0% | 27.4 | -4.7% | Appendix 6 |
Model R1, 25x25, manual smoothing for 4 hours | 21.9 | -7.4% | 26.7 | -7.5% | Appendix 1 |
Model R1, 25x25, automated smoothing for 4 hours | 22.0 | -7.1% | 26.7 | -7.4% | Appendix 2 |
Model R2, 25x25, automated smoothing for 4 hours | 20.9 | -12.4% | 26.2 | -9.8% | Appendix 3 |
Software S, quadrilateral-25x25, smoothing for 4 hours | 22.8 | -3.3% | 27.8 | -3.2% | Appendix 5 |
Distributed load – mesh 100x100 | |||||
Model R1, 100x100, automated smoothing for 2 hours | 21.9 | -7.3% | 27.9 | -2.7% | Appendix 2 |
Model R1, 100x100, automated smoothing for 4 hours | 20.5 | -14.5% | 26.6 | -8.0% | Appendix 2 |
Software P, 100x100 | 13.5 | -74.3% | 19.7 | -45.8% | Appendix 6 |
Point load – mesh 25x25 | |||||
Model R1 25x25 | 37.1 | 36.7% | 41.8 | 31.3% | Appendix 2 |
Model R1 25x25 | 28.1 | 16.3% | 34.9 | 17.6% | Appendix 2 |
Model S | 45.7 | 48.6% | 52.6 | 45.4% | Appendix 5 |
Model P | 28.1 | 16.4% | 34.8 | 17.6% | Appendix 6 |
Panel | Thickness | Materials | Mesh | Reinforcement | NU |
Node/Case | FX \[kN\] | FY \[kN\] | FZ \[kN\] | MX \[kNm\] | MY \[kNm\] | MZ \[kNm\] |
Case 101 | Br | |||||
Total sum | 0.0 | 0.0 | 0.0 | 0.0 | 0.0 | 0.0 |
Sum of reactions | 0.0 | 0.0 | 100.00 | 550.00 | -1000.00 | 0.0 |
Sum of efforts | 0.0 | 0.0 | -100.00 | -550.00 | 1000.00 | 0.0 |
Verification | 0.0 | 0.0 | -0.0 | -0.0 | 0.0 | 0.0 |
Precision | 6.43486e-13 | 4.51850e-24 | ||||
Case 102 | Br displaced | |||||
Total sum | 0.0 | 0.0 | 0.0 | 0.0 | 0.0 | 0.0 |
Sum of reactions | 0.0 | 0.0 | 100.00 | 550.00 | -1012.50 | 0.0 |
Sum of efforts | 0.0 | 0.0 | -100.00 | -550.00 | 1012.50 | 0.0 |
Verification | 0.0 | 0.0 | -0.0 | -0.0 | 0.0 | 0.0 |
Precision | 7.68058e-13 | 4.56828e-24 | ||||
Case 201 | Point | |||||
Total sum | 0.0 | 0.0 | 0.0 | 0.0 | 0.0 | 0.0 |
Sum of reactions | 0.0 | 0.0 | 100.00 | 550.00 | -1000.00 | 0.0 |
Sum of efforts | 0.0 | 0.0 | -100.00 | -550.00 | 1000.00 | 0.0 |
Verification | 0.0 | 0.0 | -0.0 | -0.0 | 0.0 | 0.0 |
Precision | 1.03246e-13 | 4.60955e-24 | ||||
Case 202 | Point 6 forces | |||||
Total sum | 0.0 | 0.0 | 0.0 | 0.0 | 0.0 | 0.0 |
Sum of reactions | 0.0 | 0.0 | 100.00 | 550.00 | -1012.50 | 0.0 |
Sum of efforts | 0.0 | 0.0 | -100.00 | -550.00 | 1012.50 | 0.0 |
Verification | 0.0 | 0.0 | -0.0 | -0.0 | 0.0 | 0.0 |
Precision | 4.12474e-13 | 4.63262e-24 |