PART 2 – USEFUL ELEMENTS

$translationBooks

Chapter A. Understanding the finite elements

Chapter A. Understanding the finite elements

A.1. What does a finite element software do? Example of framed structures.

A.2. Explicitly, what is a finite element?

Annex 1 – File of the matrix calculation example


$translationBooks

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

The purpose of this introduction is to show, in a simple example, what lies behind a static calculation carried out with a finite element beam software.

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.

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, [Kij][qij]=[Fij] (Figures 1 and 2), allowing the components of the vectors [Fij] to be expressed as a function of those of the vectors [qij]. [Kij] is called the stiffness matrix of the beam, [Fij] the force vector at the nodes, and [qij] the vector of nodal displacements.

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.

Figure 3 – Rotation matrix

To calculate the displacements of all the nodes, the software:

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:

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.

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.

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

Beam 2: Stiffness matrix

The transformation is applied to these two matrices to make them compatible with the global coordinate system.

Rotation matrix for α = 1.571 Rad:

And its transpose:

Rotation matrix for α = 0.197 Rad:

And its transpose:

Beam 1 - Result of the operation [K*] = [Λ]T [K] [Λ]:

Beam 2 - Result of the operation [K*] = [Λ]T [K] [Λ]:

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):

The blocked displacement components can be removed from the matrix since we already know that their value is equal to zero:

This matrix is easily inverted using the spreadsheet:

Load 1: External forces applied on a node

Figure 6 - Load definition

The nodal displacements are calculated (in the global coordinate system):

The forces in the column (beam 1) can be determined after transforming the displacements to the local coordinate system of the beam:

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).

 Figure 7 - Diagrams N, V, M - example 1

Loading 2: External forces applied to a beam (i.e. other than at the nodes).

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:

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.

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...

... and add them together with the forces of perfect clamping, with the appropriate sign convention:

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.

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).

Figure 10 - Matrix with contrasting values


$translationBooks

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.

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.

To summarize, the software calculates:

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:

Main remarks concerning common usage

Example of a load on a bridge slab illustrating the differences in results during a FE calculation.


$translationBooks

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 

B.7 Organization of the computational model


$translationBooks

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:

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...

c) In the case of a structure whose construction kinematics have an impact on the final state, the software must be able to authorize the complete simulation of the phasing, allowing, among other things, selective activation of the elements (such as the tensioning of prestressing cables and braces, for example), which makes it possible to work on the part of the structure under construction.

d) If a dynamic calculation is necessary (for example for a seismic calculation considering the effects of the soil or a vibration calculation or even a fast dynamic problem such as an explosion) not all software can be used.

e) Non-linear calculations are not systematically possible (calculation with material non-linearities, elasto-plastic supports, calculation of large second-order displacements for buckling verification, etc.).

f) Modelling of cable structures (whose transverse stiffness to bending and torsion is not very important compared to the longitudinal stiffness) is also particular and only provided by some software.

g) The determination of a thermal field (volume loading expressed from a variation in temperature and the coefficient of thermal expansion of the material) may require additional modules to the software.

h) Foundation modeling, for a foundation slab with uplifting, for instance, is generally linked to non-linear calculations and thus agrees with point d).

B.2 Depending on the study phase

The design phase of a structure has an impact on the level of precision expected from the calculations.

The table below shows the level of detail generally expected for each phase. Depending on the specificities of the project and the requirements of the customer, the content of the phases may vary:

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
B.3 Based on the verification objectives

For the same object and the same study phase, several models may have to be set up, each dealing with different verifications.

One must try to ensure that the same model can meet as many verifications as possible, but the problems often have to be decoupled.

B.4 Based on the expected results

The choices can be influenced by the results different software can handle. 

a) Integrated post-processing modules make some software interesting, in particular those that allow the rebars of reinforced concrete sections to be obtained from stresses, or those that incorporate the verification of steel profiles when buckling or the verification of conventional connections. Beforehand, it is essential to check the conformity of the post-treatment with the reference regulations of the project.

b) The types of output results can vary and be relatively adaptable (listings, stress diagrams, maps, combination envelopes with or without conservation of concomitances).

B.5 Depending on time and resources

In terms of deadlines, and therefore budget, a distinction must be made between the modeling time (geometry, loads, combinations, etc.), the calculation time, the time to set-up (debugging errors, verifying support conditions, etc.), and finally the analysis time. These durations can vary significantly depending on the software because their user interface is less intuitive (the design interface can be either graphical or programmable in a command window or using spreadsheets). The extraction of results is not necessarily instantaneous and can be useful to identify critical points.

Moreover, the resources available within the design office guide the choice of the type of calculation: the hardware, on which the software is installed, must be open, so does the user license, so that it can be easily handed over to another user. The availability schedule of the tools can play an important role in deadlines and possibly lead to a change of software.

If the design office has a type of hardware with reduced capacity, the degree of complexity of the calculations is reduced accordingly. And if the complicated computational model is kept, the design office should not "tinker" a model adapted to the capacity of its equipment, because the simplifications adopted can then lead to issues concerning the accuracy of the results. It is then in the design office's best interest to subcontract the calculation.

For large structures, it may be preferable to implement two levels of modeling, using sub-models. Indeed, a single model can quickly become disproportional in size, and therefore difficult to structure and manipulate. However, it is necessary to be able to link the models together. Furthermore, the need for specific computing capabilities can also lead to the splitting of models and the use of different software.

Another reason for splitting the models as described above can be linked to the study schedule (a consequence of the organization of the projects): the calculation of the whole work sometimes precedes by several months, for important projects, the calculation of certain parts of the work. There are no reasons not to compensate by post-processing for certain shortcomings of the software, by extracting the results of a sub-model and to process them manually or using another software.

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.


$translationBooks

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 :

The model must be based on input data, with at least:

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.

  1. 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.

  1. Specifics of the study

All the specifics of the study must be listed at the beginning of the study:

It is necessary to show that the modeling will consider all these points.

  1. Planning of the study

It must clearly show:

  1. Modelling Principles

The goal is to explain the calculation methods, making sure to:

 

$translationBooks

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

C.2 Modelling of the main elements

C.3 Finite elements and meshing

C.4 Modelling of the non-structural elements or the equipment

C.5 Boundary conditions

C.6 Connections – links – assembly 

C.7 Eccentricity 

C.8 Combined cross-sections (beam/deck)

C.9 Materials

C.10 Behaviors specific to shear and torsion

C.11 Loads modeling

C.12 Further information related to volumetric elements 

C.13 Further information related to non-linear calculations

C.14 Further information related to prestress 

C.15 Further information related to phase calculation

C.16 Further information related to structural dynamics and seismic calculations


$translationBooks

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.

(*) 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).

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.


$translationBooks

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:

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:

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:

Example of a structure with close openings... which clearly cannot be neglected.

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:

To establish an order of magnitude, a structure can be considered as being of low sensitivity:

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, ...).

Illustration of the angle between two supports

The example of a girder grid "Modelling the same structure using different approaches" (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:

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):


C.2.5 The use of symmetries

As discussed in Part 1 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):

Symmetrical load case: 

In this case, the results are identical for both structures.

Case of asymmetrical loading: 

In this case, there is a significant difference in the results:

The examination of the bending moment influence lines on the second support in both configurations provides an immediate explanation:


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).

Because of its shape, it contains planes of symmetry. The following plane of symmetry was chosen as shown in the figure below:

The foundation slab can then be subjected to a loading that is either symmetrical or antisymmetrical.

For example:

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:

In the second case (antisymmetric loading), the nodes located on the plane will be:

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.


© doc Plaxis

Even 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:

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:

In this case:

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:

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).

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


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.

Global modeling with beam elements (pseudo-volumetric view)

Local modeling with plate elements (view of average surfaces)


$translationBooks

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 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:

C.3.2 Mesh shape

The first part of this guide (Part 1 § A.3) 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.

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.

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.

             Surface creation order                                                       1st mesh

Elementary surface modelling = Non-regular mesh + degenerate elements

           Adjustment of the geometry                                                2nd mesh

Improved surface modeling + controlled mesh = Meshing and satisfying elements


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:


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).

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.


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:


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.

View of the local coordinate systems of the elements

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:

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:

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.

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):

By refining the mesh, the graphs become:

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:

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. 

Integral of the shear efforts - plate with two single support lines

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%)

Integral of the bending moment - bi-clamped plate


$translationBooks

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:

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

For seismic analyses, it is important to ensure that the element will not resonate with the supporting structure. The following publications are useful references to identify when the element/structure interaction should be considered in the model.

AFPS proposal to know when to consider the dynamic interaction between non-structural elements/equipment and the structure (Recommendations AFPS90, 1993).

Legend :

Note: depending on the direction studied, the mass of the supporting structure may be limited to the support floor only (for more details, refer to the documents mentioned above).

For seismic calculations of buildings, non-structural elements (such as partition walls) must be considered when modeling the structure as they are likely to modify its transverse stiffness. These elements may be subjected to justifications such as in EC8-1, Article 4.3.6 for framing with masonry infill.

It may also be necessary to remove small elements in a model intended for modal analysis.

 

$translationBooks

C5. Boundary Conditions

C5. Boundary Conditions

C.5.1 General case

The boundary conditions are determined by the degrees of freedom that can be fixed or not at the nodes located at the boundaries of the structure (supports, cuts ...).

The notions of reference frames and boundary conditions are closely related here. The orientation of a boundary condition (forces, moments, imposed displacements, accelerations...) will depend on the orientation of the current reference frame when it is implemented or on the entity (node, element) upon which it is applied.

In what concerns the coordinate systems, a distinction must be made between the ones linked to elements and the ones linked to the nodes.

Usually, by default, the node coordinate systems are identical to the global coordinate system. However, a different coordinate system can be assigned to one or several nodes in order to be able apply a boundary condition to the node(s) in a particular orientation. Simple graphical controls of the orientation of nodal loads (forces, moments, imposed displacements) enable visualizing the correct definition of these nodal coordinate systems.

For the elements, the local coordinate systems are generally linked to the main orientations defined during the creation of the element. Simple graphical controls of the orientation of the loads applied to the elements (such as pressure) allow visualizing the good definition of these element systems.

The boundary conditions must ensure the stability of the structure with respect to the loads applied and be representative of its overall behavior. Stability must systematically be reached in the 6 global components X, Y, Z, RX, RY, and RZ, even if the loads are applied only to a few directions.

Stability following a translation is always achieved by blocking at least one node in the direction of this translation.

Stability about an axis is achieved either by fixing one node in rotation (along the axis of rotation) or by blocking two nodes in translation in a plane perpendicular to the rotation.

It is important to check that the reactions in the fixed directions are zero in order to have numerical stability.

Example:

Objective: loading of a slab supported by 4 columns ;

Summary:

We will check that at the nodes following UX and UY, the RX and RY reactions are zero.

Example of the minimum stability of a Z-loaded slab

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:

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, ...).

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:


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.

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.

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.

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).

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.

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.

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.

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.

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.

Geometry

Unitary results (1kN or 1kN.m) introduced

Results:

Displacements under the loads = flexibility matrix [S]

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:

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.

Illustration of the complexity of the constitutive law of soil springs

C.5.3 Modeling of support devices

There are two ways to model the support devices of a structure:

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.


Example of a bridge pile model including the elastomeric bearings.

If bar elements are used, there are several possible choices:

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.

Modeling details of a pile supporting two isostatic spans

 

$translationBooks

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).

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).

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:

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.

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).

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).

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.

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:

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:

Unfortunately, the numerical computations converge, but ... several aspects of the results can and should attract the attention of the modeler:

It is enough to create an embedment using (fictitious) bars at the foot of the column, in the slab ...

... to obtain accurate overall results. (The local efforts at the foot of the column are of course disturbed by these fictive bars).


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.

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.

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

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:

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.

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.

The global model with simplified modeling of a girder in an extremity.

A detailed local model of the abutment box


$translationBooks

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:

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 Example of Prestressing and Offsets.

Illustration of the offset of a series of beam elements with respect to a horizontal upper surface.

 

$translationBooks

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:

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:

C.8.1.2 How to model the beam/slab floor

The first aspect concerns the floor modeling method. Indeed, several options are available:

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.

Plan view of the slab

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 study 1: modeling the beams only - the slab is not modeled

Modeling scheme

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

Modeling scheme

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.

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

Modeling scheme

Bending moment diagram (kN.m) in the beam

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!!!

Longitudinal bending moments in the slab

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.

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.

This example shows that:

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...):

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:

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...

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).

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:


Beam grid model

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.

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): 


Bending moments (only the drop-beams) - kN.m


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:

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: 

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:

→ 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.

Mapping of the reinforcement in the upper fiber of the slab

Reinforcement in the upper fiber of the slab at the central support, central beam (18.36cm² along 2m)

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: 

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:

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):

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):

The use of software specifically developed for mixed calculations is always recommended whenever possible.

See in Part 3, example B - Mixed and Steel Beams.


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.

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 ...

The blue distribution surfaces are meshed like slabs but do not contribute to the strength of the structure.

Plan view of the floor with the load-bearing direction of the steel deck

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:

Mixed floor without slab modeling - Bracing provided by the profiles


Bracing provided by the slab


$translationBooks

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.

$translationBooks

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:

 

Comparing calculations of the angle of rotation of a cantilever I-beam

 

Data - cantilever beam:

Plate element model: 

Loading: 

Reaction: 

Displacement θ(L)=0.042 rad

Beam-element model 

Loading:

Reaction: 

Displacement θ(L)=0.1198 rad

Analytical calculation

The differential equation for the angle of rotation is given by:

With the boundary conditions given in the previous paragraph, the solution of this equation is:

With:

Application:

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:

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.

 

$translationBooks

C11. Modeling the loading

C11. Modeling the loading

As explained in chapter E, 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

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

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:

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


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”) ...

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:

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:

At mid-span 1, one gets |V|max = 31.3 kN: 

The diagram below shows the same shear diagram, but with a beam loaded according to the IL:

One gets |V|max = 53.7 kN, which is a significant difference. 

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:

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:

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:

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:

Trucks very close to one another, envelope, and unfavorable position.

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:


Loading according to the IL:

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").


$translationBooks

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:


(Taken from Part 3 - Example C - Modeling of girder grids).

$translationBooks

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:

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

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.

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.

Modal 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.

- Instabilité par flambement des arcs (CTICM) - Lien vers l'article.

$translationBooks

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. 

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 

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: 

(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=∞).

HA 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.

Converted to loading on the beam:

The resulting shear efforts, i.e. the shear efforts considering the hyperstaticity of the system:

The bending moment:

For control purposes, we can:

“Isostatic" shear effort diagram:

“Isostatic" bending moment diagram (the curve divided by HA is the rope path):

It should be ensured that the support reactions in the "isostatic" prestressed load case are equal to zero: 

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.

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.

At the anchor A, the rope applies to node n1 of the model the loads (HA, VA, MA), MA being the moment produced by HA 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.

 

$translationBooks

C15. More about phased calculations

C15. More about phased calculations

The reader may also refer to Part 1 - D.3 Construction Phases.

Structural phasing can lead to modification:

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, ...).

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).

Accumulation of the loadings

Phase 1: Loading the structure with a temporary support

Phase 2: Removal of the temporary support

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).

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:

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.

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) :

Vertical translation for the Z-correspondence of the lips

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".

$translationBooks

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

 

Overview of the corner block model

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.

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.

 

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.

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.

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.

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:

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:

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

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:

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:

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. 

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.

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.

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:

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.

 

$translationBooks

Chapter D. Analysis and processing of the results 

Chapter D. Analysis and processing of the results 

D.1 General information about numerical calculations

D.2 Load combinations

D.3 Results processing 

D.4 Validation rules: the behavior of concrete elements

D.5 Understanding and analyzing the peaks (case study about concrete)

D.6 Understanding and analyzing the peaks (case study about steel assembly)

D.7 Further information specific to dynamic calculations


$translationBooks

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.

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.

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 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 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:

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.

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.

These problems of global and local instabilities can be detected by performing simple calculations:

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.


$translationBooks

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.

Illustration of the structure

The following two unit cases are defined:

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...

Results of the unit cases: bending moments - gravity loads (left) and water pressure loads (right)

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) ...

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:

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.


$translationBooks

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:

D.3.2 Values at nodes, Gauss point values or values at the center

See also A.2 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, 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:

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). The software used does not give access to the values at the Gauss points.

Mapping of transverse bending moments - values at the center of the slabs - overview (28.52kN.m/m is an extreme calculation value)

Values at node 3 - they are different depending on the finite element

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 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.


$translationBooks

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:

The first step is to calculate the following intermediate stresses:

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.

Horizontal bending moments MYY | Bending moments MXY

Ay reinforcement is calculated manually with fyd=200MPa (SLS).

 Ay manual = 10 x (MYY + MXY)/(0.9 x 0.17 x 200) cm²

Values that can be compared with the reinforcement areas calculated by the software:

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 Mxx and Myy 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:

Taking into consideration the previous calculations of reinforcement distribution, this gives:

Hence the reinforcement:

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.


Stresses Nxx (horizontal) (kN/m) – Stresses Nyy (vertical) (kN/m)

Stresses Nxy (shear) - Reinforcement mapping (cm²/m²) for one layer

The steel sections are calculated manually and compared with the map values.

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:

Hence the bending reinforcement: A-tension = 10 000 /(0.9 x 3.9 x 50) = 57 cm2 or 29cm2 per layer.

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.

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:

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.

Visualization of horizontal efforts Fxx

Calculation of reinforcement with reinforcement mappings:

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).

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.

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:

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:

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:

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.

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.

Principal stresses S2 (compressions)

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:

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:

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).

Load path in a wall-beam with multiple openings, S1 stresses

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.

 

$translationBooks

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.

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?

Slab of 3 m articulated span subjected to a concentrated load of 10 KN at its center (node stresses)

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.

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.

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.

  1. Unsmoothed efforts on the elements

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.

  1. Smoothed efforts on the elements

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.

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.

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?

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

D.5.2.1 First analysis: geometrical

Experience shows that 90% of the peaks are located at the level of geometric singularities (columns, supports, wall/wall or wall/slab intersections, etc.). This is due to the fact that the modeling, carried out from middle planes or middle fibers, does not represent the elements with their real volumetric geometry (for example, a slab is represented by a plane element and the columns on which it rests, by wire elements). In a pictorial way, this leads, as explained in D.5.1, to taking into account forces applied to null surfaces, thus inevitably leading to numerical problems. It is therefore essential to identify these singularities on the model.

  1. Examples of peaks related to geometry

Below we share an example of a slab on a column/beam array grid for which moment peaks appear at the supports formed by the columns.

These peaks must be interpreted in detail, it is possible to reduce the values of the dimensioning moments by limiting the maximum demandclipping at the beams.

Example of a slab on a grid n array of columns and beams

Visualization of bending moments in the slab

Peaks appears; they can be limited clipped at the beams:

In the above case, conventional clipping is performed in the plane of the edges of the beams or column in the case of a flat slab on headed columns.

Some types of software allow to define supports with plan dimensions to directly obtain the efforts in the plane. Example of a 10×10 m² slab, 30 cm thick, subjected to its self-weight, supported linearly on an edge and on two point supports in line with two posts 1 m from each corner. The left support is a classic point support, the right support is a column type support of 50×50 cm².

The representation of efforts with and without reduction of effort shows a significant difference in values.

Note: It is always advisable to check the methodology used by the software and to ensure that it is compatible with the regulatory justifications to be carried out.

  1. Peaks caused by point forces

The peak treatment at concentrated loads is similar to the peaks caused by point links. (A force or torsor can represent the effects of point support; there is a strict equivalence).

Example:

We take the trivial example of a load arriving via a column on a wall (30 cm thick wall, 55×30 cm² column).

Depending on what we want to calculate, the approach will not be the same. If we are looking for a global vertical load calculation, the approaches on the left, either via a point load or via a wire bar are perfectly suitable. However, if we are interested in local effects, it is absolutely necessary to use a distributed load to minimize the stress peak, which does not facilitate automated calculations (and does not anticipate other manual calculations to be performed: diffusion, punching ...).

Peak related to the way of modeling of a load on a slab: case of a wheel load on a bridge slab.

A concentrated load which is perpendicular to a slab generates a moment peak (see D.5.1). This peak must be processed to calculate the reinforcement. It can be reduced by replacing the concentrated load by a loading block that takes into account the diffusion of the load in the slab (diffusion of a wheel on a bridge slab).

Example:

The longitudinal moment for the same 100 kN load is compared using four approaches:

100 kN force in the center of a mesh → Mx=26.62 kN.m/m

100 kN force on a node → Mx=48.12 kN.m/m

Distributed pressure on a mesh → Mx=26.62 kN.m/m

1/4 force on 4 nodes → Mx=26.62 kN.m/m

In conclusion, we realize that modeling a distributed load by a point force can be very detrimental, especially if this load is applied to a node of the mesh: it is better to use pressure (knowing that the software distributes the loads to the nodes), or alternatively to split the force into several loads to avoid the potential peak force.

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:

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.

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:

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.

The observation of the deformation should also alert us:

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:

To illustrate this, the table below summarizes the consequences on the reinforcement of each stress component:

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.

Theoretical moments are -11.2 kN.m on supports and 6.3 kN.m in span.

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:

Moment Clipping at the plane of the supports = -10.6 kN.m

The moment in the center of the mesh will then represent the moment at the plane of the support.

The same type of reflection and approach is to be carried out in order to reduce the transverse shear effort, if necessary.

  1. 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:

Firstly, a wireframe model is used to calculate the moments at the central support (truncated view):

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).

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:

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:

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

For out-of-plane concentrated loads, the distance of the load from the support and its diffusion must also be taken into account.

Reinforcement peaks are frequently located at the edge of the shaft, in which case the redistribution of forces can only be in one direction and therefore over limited widths:

In the case of small openings (sleeves in particular) that fit into the reinforcement mesh or cause the interruption of a single reinforcement, it is possible to dispense with additional reinforcement.

Proposed rule for smoothing longitudinal reinforcement peaks in membrane elements (walls)

For elements subjected to tensile membrane stresses, redistribution can only take place in one direction.

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

In bracing walls subjected to an axial bending moment perpendicular to the wall plane, the tensile membrane stress varies linearly.

When smoothing the reinforcement peaks, the smoothed reinforcement must be extended over a length large enough to maintain the bending capacity: F1 x d1 > F0 x d0, where:

For elements subjected to membrane shear, it is possible to transfer part of the required section AX to section AY, if it is overabundant and vice versa. The Capra Maury method, which optimizes the sum of the reinforcement sections AX + AY, is used in common software.

The AY cross-section can sometimes be determined by the minimum reinforcement condition and the expected AY cross-section is then bigger than the required AY cross-section from the strength calculation, thus allowing a redistribution of reinforcement cross-sections. The strength of the section should then be checked with the new reinforcement sections.

Conclusion concerning the smoothing of longitudinal reinforcement peaks

In all cases, it is necessary to take into account the origin of the steel requirements by analyzing the stresses (Nxx, Nyy, Nxy, Mxx, Myy, Mxy) and to interpret the results case-by-case, with a concrete approach.

In general, the wall reinforcement comes mainly from membrane forces (Nxx,Nyy,Nxy), the bending forces (Mxx,Myy,Mxy) being then negligible. On the other hand, floor reinforcement is mainly due to bending forces (Mxx,Myy,Mxy), and in some cases by membrane forces (Nxx,Nyy,Nxy) when the building is subjected to horizontal forces (wind, earthquake) or irregularities (wall beams).

A wall beam is a good example of an irregularity producing horizontal forces in floors: the following example is based on the wall beam resting on 2 columns studied in chapter D.4.5, but with a lower floor; the tensile stresses in red show that the bottom tie is formed not only at the base of the wall but also in the lower floor:

A wall beam is a good example of an irregularity producing horizontal forces in floors: the following example is based on the wall beam resting on 2 columns studied in chapter D.4.5, but with a lower floor; the tensile stresses shown in red show that the bottom tie rod is formed not only at the base of the wall but also in the lower floor:

Tractions are even more important (here +50%) in the case of openings at the wall base:

Proposed rule for smoothing shear reinforcement peaks (the shear being perpendicular to the elements)

Generally, peaks in shear forces which are perpendicular to the elements occur at the intersection of several plates.

Reinforcements shear stress peaks often occur when shear stress is concomitant with high traction.

As a reminder, for the justification of reinforced concrete, the concomitance of a shear force with a traction requires particular attention because it means that there is no compression strut formation in the concrete and therefore a risk of breakage.

The resolution of this type of peak requires to look back at the stresses, to average the shear and normal stresses and to recalculate the reinforcement.

Approach illustrations:

Example 1:

Example 2:

The reinforcement peaks read on the charts are smoothed according to the following principle:

Smoothing principle of the local peaks of longitudinal reinforcement

Smoothing principle of the local peaks of longitudinal reinforcement

Smoothing principle of the local peaks of transverse reinforcement

 

D.5.5 Stress distribution in beams and slabs

 

It is important to remember that, with few exceptions, the calculation of the internal forces in the elements is a linear elastic calculation with a constant concrete modulus.

Peak stresses often determine a cracking of the reinforced concrete section and thus a local reduction of the peak stresses and a redistribution of the stresses.

It is sometimes useful - and it is accepted - to redistribute bending moments. A distinction must be made between:

However, it should be noted that the professional recommendations for the application of standard NF EN 1992-1-1 (NF P 18-711-1) authorize, for buildings, to use in the SLS, a moment redistribution with the same redistribution coefficients as in the ULS.

Within the Eurocodes, the ratio δ of the moment after redistribution to the elastic bending moment must be greater than or equal to 0.7 for class A longitudinal reinforcement and 0.8 for class B or C.

This redistribution of moments in a continuous beam is possible if the beam does not participate in the bracing. It is more delicate if the beam belongs to a portal frame (beware of the elastic moments coming from the portal frame effect).

We must not forget to take into account the impact of the redistribution of bending moments on shear forces.

 

$translationBooks

D6. Understanding and analyzing the peaks (case study about steel assembly)

D6. Understanding and analyzing the peaks (case study about steel assembly)

The results of a calculation performed on a surface finite element model (plate or shell type elements) may present stress peaks (or singularities). The presence of stress peaks is not annoying if they are located in areas out of interest with respect to the objectives of the study and if their presence is justified.

It should be kept in mind that a stress peak, i.e. a very high stress, must concern two or three nodes, or even a single node at most (but the structure may nevertheless present several stress peaks).

When dimensioning an assembly of plates which are welded together (metal bridge box at a support for example), the realization of a finite element model is necessary to correctly take into account the diffusion of stresses. And of course, from the same model, the stresses in the plates can be extracted to proceed to the dimensioning of the assembly of these plates.

Nevertheless, the general idea will remain to always keep a critical eye on the results obtained. They will have to be analyzed properly before they can be considered reliable with regard to the objectives of the study carried out.

This analysis of the reliability of the results often comes up against the interpretation of the possible presence of stress peaks.

The purpose of this paragraph is to give clues to help the modeler who is responsible for assessing whether or not a stress peak is a problem.

The appearance of stress peaks can have different origins, of which the main ones are:

D.6.1 Modeling – Details

Before embarking on the surface modeling of a metal plate assembly, it is essential to know and master the software's CAD tools and its meshing capabilities.

It is customary when creating geometry to neglect certain details. Two cases among others:

Note 1: The modeling of a connecting fillet will no longer create a stress peak, but a simple stress concentration. Stress concentration charts are based on this type of modeling.

Note 2: In fracture mechanics, the crack model characterized by a zero angle is a special case used to model crack propagation which is based on the notion of stress intensity factor.

Transverse stiffeners - the main beams of a bridge require transverse stiffeners at the support zones. The modeling of these stiffeners is often necessary in view of the forces that can transit in this zone and locally stress the web. According to the bridge’s rules, these stiffeners have a particular geometry and too often this geometry is oversimplified during the modeling process;

Real geometry / Simplified geometry

The stress transition may not be affected, but the mesh of the stiffener will have to be controlled so as not to end up with degenerated elements that can create singularities. And at the tip of the stiffener, a stress peak may appear which in case of misinterpretation may lead to false conclusions. See also § C.3;

Details such as connecting fillets, mouse holes, chamfers, etc. may therefore not be modeled if they are located outside an area of interest. The time spent modeling details may not be negligible, but if the objective of the simulation is to calculate a stress or a deformation in an area with such details, it is essential to model them and, moreover, to associate a representative mesh to them.

Non-representative mesh / Representative mesh

In the absence of detailed blueprints of the constructive details to be modeled, we will rely on the constructive provisions and bridges rules, which, in terms of metal assemblies (connecting fillets, local plates, stiffeners, etc.), provide a basis generally leading to a satisfactory diffusion of efforts. For example, the Commission for the standardization of metallic and mixed construction  (CNC2M) recommendations for the dimensioning of steel beams with openings in the web according to NF EN 1993 specify that, for a rectangular opening, the radius of the connecting fillets must be bigger or equal to twice the web thickness without being smaller than 15 mm, or that an isolated opening with a maximum dimension less than 10% of the web height of the beam is not considered significant (this opening must nevertheless be taken into account when checking the section).

In some cases, the consideration of details cannot be neglected (see also § C.2.2). For example, during a fatigue verification of the connections of an orthotropic slab, simplified calculation models described in the design regulations may be used. However, these models are safe and, if the fatigue strength is not justified with these simplified approaches, two possibilities are available for the designer:

In order to take into account the vehicle traffic effects (longitudinal and transverse effects, influence lines), it may be necessary to model a fairly substantial length of the structure. On the other hand, the detail modeling zone may be limited.

D.6.2 Modeling - Surface model creation and meshing

It is also important to have a good understanding of the software's meshing possibilities. Most types of software can automatically mesh a plate assembly.

The user's intervention can then be limited to the definition of a few parameters such as the average size of the elements or their shape (quadrangular, triangular). It is better, however, to be able to control the mesh by choosing the order of the surfaces to be meshed, by imposing finer mesh sizes in some zones, in order to avoid the presence of degenerated elements.

Example of degenerated mesh

In a complex assembly, due to the shape and number of parts assembled, the risk of mesh inconsistencies is high. To reduce this risk, several points should be considered, as a reminder:

Elementary surface decomposition of an I-beam

Example of panels with deformed surfaces

D.6.3 Modeling - Loading and boundary conditions

One of the frequent causes of the appearance of stress peaks is the presence of point loads or point blockages.

If a point load (respectively a point support) put in place is outside the area of interest, the presence of a stress peak is not annoying. On the other hand, if it is in the area of interest, rather than a point force, it is better to apply the force on several nodes (respectively block several nodes).

As described in the previous chapters, in reality, point forces and point supports do not make physical sense (note, however, that in a wire beam model, point supports do not create peaks).

Practical application:

Let us consider a HEB beam modeled in plate elements. A stress peak would appear, if the stress torsor in a section was applied at a node. It is better to get closer to reality, by transforming the stress torsor into normal and tangent stresses (as linear forces, if any) and proceed as follows:

Normal force / Shear force / Bending moment

The same will be done to model the beam supports. Let us consider the two following cases:

1st case - boundary conditions/longitudinal iso-stresses (in MPa) - the peak stress area is circled

2nd case: in each extremity the vertical and transversal blocking of the nodes of a web part is performed in order to get closer to reality.

2nd case - boundary conditions / longitudinal iso-stresses (in MPa)

The stress peaks appearing in the 1st case are thus due to the presence of a point nodal reaction. However, by observing the results only on the central part of the beam, we find identical results to those of the 2nd case.

1st case - central part - longitudinal iso-stresses (in MPa)

bi-supported beam (supports under the bottom flange) subjected to a distributed load. First, only the beam (type H) is modeled and boundary conditions are applied such that, near each of the two ends, the nodes of the bottom flange are blocked in the vertical direction.

Case without stiffeners - boundary conditions / Longitudinal Iso-stresses (in MPa)

Case without stiffeners - vertical iso-stresses (in MPa)

Stress peaks appear at the lower flange/web intersection despite the fact that vertical blocking was performed on several nodes. The problem here is more of a design problem. It is common practice to install transverse stiffeners perpendicularly to the supports (see design regulations for the transverse force resistance of the beam web and checks for local buckling). If we take the model by adding transverse stiffeners perpendicularly the supports, the peak stresses perpendicular to the supports disappear.

Case with stiffeners - boundary conditions / longitudinal iso-stresses (in MPa)

The stress peaks appearing in the absence of stiffeners are therefore due to a design problem. However, if we observe the results only on the central part of the beam, we find similar results to the case with stiffeners.

Cases without stiffeners - central part - longitudinal iso-stresses (in MPa)

D.6.4 Results analysis - Model validation

Once the modeling is complete, having best followed the advice given above, the calculation is executed. It is necessary to carefully analyze all the messages that can be generated by the software. Usually, an error message will block the solver, unlike warning messages, which must be carefully analyzed and interpreted. It is recommended not to ignore these messages without having carefully evaluated the possible consequences, even if it means calling the editor's hotline.

It is important to understand the possibilities offered by the software for the display and the types of results. The following is a non-exhaustive list of parameters that should be considered:

In the example below, stresses well above the elastic limit appear on localized peaks.

Example of a scale not adapted to a stress analysis

An upper bounding of the scale, possible with a lot of software, makes it possible to show the areas impacted by overruns:

Scale bounding 

The software's operating parameters being well understood, before any exploitation of the results and analysis of possible remaining stress peaks, it is advisable to carry out some simple checks to validate the calculation model:

Finally, these are the fundamental checks that must be done for any finite element modeling (see § E.2 Self-checking).

D.6.5 Results analysis - Acceptance of residual peak stresses

As mentioned above, it is possible to use a model with stress peaks if we are certain that these peaks do not disturb the outcome of the objectives of the study. In any case, it is up to the engineer to evaluate whether or not a stress peak is disturbing or not, using his or her experience and critical thinking.

The implementation of connecting fillets or local stiffeners is intended, among other things, to ensure a better diffusion of efforts. The constructive provisions and the bridges regulations in terms of metal assemblies are in accordance with this.

Therefore, the non-modeling of a constructive detail will probably result in a stress peak.

However, the modeling of the constructive detail does not exempt us from the presence of a stress concentration all the stronger that the mesh of the local area of the detail is thick. Sensitivity tests on the size of the elements can be performed in order to get a good understanding of the displayed results. Stress concentration charts can also be useful.

Examples of stress concentrations at singularity level

Stress concentrations peaking at values above the elastic limit of the material may be acceptable at the ULS if they are very localized and in facesheets. However, their justification may sometimes require an elasto-plastic calculation, especially if the area of stress exceeding the elastic limit is transverse (risk of plastic hinges). If the software allows it, this elasto-plastic calculation is performed considering a bi-linear behavior law of the material. Appendix C (informative) of EN 1993-1-5 authorizes a limit value of the maximum deformation of 5% for the zones in tension. For areas in compression, it is advisable to remain vigilant with regard to local warping phenomena.

The meshing of the areas of interest must be adapted to the fields of expected stresses or deformations.

If the mesh is poorly adapted with, for example, abrupt changes in size, stress jumps from one element to another are to be feared. Faulty discretization will result in significant discrepancies between simulation results and reality. These discrepancies can be reduced by carrying out a sensitivity study of the mesh: the mesh is considered satisfactory when the refinement leads to a small variation of the result; for example, a variation of less than 5% for element sizes divided by 2). But be careful, it is not because a result seems to have stabilized at 5% that we approach the reality at 5%.

It is not necessary to refine the mesh over the entire model. Most of the software allows to display error maps to locate areas with high stress jump. Some software even allows to automatically correct the mesh to reduce these deviations (adaptive mesh).

We have previously presented the effects of the implementation of a punctual effort or blockage.

However, even if care has been taken to distribute the load over several nodes, stress concentrations may occur with maximum values above the elastic limit of the material. This situation may nevertheless be quite acceptable depending on the purpose of the study and modeling. Take the case, for example, of the modeling of the attachment zone of a suspender cable. The stress from the suspender is distributed sinusoidally over the nodes of half the circumference of the bore (hole).

We obtain a stress concentration around the axis bores with a maximum value of 558 MPa, a value well above the elastic limit of 400 MPa. However, this maximum value is not to be compared with the elastic limit. The stress concentration here is due to the diametral pressure and the regulations indicate that the diametral pressure resistance of the plate is equal to 1.5.t.d.fy. Since the thickness t of the coping and the bore diameter d are taken into account in the modeling, 558 MPa should be compared to 1.5 x 400 = 600 MPa.

D.6.6 Synthesis

If the stress peaks are due to singularities (reflex angle, interface between two different materials, point loads), they can be neglected ... if the state of stress in the proximity of the singularity is not part of the objectives of the FE study. Otherwise, it is necessary to improve the modeling (by replacing the reflex angle by a connecting fillet, replacing the zone of discontinuity between behavior laws of different materials by a transition zone in which the parameters vary continuously, replacing 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 do a successive mesh refinement of these areas to know the more realistic stress level.

As far as smoothing is concerned, there is no simple and direct method. The reader will be able to look at what is practiced for fatigue calculations, in the case of a large stress gradient in the weld proximity in connections, with the application of the hot-spot geometrical stress method (see bibliography (ref. Hobbacher)).

Concerning the value of the maximum stress obtained, it must be compared to the limit value specified by the Calculation Standards. For steels, the Eurocodes standards define the value of the elastic limit according to the grade of steel and the thickness of the plate or tube; for example, for a tube in S355 steel with a thickness of 35 mm → elastic limit = 345 MPa according to EN 10210.

Any exceeding of this limit:

Finally, it should be remembered that an FE calculation (unless certain very specific calculation options are activated) does not take into account phenomena other than shear lag, for example instability phenomena such as warping and plate buckling.

Numerical application: Illustration of chapter D.6 - Peaks in angles, mesh incidence and fillet incidence. Link to the file.

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):

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.

  1. 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.

Zoom - Von Mises stress in the angle:

Refinement x2:

Refinement x2:

Refinement x2:

Refinement x2:

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

The curve below gives the evolution of the stress peak according to the mesh thinness.

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.

Base mesh 10x10 mm²:

Refinement x2:

Refinement x2:

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:

Let us assume that we have an elastic limit at 440 MPa, filtering at 440 MPa:

(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.

  1. 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.



$translationBooks

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:

Three cases are studied:

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

It is therefore important to take into account all significant modes otherwise the calculation efforts could be significantly underestimated.

 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.

Looking at the modal deformations, we realize that these are modes with anti-symmetric deformations:

Modal deformation - mode 1

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:

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.

 Trap: Torsional modes

Example of a building in torsion

Generally, common buildings have a torsional mode. On the example below, we can observe:

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


D.7.3 Verification of the main eigenfrequencies

In order to verify the effective behavior of the structure in dynamics, it must be ensured that the main eigenfrequencies of the structure have a coherent rough estimate.

These frequencies correspond to the main modes of bending, torsion, shear, and they generally correspond to modes with important participation factors and participating masses.

It should nonetheless be noted that limiting to modes with a significant participation factor is not an exhaustive guarantee of the modes that may be problematic under dynamic loading. Indeed, participation factors can be calculated by software based on signed modal displacements. Thus, it may happen that the participation factors taking into account the accumulation of values return low values when the mode is important.

This can happen, for example, for a continuous beam on three identical supports with two identical spans. The main mode of bending of this beam is the bending of one span in one direction and the bending of the other span in the other direction (wave form). The participation factor of this mode can be very small, as the displacements of one span counterbalance the displacements of the other span in the calculation, whereas this mode is the main bending mode of the structure, and can be the one giving the highest acceleration response if the structure is subjected to periodic excitation.

When the structure is complex, the dynamics formulas given in the literature do not allow to find precisely the eigenfrequency values obtained, since these formulas concern simple structures (eigenfrequency of an isostatic beam on two supports, of a cantilever beam, of a fixed end beam or an oscillator with a few degrees of freedom). However, these classical formulas allow to estimate the rough estimate of the main eigenfrequencies by estimating in a simplified way the behavior of the structure to reduce it to simple functioning for verification.

In the case of a beam type structure, we can thus estimate the eigenfrequencies of bending from the classical formulas. For example, and in a very general way, the eigenfrequency of bending of a beam on two supports with rotational flexibility will be between the eigenfrequency of bending of the same beam but on hinged supports and the eigenfrequency of bending of the same beam on fixed supports.

D.7.4 Modal/spectral dynamic seismic calculations

D.7.4.1 Verification of the first modes' relevance (instabilities, displacements)

The first 2 or 3 global modes visualize the functioning of the structure, which allows on the one hand to understand how it works, and on the other hand to identify modeling problems.

For a well-dimensioned building, the first 2 modes are always according to X and Y, the third mode is a torsional mode.

For common buildings, the fundamental period is of the order of 1/25 to 1/16 of the number of floors.

D.7.4.2 Verification of the global X and Y axes with respect to the first modes

It is necessary to verify that the seismic directions studied X and Y are aligned according to the first important modes. If not, the complete quadratic combination (CQC) calculations will be wrong.

The solutions are:

D.7.4.3 Validation of the number of modes - Complementary mode

Eurocode 8 specifies a minimum percentage of mass to be of interest in the spectral calculation.

If 90% of the mass is not interested, the software allows a complementary mode to be taken into account. It is a fictitious mode affected by the mass not excited by the studied modes and affected by the spectral acceleration associated with the last studied mode.

It has been shown that neglecting modes distorts the results (see 1st example in D.7.2).

D.7.4.4 Spectral Calculation and CQC Combinations

The spectral calculation allows to obtain the structural effects (efforts, displacements...) of each mode. Then, according to the statistical distribution of the earthquake according to the frequencies (defined by the regulatory spectrum), the effects are combined in order to obtain the statistical response of the structure to an earthquake.

The combination of the different unit modal calculations is done according to the CQC or SRSS mode, the theoretical definition of which is provided in Part 1 - Chapter 2.

It is important to differentiate between the regulatory spectra used in construction (which are generally dimensioning spectra) and those used for bridges (which are elastic spectra).

We go from the second to the first by dividing by a behavior coefficient (equal to or higher than 1.5) which takes into account the plasticity of the structure. The values of the behavior coefficients are defined by Eurocode 8.

In all spectral calculations, it is important to be sure that the damping of the structure is well defined. Depending on the software, the damping is assigned to modes or materials. In the second case, the mode damping will depend on the participation of each material in the deformation of the considered mode.

Caution, if we want to attribute a damping in the springs modeling the soil, this corresponds to a study of type soil-structure dynamic interaction, and it is not possible to use a dimensioning spectrum, only an elastic spectrum.

Finally, as indicated in C16.8, a different behavior coefficient can be assigned to each direction.

After the CQC or SRSS combinations (which combine the modes), the Newmark combinations must be made (seismic direction combinations), and then the action combinations.

D.7.4.5 Verification of support reactions under elementary cases

First of all, we evaluate the support reactions of the elementary seismic cases EX EY EZ and we compare it to the total masses.

Verification of support reactions can only be done by signing the modes.

For a building based on a base slab or a strip footing, it is important to limit the detachment of the supports. Indeed, the elastic calculation shows tensions in the supports that do not exist in reality because the foundations heave.

Negative support reactions (in red) cannot exist because in reality the foundations heave, so the actual stress distribution on the ground is different from the calculated one (cf. C16.8.3).

Support reactions of a building under superficial foundations

It is allowed to consider representative "elastic" models if the heave is limited: the limit is taken equal to 30% in the general case (10% in the case of nuclear buildings).

When detachment is important, much more complex non-linear seismic calculations are required. This verification of non-heave of the building must be done with care:

CQC Support reactions / Signed CQC Support reactions 

Seismic combinations (CP + E) make no sense if the seismic E efforts are all positive, while the CP dead loads are either positive or negative.

Example of the 24 Newmark combinations for the current frame:

D.7.5 Dynamic calculations other than seismic calculations

This paragraph concerns dynamic calculations other than spectral modal calculations (e.g. vibration of a railway structure or a pedestrian bridge in order to verify comfort criteria), and corresponds to calculations in which the load and the structure are calculated with an evolution over time.

D.7.5.1 Verification of free vibration or resonance behavior

In the case of a comfort study of a railway structure or a footbridge, it is advisable to look for loads cases that can cause the structure to resonate and the consequences of such resonance. For this, it is therefore necessary to apply periodic loads that can cause these resonances.

As a reminder, the resonance of the structure occurs when the periodic loading is at a frequency identical to one of the structure’s eigenfrequencies.

To verify that the frequencies of the applied periodic loads are consistent with those of the structure, we can easily find them on the time graphs obtained a posteriori. This method is applied to the temporal evolution of the acceleration, velocity or displacement of a representative node (for example the middle of a beam).

To do this, we count the number of periods between two distant points in time and divide this number by the time separating these two points. This gives a good approximation of the vibration frequency of the node in question:

Structure’s first eigenmode   temporal acceleration of a representative node

6.36 Hz/6.25 Hz =1.018; the approximation giving 6.25 Hz gives the right rough estimate
=> the node is excited according to the first eigenmode of the structure.

If the curve shows a very marked periodic variation over the time period in which the loading is applied, this corresponds to a forced vibration of the structure, and the method described above ensures that the frequency of the loading is indeed that expected.

If the curve shows this periodic variation over a time period after loading (the calculation was continued after the loading was stopped), this corresponds to the free vibrations of the structure. The method described above allows, in this case, to estimate the main eigenfrequency of the structure and thus to make sure that the excited eigenmode is the right one.

 

$translationBooks

Chapter E. How to ensure quality?

Chapter E. How to ensure quality?

Below are some simple advice to assess the quality of the finite element calculations. The principal challenges are:

The advice below covers the engineer’s or the team’s handling of the software, the verification controls that must imperatively conduct any engineer at the end of its modeling, and the tracing of the minimum items so that the work can be completed thereafter. 

E.1 Starting with a new software

E.2 Model validation using self-checking

E.3 Traceability and group work


$translationBooks

E1. Starting with a new software

We propose below some simple advice to deploy a quality approach in finite element calculations. The main issues are:

The advice below deals with the good handling of a software by an engineer or a team, the self-checking tests that each engineer must imperatively carry out at the end of his or her modeling, and finally the minimal elements to be traced to allow the work of several engineers or the later resumption of a model.

E1. Starting with a new software

When a new software is acquired in a design office, or when new engineers arrive, there is a very important, and unfortunately often overlooked step: the appropriation of the software and the validation of the user-software couple.

This validation, under the responsibility of the management, is at the heart of the quality approach of the studies that will be produced. We have seen, in the previous paragraphs, all the possible errors linked to a lack of knowledge of the software's operation, during the modeling process and when the results are used.

Tools exist to help during this validation phase. In particular, we can quote the "Validation guide for structural calculation software” published by AFNOR (French Standardization Association) 1990 (ISBN 2-12-486611-7). This guide, initially established for software validation for developers, provides a database of test data and simple modeling examples, accompanied by the correct results.

It is advisable to choose a few tests from this database, distribute them as an exercise to the team and share the results, right or wrong, of these tests so that everyone understands how the software works, the options taken by default and the mistakes to avoid.

 

$translationBooks

E2. Model validation using self-checking

E2. Model validation using self-checking

Before exploiting the model results, several verifications should be carried out on:

If some of these points prove to be redundant for the person who carried out the modeling himself or herself (see previous paragraph), they are essential in the case of the exploitation of a modeling carried out by a third person.

If the final objective of the global study is to perform non-linear calculations (geometrical non-linearities, non-linear material behavior law...), this validation is essential because it can avoid the unnecessary execution of long calculations. This is really important because obtaining an acceptable solution for a complex problem to be solved is rarely immediate.

In general, the realization of a small simplified model using bars allows to quickly validate some rough estimates for values from an FE model. See the example of the High-rise building tower (skewer model): Example A - High-rise building (part C).

It is also necessary to verify the model as the model progresses, especially in the case of dead weight load. All too often, we see engineers starting a model for several weeks and then stumbling over multiple error messages. It is also possible to save intermediate data files throughout the day, by incrementing the file name, so that you can return to a previous version very easily (the one that worked before the last updates).

This approach will also make it possible to evaluate the time required to generate the model, calculate and display the results.

Some important checkpoints are presented below. This list is neither limitative nor exhaustive. For specific problems, other checkpoints may be considered.

E.2.1 Initial model verifications

Before any calculations are carried out, it is necessary to carry out some basic verifications.

These verifications may seem tedious, but the detection of errors, often basic, can save a lot of time in the end.

a) Model geometry control

Simple graphical controls usually reveal inconsistencies in the geometric features of the elements.

Some software allows you to visualize the elements with their real section. This possibility is particularly interesting for beam type elements because it allows to control visually the correct orientation of the main axes and the adequate position of the longitudinal axis which will be used as reference for the loading for example.

The connection of the elements, the correct connection of the shells and the boundary conditions are an integral part of the geometric verification. The visual inspection of local coordinate systems before applying local loads is also part of the geometric verification.

b) Element features

For beam type elements, some software can propose predefined profiles. The very first time you use one of those elements, you should verify that the features displayed by the software correspond to the geometry; compare these features with those provided by the catalogs in the case of standard sections, or make approximate manual calculations of the features for non-standard sections.

For a section defined by its contour, the surfaces and inertias calculated by the software must be verified.

For curved problems or with eccentric loads, it is important to verify the position of the torsional center of the beams and to verify whether or not the software takes into account a possible offset between the center of gravity and the torsional center.

c) For material features, a proofreading of the data is necessary.

In the case of a mono-material model, an error on the Young's modulus can affect the results of the deformations without having an impact on the stresses. Whereas in the case of a multi-material model, an error on one of the modules will influence all the results.

d) Comparison with previous versions

When we have a simplified model from a previous phase, or when we make a modification on a model, we must systematically recheck certain main measures to detect possible errors.

e) Load features

For loads, a proofreading of the data is also necessary.

It is a question of visualizing all the loads applied to the model and this for each of the defined load cases.

The load values must be correctly identified; characteristic values or pondered values. The orientation and direction of these loads must also be verified.

If the model contains several load cases, it should be observed whether they are independent or successive load cases.

For dynamic studies, a verification of the masses of the model in all directions is essential.

E.2.2 Basic verification of calculation results

This step is based on simplified linear static approaches.

For each calculation performed, basic verifications must be made. These verifications, in addition to participating in the model validation, will also allow a beginner to become familiar with the post-processor of the software used and to verify that the different options of the elements and/or calculations have been activated correctly.

a) Deformation – Rough estimate of results

The general pattern of the deformation is very explicit because it gives an immediate response on the structure's behavior to a given load or stress. It allows to validate the hypotheses on the static scheme (simple support, fixed, ...) and on the modeling of the assemblies.

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.


$translationBooks

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:

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:

BIM model

FE model from the BIM model

 

$translationBooks

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?


$translationBooks

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, 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.).