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:

the element to work under normal stress, in flexion, or both?

them to consider shear and the associated deformations?

them to deform inplane or out of plane?
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 nonlinear 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 = Nonregular 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 nonlinear 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 nonlinear 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 postprocessing 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 Xaxis of the beam elements is usually directed from the "origin" point to the "end" point, with the Y and Zaxes being in theory positioned in any way relative to this Xaxis. However, the position of these Y and Zaxes must be homogeneous for elements of the same family, on the one hand, to facilitate the application of transverse loads (e.g. wind load), and on the other hand, to read the extreme fiber stresses which are defined by the Y and Z translation of the neutral fiber.
In most software packages, the local axes of the elements are oriented by default either with respect to the global coordinate system of the model (alignment of the local Z with the global Z) or with respect to the order in which the entities are created. It is always possible to force a homogeneous orientation on a set of elements.
Similarly, for 2D elements:

the outgoing normal must be known when defining load cases (earth pressure, fluids, or temperature fields).

it may be advisable to follow the logic of determining the outgoing normal, both for the input of the concrete covers in the case of a reinforcement calculation, but also to direct the element beforehand according to the assumed direction of the reinforcement to be installed (or checked). One will try to follow the same logic for the whole model (e.g. upward normal for all floors) so that errors are not induced in the exploitation of the results.

a uniform orientation also helps avoiding discontinuities in the display of stresses for a given fiber in two adjacent plates, for example.
Example: Plate and local coordinate system of elements
Subject: the direction of plate definition can, for some software, generate the orientation of the local coordinate system of the elements.
Example: Plate 6×6 m² (modeled with 2 plates of 3×6 m²), supported on 4 sides, loaded with 3 T/m².
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 cutoff point...
Check that all local coordinate systems have the same orientation.
C.3.6 Model size
The calculation time is often a determining factor in the cost of the project. Therefore, it is always interesting to try to optimize this calculation time.
The calculation time of a model depends on many parameters:

the number of degrees of freedom (number of nodes x DOF).

the performance of the machine.

the software performance (algorithm, parallelization, ...).

the amount of data saved (temporary nonlinear calculation).

the type of calculation (linear  nonlinear).
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 CO2generating clouds.
C.3.7 "Merge" or "Combine" option
Most software have the option to merge nodes or geometric construction points that are very close to each other within a tolerance set by default or by the user. This avoids mesh discontinuities.
This operation presents certain risks, particularly in the presence of expansion joints or the absence of welds that the model could ignore.
In the presence of joints, the user might choose between:

representing the joint with its width (modeled distance between the 2 lines defining the 2 edges of the joints). This is easily visible when manipulating the model and less likely to be "merged" by mistake afterward, but this may lead to elements with heterogeneous sizes (associated with the size of the joint) if the ends of the lines do not meet,

placing the points and lines in the same position in the model but modeling them independently. It is then difficult to check that the joint is well represented (unless the node numbers are displayed later) and node "merging" operations must be carried carefully.

use the linear release features offered by some software.
The merge operation may also impact the node links. Therefore, the mechanical links between nodes must be defined after merging.
C.3.8 Group of elements (for visualization and later processing)
Most software offers the ability to define groups of nodes or groups of elements.
This feature is very convenient and facilitates the assignment of materials and masses, the application of loads, or the postprocessing 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 crosssection, 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  biclamped plate
No Comments