# How to Mesh your CAD Model for Structural Analysis (FEA)

New to engineering simulation or to SimScale? Then meshing might be one of the things you’re struggling to learn. This article aims to teach you a few tips on how to mesh of your CAD model and ensure accurate results of your structural analysis.

Mesh generation (commonly know also as grid generation) is the practice of generating a polygonal or polyhedral mesh that approximates a geometric domain. Three-dimensional meshes are required in physical simulations such as finite element analysis or computational fluid dynamics (CFD) and need to consist of tetrahedra, pyramids, prisms or hexahedra.

At present, SimScale allows the meshing of structures with Tetrahedral meshing, which has the following options:

- Automatic
- Parametric
- Tetrahedral with local refinement

As shown in Fig. 01 below, all these cases allow for the specification of mesh order: first or second. Using a first-order generates a mesh with four-noded tetrahedral elements and second-order a mesh with ten-noded tetrahedral meshes.

**Fig 01: Meshing options offered by SimScale for structural mechanics problems**

A general overview is available in the SimScale documentation. In this article, we discuss some points to remember when considering problems related to solid and structural mechanics. Most points discussed here are pertinent to both tetrahedral and hexahedral elements, the discussion is primarily focused on the tetrahedral mesh.

## How to mesh solid bodies: Identify symmetry

In many problems, it can be helpful to identify symmetries that can exist in geometries. Using symmetry is one of the common and powerful ways to reduce the size of the problem. By definition, symmetry is said to exist if there is a symmetry of geometry, loads, and constraints about a line or plane of symmetry.

*Fig 02: Example of symmetry in solid bodies: A plate with a hole subjected to uniaxial tensile loading (left) and a cylinder in front-view subjected to radial pressure (right)*

As shown in Fig. 02, the symmetry of the object is exploited to create a reduced model for computation. Nodes are placed along the lines (in 2D) and planes (in 3D) of symmetry. These nodes placed along the lines / planes of symmetries are constrained for displacement perpendicular to these lines/surfaces and rotations along the line/surfaces. Considering just a quarter of the model allows for >75% reduction in the computational effort and time!

**Tip 01:** **Does the model being meshed have any symmetry? The symmetry could be along a plane or could be along an axis.**

## Interfaces and boundaries

Structures could have interfaces and boundaries like interfaces between multiple materials, contact, cracks etc. Mathematically, FEM is based on the assumption that the displacements are continuous inside an element. Interfaces are regions where possible discontinuities, like cracks etc, could occur and this means the displacement need not be continuous. Irrespective of jump in displacements, there is a definite jump in the stresses at an interface.

*Fig 03: Meshing in presence of interfaces: At the interface of two materials (left); when geometry changes (middle); loading changes (right)*

For example: Consider a material interface shown in Fig. 03. Here each material has a different modulus. In the absence of cracks, the strains at the common nodes are same. Now, knowing that stress = Modulus x strain, leads to different stresses on each side of the interface. In other words, we have a jump in stresses. Such a jump cannot be captured by an element across which interface passes. Similarly, other conditions when there cannot be an element across a boundary include:

- When geometry changes, elements cannot cross these boundaries and it is necessary to have nodes at the interface
- When loads change abruptly, nodes need to be present at the interface where the load suddenly changes
- Nodes need to be present at points where concentrated loads are applied

Automatic meshing algorithms consider the interfaces as long as the CAD geometry is partitioned along the interfaces. In general, the automatic tetrahedral mesh works well but if an element is overlapping across an interface, then partitioning these become necessary.

**Tip 02:** An interface can never pass through an element!

## Mesh refinement

The automatic mesh generators generally start by creating a surface mesh of triangles and further extrapolate using these triangles to form tetrahedrons in the volume. In many cases, during the shape of tetrahedrons formed inside the volume can get quite distorted and thus leading to failure of mesh generation. This is generally encountered in two cases:

- Complicated CAD geometries
- Geometries with high-aspect ratios

Depending on the geometry of the structure, the CAD model could contain geometries of high aspect ratios, fillets etc. In such situation, it is very likely possible that the ad-hoc automatic meshing might not generate the best meshes. Most often, these small structures are meshed over when large elements are used and the mesh does not conform to the exact geometry. In such cases, it is best to resort to a priori mesh refinements.

*Fig 04: Mesh refinement of surfaces for improved accuracy in solutions. CAD model (left), Areas needing mesh refinement identified in red (middle), Mesh incorporating refinement (right)*

Fig 04 demonstrates the capability of SimScale for providing an excellent mesh refinement. The areas needing refinement can be identified and the mesh generator ensures a suitable mesh with refinements.

**Tip 03: Mesh refinement is a definite necessity if the structure has parts of significantly different dimensions.**

## Meshing for nonlinear elasticity: Contact problems

Problems involving linear elasticity is one of the well-researched problems in mechanical engineering. For all linear elasticity problems, irrespective of mesh sizes, the Newton-Raphson iteration will converge in one iteration. However, it is always recommended to perform a mesh refinement and convergence study to ensure the accuracy of the solution. However, the same cannot be said when a material nonlinearity (like hyperelasticity, viscoelasticity, plasticity etc) are involved. The problem can be well-posed and a unique solution could exist. Yet, the problem might fail to converge if the mesh is not sufficiently fine in regions where the strong nonlinearity is observed. Here, some tips are discussed with regard to contact problems which are highly nonlinear in nature.

Contact is highly nonlinear in nature and hence to this day remains a computational challenge for modeling large deformation contact problems. Thinking of it in simple terms, at a certain time there is no contact and then suddenly there could be contact. Most problems involving hyperelasticity etc, are nonlinear but continuous. But contact is a switch or a discontinuity.

*Fig 05: Meshing in contact problems. Aspect ratio between mesh density of master & slave surface *

As shown in Fig. 05, meshing can significantly improve solutions for problems involving contact. SimScale currently allows contact where the sliding displacements are small. For such problems, mesh ratio between master and slave surfaces needs to be optimal. A general rule of thumb can be that one master element should be less than 2-3 slave elements, at worst! Additionally, if one or more surfaces are convex in nature, i.e. has sharp corners, then it can lead to non-uniqueness of solutions. The normal and tangential vectors are needed to calculate the distance between the two surfaces along the direction of these vectors. If a sharp point exists where two normals can be defined, this leads to ambiguity in choosing the normal vector causing a non-uniqueness.

**Tip 04: Mesh ratio between master and slave surface needs to be optimal. Avoid sharp corners in contact surfaces!**

## Identify stress singularities and concentrations

Have you ever wondered why airplane windows are not exactly rectangular but are curved? Some of the first airplanes had rectangular windows and it was soon realized that the sharp corners lead to stress concentration and crack initiations. Identifying such singular points and refining the mesh in these areas can lead to more accurate results.

Firstly, what is a stress singularity? A stress singularity is that point in a mesh where the stresses do not convergence. Since theoretically the stress at this point is infinity, as the mesh is being refined, the stress at this point continues to increase. Nevertheless, it is very important to note that the displacements calculated at these stress singularities remain accurate even though the actual stress at the point remains questionable. That apart, a very small distance from the point, the stresses calculated are accurate.

Yet, such occurrences are very common in reality and the user needs to identify these areas. They are regularly encountered at points where a point load is applied, the presence of sharp corners and at points with restrained boundary conditions over a single point etc as shown in Fig. 06. Such occurrences are easily seen in welded parts etc.

*Fig 06: Commonly observed reasons for stress singularities: sharp corners (left); concentrated point loads (right)*

It is important to answer the question if the local phenomenon is of interest. If yes, then the easiest way is to refine the mesh near the singularity. If no, a course mesh could do the job. Due to the applicability of St. Venant Principle, the local stress singularity is lost as one moves away from the point. Thus, the bulk results obtained are still accurate.

**Tip 05:** **Are there singular points? Both mesh refinement and a course mesh are possible ways depending on the quantity of interest.**

## Locking effects in bending problems

Geometric nonlinearities and locking effects are commonly observed when solid elements are used for meshing thin-structures. This is especially true if they are subjected to bending loads. This kind of locking is known as “Shear Locking”. Shear locking here should not be confused with the membrane or volumetric locking effects. Shear locking is observed since the first-order elements using linear interpolation function for displacement. In other words, displacements are represented by a linear function and the derivative of a linear function is constant. Thus, the strains are constant throughout an element. In reality, this is not the case. Such a wrong estimation of strain results in an inaccurate estimation of the strain-energy and the overall structure exhibits a much larger stiffness. The net displacements of a structure will be much less than that observed in the actual structure.

*Fig 07: Demonstration of locking effect in a simple cantilever beam. The blue line represents the analytical solution in the formula; Red line represents the FEM results using first-order elements; Yellow line represents the FEM results using second-order elements*

As shown in Fig. 07, a simple cantilever beam is considered for which an exact analytical solution exists. The displacement of the beam is plotted as a function of its length. As evident from the graph, second order elements perform very well to predict solution to acceptable standards of errors. On the contrary, using first order elements leads to a complete under-prediction of the tip displacement.

As already obvious, there are two possible solutions to circumvent this problem:

- Mesh refinement along the thickness by using multiple elements (5+ at least)
- Using second-order mesh could already significantly reduce the locking effect

The downside of the first approach is that it increases the number of elements and significantly increases the computational size. For example: if the beam is 1000 mm in length, 250 mm in breadth and 10 mm in thickness. If we had only one element along the thickness, we are looking at approximately **2500 elements**. Upon refinement using the first criterion, we are then looking at elements of size around 2 mm and hence about **312,500 elements**. Alternatively using the higher-order element, 2500 second-order elements could already solve most of the problem.

**Tip 06: If you are dealing with thin structures or with bending-dominated problems, a second-order mesh is a definite yes!**

## Locking effects due to incompressibility

Yes, again! Volumetric locking is commonly observed due to incompressibility constraint. It is well known to occur in rubbery materials, it is also important to note that plasticity is a perfect example for incompressibility. Volumetric locking is addressed in sufficient detail on our SimScale blog article on modeling elastomeric materials.

**Tip 07:** **Volumetric locking needs to be considered for plasticity too!**

The overall tips on how to mesh discussed here are not a comprehensive list of things-to-do but a general idea of the minimum things to account for while using FEM for structural mechanics related problems.

**Just want to learn more about simulation with SimScale? Download the company’s booklet.**