FEA boundaries can usually be obtained using simple fixed constraints. But, this can result in singularities that produce erroneous results. To determine whether results show a real stress concentration or a singularity, an accurate solution can usually be obtained by either using elastic supports or modeling contact between components.
Dr. Jody Muelaner, PhD CEng MIMechE
Singularities in Finite Element Analysis (FEA) can cause real issues, even for an apparently simple structural analysis. Singularities lead to completely erroneous results and stresses that continue to rise as a mesh is refined. Many singularities are caused by stress-raising geometry such as holes and sharp internal corners, and this is generally well understood. Singularities caused by sudden changes in boundary conditions can be harder to spot and resolve. In fact, setting up realistic boundary conditions is often the most challenging aspect of a simulation.
What is a singularity?
A singularity is a point in the model where a value, such as stress, tends to infinity. As the mesh is refined, the increasingly small elements get closer to this point and the value therefore rises. As the element size tends to zero, the stress will tend to infinity. This produces nonsensical results and prevents mesh convergence.
Geometry that causes singularities
Singularities caused by stress-raising geometry such as holes and sharp internal corners are well understood. In the real world, there is likely to be a small radius on any internal corner, meaning the stress would not actually continue to rise. In any case, local yielding will limit the stress in such features. The location of these singularities can often be readily identified, excluded from convergence results and localized models used to predict the true stress in the features responsible. Singularities at corners are similar to cracks and the stress intensity factor can be calculated using the J-Integral, or considering the strain energy release rate – the energy dissipated during fracture.
There is, however, another type of stress raiser in FEA models that is talked about less often and which can be more difficult to deal with. Where there are abrupt changes in boundary conditions, such as a split line where a fixed constraint ends, this can also result in stress that continues to rise unrealistically and causes mesh convergence to fail. Let’s explore why this happens and how it can be avoided.
How can boundary conditions cause singularities?
The most obvious way that a boundary condition can cause a singularity is when a force is applied to a single node. Since stress is force divided by area, applying a force at a single point will give an infinite stress. If the area where the load is applied is not of interest, then it can be acceptable to use such a boundary condition. Due to Saint-Venant’s-principle, which states that, if the distance from the load is large enough, two different but statically equivalent loads create essentially the same effect. This can be easily seen where the same total force is applied to the sponges in two different ways. The fingers represent point loads and the flat hands distributed loads. Although the effects close to the applied loads are different, in the center of the stack, at a sufficient distance from the loads, the effect is virtually the same.
When loads are simplified to point or edge loads, it is simply important to understand that the very high stress around the applied force does not represent reality. These regions must not be included in results, mesh convergence or adaptive meshing. Next, we’ll look at some more involved examples of boundary conditions casing singularities.
Abrupt changes to a fixed boundary condition
It is often convenient to fix a face of a model, to constrain a component that is loaded with forces applied in some other area. It should first be noted that such a fixed constraint can never truly represent reality. A fixed boundary condition essentially means that the face is bonded to an infinitely stiff body. In the real world, all solid bodies have some flexibility and often a part will actually be clamped rather than bonded. However, if the peak stresses are not expected in the region being represented by a fixed boundary, this may seem like a reasonable approximation. As with point loads, it can, therefore, be a good idea to simply exclude the stresses in this region from any mesh convergence. However, not all software allows this, and it is particularly problematic if automatic mesh refinement, or adaptive meshing, is being used.
A shaft can provide a good example of these issues. The shaft illustrated below has been cut in half and a symmetry fixture applied. The smaller cylindrical face at the right-hand end of the shaft has been split into three separate faces to allow a vertical force to be applied to a defined region. The other end of the shaft would be held by two bearings, with the outer bearing constraining axial movement against a shoulder and the end face.
When standard inelastic fixtures are used, stress singularities occur where the fixtures end. This effect is equivalent to the edge of a stiff part digging into a soft part. This can be seen below, where a bearing support extends between a split line and an external radius. It also occurs on the face of the shoulder which was constrained using a roller/slider constraint in SolidWorks Simulation. When the mesh is refined on the radius it is clear the singularity occurs where the fixtures end and is not a real stress concentration in the radius. This is particularly problematic because the radius is also a stress concentration and this region cannot, therefore, simply be excluded from the results or mesh refinement.
Using elastic supports
One solution is to use elastic supports rather than fixed constraints. In a fixed constraint, each node on the constrained surface is forced to zero displacement. An elastic support consists of an additional spring element for each node on the constrained surface. One end of the spring is attached to the node on the surface and the other end of the spring is fixed with zero displacement. The actual stresses in the springs are not normally included in the results. Using elastic supports can eliminate the issues with stress singularities at the edges of boundary conditions, but care must be taken to select realistic stiffnesses for the supports. If the stiffness is too small, the model may encounter excessive displacements which cause the solver to fail. On the other hand, if the stiffness is too great, a spurious stress concentration may still be seen at the edge of the constraint. Although an initial value for the support stiffness may be calculated by considering the type and thickness of the actual material which would provide the support. The image below shows that, with correctly set elastic supports, the model properly converges on the actual high-stress region.
Modeling contact
Another similar approach is to model contact between the supporting components and the component of interest. This can be the most accurate, but can also be seen as simply pushing the problem to another area, since the supporting components must then be constrained in some way. However, if the supporting components can be excluded from the mesh convergence and final results, the supporting components can be simply constrained by fixing faces.
Mesh convergence and adaptive meshing
Mesh convergence is one of the most important methods to ensure a reliable FEA simulation. The basic process is simply to rerun the simulation a number of times, refining the mesh around areas of interest and recording the relevant values for the simulation using each mesh. When the value of interest varies randomly, and by a small amount, in both directions, the model can be said to have converged. If there are large differences in the result, or the result keeps creeping in the same direction as the mesh is refined, then this indicates a problem, often a singularity. What constitutes a small change is somewhat subjective but can generally be considered as a few percent of the value under consideration.
Adaptive meshing takes mesh convergence a stage further, automatically refining the mesh at areas of interest and rerunning the simulation until the model is converged, or convergence fails according to some criteria. There are two types of adaptive meshing: H-Adaptive reduces the element size and P-Adaptive increases the element order. SolidWorks Simulation does not currently support P-Adaptive meshing for elastic supports.
Conclusions
In many cases, it may be possible to obtain useful results while using simple fixed constraints. However, this can result in singularities that may prevent mesh convergence and produce erroneous results. It is important to be aware of this issue, since some judgment may be required to determine whether results show a real stress concentration or a singularity arising due to simplified boundary conditions. When this happens, an accurate solution can usually be obtained by either using elastic supports or modeling contact between components.
