you are here:   / News & Insights / Engineering Advantage Blog / Why Worry About Sharp Corners and Point Loads?

Engineering Advantage

Why Worry About Sharp Corners and Point Loads?

Sharp Internal Corners & Edges | FEA Consulting
May 22, 2015 By: Steven Hale

We teach a lot of FEA training classes here at CAE Associates, and one of the issues that we emphasize is the need for quality geometry, loads, material data, and boundary conditions.  Beyond the obvious need for accuracy, there are some specific characteristics of geometry and loading in FEA that require special consideration:  most notably sharp corners and point loads.  Engineers are often given geometry that contains sharp corners and loads that include forces at discrete points or edges.  So why not use this information as supplied? What’s the big deal with sharp corners and point loads? The problem with sharp internal corners/edges and point loads is that they are sources of numerical singularities. This means that these locations are incapable of predicting accurate results even with accurate input data and a very fine mesh.  Two examples of sharp internal corners are shown in Figure 1 above.

These regions represent stress concentrations with an infinitely small radius.  Numerically, finite element analysis calculates stress in these corners based on the local element size, with smaller elements yielding higher stresses. As a consequence, increasing mesh refinement only serves to increase the stress without limit.  An example of this is shown in Figure 2 for a stiffened panel subjected to a bending load.

Figure 2: Stress vs. Mesh Density for a Stiffened Panel in Bending - Stress Convergence Behavior

The top (blue) line shows that the stress does not converge to a solution with increasing mesh refinement as it should.  The best way to resolve this problem is to replace the sharp corners/edges with fillets.  The effect of this change is shown by the bottom (red) line in Figure 2 where the sharp corner was replaced by a small fillet. This eliminates the singularity and allows for the stress solution to converge as the mesh is refined.

Applying loads directly to edges or points presents a similar problem.  In theory, the area over which the load is applied is infinitely small, resulting in an infinitely high stress.  In such cases, FEA calculates stress based on the sizes of the elements attached to the edge or point to which this load is applied. As such, increasing mesh refinement reduces the element size, causing stresses to increase without limit. This effect is shown in Figure 3 (top blue line) for the same stiffened panel but with a load applied to an edge near the free end. 

In this case, the local stress directly beneath the applied load is very high and increases significantly as the local element size decreases.  The best way to resolve this problem is to simply distribute the load over an area.  This effect is shown by the bottom (red) line in Figure 3 where the same load was distributed over a small area instead of an edge. As expected, this eliminates the singularity and dramatically reduces the local stress.

Figure 3: Stress vs. Mesh Density for a Stiffened Panel with an Edge Load and a Distributed Load - Stress Convergence Behavior

In many cases, eliminating sharp corner and point load singularities as suggested would be difficult to accomplish without some time and effort.  Leaving these features in your model is certainly an option, but only if they are located away from all critical regions where accurate results are required.  Even if they are left in a model, you need to be aware that these singularities exist and will adversely affect your results in these locations.  When reviewing stress results, you should always be aware of all sources of singularities and recognize that stresses in these locations should not be presented as real or accurate.

There are other sources of numerical singularities such as point constraints or “cracks” in the mesh, however sharp internal corners and point loads are often the most commonly encountered ones.  Being able to recognize and deal with them is a critical part of the finite element modeling process! I am very interested to hear about any experience you have in dealing with numerical singularities.  How have they affected your critical results?  Do you always remove them or do you have other ways of dealing with them?