Typically, as you make your mesh finer, your stress converges to its nominal value (see this blog for an example!). However, this may not always be the case. Below we have a round shaft loaded in tension with different mesh sizes:
As you can see, as the mesh gets finer, the maximum stress continues to increase (diverging) and is always concentrated on the last row of elements before the thickness change. Does this mean that FEA is broken and we can’t trust its results anymore? Not at all - this is a stress singularity known as a reentrant corner.
What Is A Reentrant Corner?
We can define a reentrant corner as a perfectly sharp inside corner that causes an infinite change in stiffness in the part. Because the change in stiffness is infinite, the stresses in a reentrant corner will always diverge.
Let’s illustrate this with an example. Here we have four beam elements arranged in an angle with the elements and nodes labelled. Since element 3 is along the x axis, its stiffness matrix involves the derivatives of the shape functions at nodes 3 and 4 with respect to x (dN/dx). However, at node 3, the derivative of the shape function with respect to x is 0 since element 2 is along the y axis. This leads to a stiffness matrix containing only 0s.
Since element 2 is along the y axis, its stiffness matrix involves the derivatives of the shape functions at nodes 2 and 3 with respect to y (dN/dy). However, at node 3, the derivative of the shape function with respect to y is 0 since element 3 is along the x axis. This also leads to a stiffness matrix containing only 0s. No matter which element you use to formulate the stiffness matrix, the stiffness matrix at node 3 will also be full of 0s, leading to the stress singularity.
If we added a radius to this example, we can then formulate a stiffness matrix at node 3 since both elements 2 and 3 have changes in x and y.
Reentrant corners are very common in FEA – they can occur because of how a component is modeled in the CAD, or they are made as a result of geometry simplification.
What To Do About Reentrant Corners?
The first (and most important) step is to recognize the reentrant corner in the first place! If you’re not sure you can always try to make the mesh finer in the area and see if the stress is diverging or not, similar to the study done earlier in this blog.
Once the reentrant corner is identified the easiest approach is to simply ignore the stresses right on the reentrant corner. This approach is most valid if the reentrant corner is not in a high stress area of concern. Typically, the stresses one or two elements away from the corner are more realistic. This is known in more academic terms as Saint-Venant’s principle, which states:
“Stress and strain produced at points in a body sufficiently removed from the region of load application will be the same as the stress and strain produced by any applied loadings that have the same statically equivalent resultant, and are applied to the body within the same region.”
If the cross section allows for it, performing a hand calculation on the section forces at the reentrant corner will typically give a more accurate result as well, especially if running a linear static analysis.
If the reentrant corner is in a high stress area of concern, the other approach is to add a small radius, which changes the stress singularity into a stress concentration. This would allow the mesh to converge properly. Additionally, in almost all real-life applications, perfectly sharp reentrant corners do not actually exist due to manufacturing constraints, so adding a small radius would be valid. Just beware of doing this to all reentrant corners in your model as the element count, and therefore, runtime, can get very large very quickly. Consider sub-modeling if needed. Also, if you have physical test results, you could correlate to them using your model.
In this example, a shaft with a cross section of 10 mm in diameter and 10 mm long is loaded with a force of 500 N in the X direction. The analysis was run with linear static assumptions.
In the contour below, there is no radius between the shaft and the thicker piece (which is 30 mm in diameter). Just like the tension example from earlier in this blog, the stress values at the corner diverge since there is no radius and therefore there is a reentrant corner.
The table above compares the stress values from the FEM with the hand calculated stress at 1mm away from the reentrant corner. As you can see, the FEM stress matches the hand calculated stress quite well at 1mm away from the corner, while the FEM stress diverges at the corner. The formula used for the hand calculated stress is
where P is the expected stress, V is the shear force, M is the bending moment, A is the cross-section area, I is the area moment of inertia, and r is the radius. At 1mm away from the corner, we expect V = 500N and M = 4,500Nmm.
As an alternative to probing the stress directly from the FEM, you can pull the section forces, which will get you a much more realistic answer which will converge as the mesh gets finer.
Section Forces, corner: [Expected: V = 500N and M = 5,000Nmm]
Section Forces, 1 mm from the corner: [Expected: V = 500N and M = 4,500Nmm]
The table above compares the stress values calculated from the section forces (using the same formula as before) with the hand calculated stress at the reentrant corner and at 1mm away from the reentrant corner. Compared to the previous table with the FEM forces, the section forces converge toward the hand calculated value at both locations. HOWEVER, there is one very important caveat – even though the stresses at a reentrant corner won’t be infinite in real life, the corners will still be stress concentrations and will therefore have elevated stresses. This elevated stress is equivalent to the hand calculated stress multiplied by a stress concentration factor (Kt). If there is a known or assumed radius, the stress concentration factor can be quantified using a resource such as Peterson’s Stress Concentration Factors and used in conjunction with the section forces to find the real stress, which is done in the example below.
In the contour below, a radius of 0.5 mm is added to the same shaft.
The image above shows that the stress values converge when a small radius is added. These stresses will not match the section forces in this case due to the stress concentration caused by the radius; however, this stress concentration is quantifiable using Peterson’s Stress Concentration Factors. In the table below, the hand calc stress from the corner before is multiplied by Kt = 2.39, which was calculated using Peterson’s.
From Peterson’s Stress Concentration Factors:
It is important to stress that mesh size does matter a lot when using a radius – if there’s not enough fidelity through the radius, you will not get the correct stress value. In the plot above, the stresses in the circled region are <5% away from each other, with the variation being due to each mesh size (0.125mm, 0.25mm, and 0.5mm) having different amounts of elements through the radius.
Reentrant corners are stress singularities that mathematically diverge as the mesh gets finer. While perfect reentrant corners are very rare in real life, they are very common in FEA due to geometrical simplifications. The two most effective approaches to handling them are to either ignore the stresses at the corner or to introduce a small radius. Knowing how to effectively handle these is an essential aspect to performing proper FEA.
If you’ve been struggling with a reentrant corner in your project, our well-rounded services team can help! Reach out to us today!