Stress Singularities, Concentrations and Hot Spots

You run your study and you find the maximum stress is 150MPa.  The yield of the material is 300MPa so the stress is below the yield with a factor of safety of 2.  Is the design safe?  Not necessarily.  You decrease the mesh size by half and find the stress is now 320MPa.  So the stress is now over the yield.  Is the design a fail?  Not necessarily.  You need to identify if the maximum stress is a real stress concentration or if it is a numerical singularity.

What is a singularity?

Singularities are not a SOLIDWORKS Simulation specific problem, but a general one introduced by using Finite Element Analysis (FEA).  Singularities are inherent in all FEA calculations due to the inability to mathematically calculate stress at locations such as sharp corners, point loads, or fixed boundary conditions.  Mathematically the stress at these locations is infinite however due to errors in meshing and calculations, FEA shows a value for the stress result. So how can we tell if we have a singularity? Stress singularities arise due to either a geometric discontinuity or a concentrated load or fixture so we can investigate the location of the high stress. They are also divergent in nature, so reducing the mesh size, the value of stress will increase to the theoretical value of infinity. So we can decrease the mesh size in the location of the high stress and observe the change to see if it is diverging to infinity.

Stress concentrations

Stress concentrations are where you have large stress gradients over adjacent elements at a localized area of a model. You will see stress concentrations where there are changes in geometry, such as a presence of a hole in a plate, at boundaries where different materials are present, and at points where bodies come into contact. High stress gradients due to stress concentrations will converge to a specific value if the mesh is sufficiently refined. So if the stresses at the elements do not increase with mesh refinement and converge towards a finite value, then they indicate a stress concentration.

Stress Hot spots

In Simulation 2017 the stress hot spot diagnostics tool was introduced to assist you in detecting irregular high stress gradients between adjacent elements. Further investigation can then be done in these areas to identify if they are singularities and need to be ignored or they are in fact stress concentrations.
The stress hot spot diagnostics tool detects stress singularities in a model in these cases:

• Near sharp geometric edges and internal re-entrant corners on solid and shell bodies.
• At regions where applied boundary conditions restrict the body to freely expand (or contract) under the loading environment. Remember that in the real world there are no “infinitely stiff” supports or fixtures.
• On geometric edges of solids where loads/fixtures are applied, or where abrupt transitions of boundary conditions occur (very rigid to flexible).
• Around vertices where point loads and point fixtures are applied (on solids or shells).

Note: Stress hot spots are not detected at areas of contact and at faces where rigid fixtures are applied.

The stress hotspot diagnostic tool can be found by Right-click the Results folder and click Stress Hot Spot Diagnostics.

To run the stress hot spot diagnostic you are required to select a sensitivity factor.

This filters the elements based on the magnitude of the equivalent strain relative to the maximum equivalent strain for each body. A higher sensitivity factor includes more elements with high strains, and may detect multiple stress hot spot areas on multiple bodies (at the expense of longer computational time). For example, for a sensitivity factor of 60%, the tool includes elements that fall within the top 60% of highest equivalent strains for each body.
By Default only elemental stress is evaluated but you can choose to include nodal values as well.
After you run the Stress hot spot diagnostic you can show the plot and isolate just the elements identified as having a high stress gradient.  You can also go back to change the sensitivity.

• Identify if it is a Singularity or a stress concentration by investigating the location and refining the mesh. When you rerun the stress hot spot diagnostics tool, the areas of stress concentrations should be filtered out if the mesh is fine enough, and the remaining stress hot spots would point to stress singularities. Note that in the physical world, stress singularities do not occur as the material will yield or crack when stresses exceed the material’s ultimate strength limit.
• If the stress hot spot is identified as singularity try and remove the source of the singularity. For example if it is a sharp re-entrant corner add a fillet. Remember that in the real world a manufactured “sharp corner” will always have a small fillet radius. If it is due to loads or fixtures on vertices or along edges, try to distribute the load on the model. If you are able to eliminate the singularity run the stress hot spot diagnostic tool again as the first singularity may have overshadowed other singularities.
• If you cannot eliminate the stress singularity you will need to ignore these localized areas, especially if they are not near the area of interest in your simulation, and examine the stress results further away which should remain “unpolluted”. Remember that even if the load is applied as a singular point load creating a stress singularity (σ = P/A and A=0 → σ=∞), the stress distribution some distance away from the applied load will still be correct.

For more information see solution article S-060938 in the Solidworks knowledgebase