Stress Hot Spot PropertyManager

The Stress Hot Spot diagnostics tool detects regions of the model where stress gradients between adjacent elements are irregular. In certain cases, these irregular high stress gradients can be attributed to stress singularities.

The Stress Hot Spot functionality is only available with linear static studies that use solid and shell mesh elements.

The stress hot spot diagnostic tool identifies regions of the model with irregular stress gradients between adjacent elements. The cause of the irregular stress gradients could be due to stress singularities.

When the Stress Hot Spot diagnostics tool detects irregular stress gradients around leading edges, it prompts you to refine the mesh locally, and run a stress singularity detection.

The concept of a stress singularity exists in numerical analysis, and does not have a physical meaning, as there are no infinite stresses at a singular point
The stress hot spot diagnostics tool detects irregular stress gradients in these cases:
  • Near sharp geometric edges, and on corners on solid and shell bodies.
    (a) Stress singularities detected at sharp edges where no fillets are applied. The angle between the geometric planes at the common sharp edges ranges from 0º to 360º. (b) The stress hot spot diagnostics tool can detect stress singularities at corners (internal and external). These corners are located on angles ranging from 0º to 360º.
  • 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).
Stress hot spots are not detected at areas that come into contact.

To open the Stress Hot Spot diagnostics:

  • Right-click the Results folder, and click Stress Hot Spot Diagnostics.
  Sensitivity Factor Filters the elements that participate in the stress hot spot diagnosis 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.

  Node Values When selected, you can view the stress hot spots on contour plots of nodal or elemental von Mises stresses. Elemental plots display one stress value for each element. Nodal plots display one stress value for each node.
  Run Stress Hot Spot Diagnosis Executes the stress hot spot diagnostics tool. If stress hot spots are detected, in the next step you can view a von Mises contour plot with the hot spot areas colored in gray.
You can select a different color from the default gray to render the stress hot spots in the Chart Options > Specify color for values above maximum value . You cannot modify the maximum threshold stress value shown on the chart of a Stress Hot Spot plot. Regions of the model with stress values higher than the maximum threshold stress value are highlighted in gray and flagged as stress hot spots by the solver.
  Show/Hide Stress Hot Spots Toggles the visibility of the stress hot spots on the von Mises contour plot.
  Show/Hide Stress Singularities When you run Stress Singularity Diagnosis, toggles the visibility of stress singularities on the von Mises contour plot.
  Isolate Stress Hot Spots Renders only the elements at the stress hot spot areas. The rest of the model is shown in transparent mode.

In the plot legend you can view the sensitivity factor considered for the analysis, the number of elements flagged as stress hot spots, and the percentage of elements flagged as stress hot spots.
  Isolate Stress Singularities When you run Stress Singularity Diagnosis, renders only the elements on the leading edges causing stress singularities.
  Plot Convergence Graph Available when you run the Stress Singularities Diagnosis. Plots the maximum von Mises stresses observed on the leading edges with successive mesh refinements. Divergent von Mises stress values point to stress singularities. For example, the plot shows divergent von Mises stresses across three mesh refinement levels for four leading edges. These edges are the cause of local stress singularities.

Consider rounding sharp edges with fillets to avoid the occurrence of stress singularities.

Detect Stress Singularities (slower)

When the Stress Hot Spot diagnostics tool detects regions of the model with irregular high stress gradients, you can apply local mesh refinements to selected geometric edges in the hot spot regions to check if these sharp edges cause stress singularities.

  Mesh refinement level

Sets the mesh refinement level: two, or three.
  Element size reduction factor across levels Sets the mesh reduction factor across the mesh refinement levels. See the calculated mesh size for each refinement level in the Mesh Refinement Details table. You can also enter the mesh size value for each refinement levels. For the selected geometric entity, clear the check box under Include, and enter the desired element size across mesh refinement levels.
  Element size growth ratio Sets the element size growth ratio between successive mesh layers. Assuming that the mesh element size used for meshing an edge is e, and r is the element size growth ratio, the average element size in layers radiating from the edge will be: e, e*r, e*r2, e*r3, ...., e*rn.
  Mesh Refinement Details Displays the edges where local mesh refinement is applied to detect local stress singularities when running Stress Singularity Diagnosis. Select an edge to highlight in the model.

The current mesh size and the successive mesh sizes across the refinement levels are listed. Only edges located on sharp angles of solid bodies can be considered for Stress Singularities Diagnosis.
  Restore the study with the original mesh settings When you run stress singularity detection, the program retains the original mesh element size as the current mesh value.
  Overwrite existing mesh and results with final level settings

When you run stress singularity detection, the mesh size from the last refinement level becomes the current mesh size. The plots from the Stress Singularity Diagnosis are based on the final mesh level settings.

The last refinement level is saved to a mesh control definition in the study tree under Mesh.
  Run Stress Singularity Diagnosis Following a Stress Hot Spot Diagnosis, you can run a Stress Singularity Diagnosis. The program detects geometric edges of your model where stress hot spots are detected and applies successive local mesh refinements to identify stress singularities. You can re-run a Stress Singularity Diagnosis by further refining the local mesh on leading edges by setting new mesh refinement levels.
Stress hot spot plot. Elements in regions identified as stress hot spots are in grey. Probed annotations on elements display the Stress Hot Spot string for Value.
Isolate Stress Singularity plot. Probed annotations on elements display the Stress Singularity string for Value