Adaptive Mesh Refinement

• Use Adaptive Mesh Refinement to reduce the mesh size in specific areas of the model, automatically. The solver identifies critical stress regions in the model, and automatically remeshes the model using increasingly smaller elements in the critical regions, then repeats the solution. The process continues until the stress results variation between two consecutive iterations is smaller than a specified value. Adaptive Mesh Refinement is essentially an automated means of performing a mesh convergence study.

Adaptive Mesh Refinement is available for the following simulation study types:

• Static Stress
• Modal Frequencies
• Thermal
• Thermal Stress

There are five refinement controls:

• None disables adaptive mesh refinement. This is the default setting.

• Low, Medium, High - As you increase the level of refinement, the following adjustments are made to the preset settings:

  • The Maximum Number of Mesh Refinements increases.
  • The Results Convergence Tolerance decreases.
  • The Portion of Elements to Refine increases.

• Custom activates the individual input fields in the dialog so that you can specify your own custom refinement settings.

Maximum Number of Mesh Refinements

The Maximum Number of Mesh Refinements is the maximum number of mesh refinement and solution iterations the program may attempt. Once this number of refinement passes is reached, the solving phase terminates (whether the results have reached the desired accuracy or not). This option provides a means to prevent a model with diverging or unstable results from running for an excessively long time. Also, solving times can become very long if the mesh is refined to the point that an extreme number of elements are generated. In most cases, good results are achieved in a reasonable number of refinement steps (less than 8, for example).

Results Convergence Tolerance (%)

Once the %change in the results between two consecutive iterations is less than, or equal to, the Results Convergence Tolerance, the results are considered to be acceptable. No further adaptive mesh refinement or solutions iteration is performed. For any results change greater than the specified percentage, the mesh is further refined and the solution rerun. The smaller the value is, the more accurate the results must be to complete the refinement process.

Portion of Elements to Refine (%)

Refinement occurs at critical regions of the model (such as, where the stresses are highest in a structural analysis). This option controls how much of the model is refined. For example, at 5%, only the those elements in the top 5% with regard to the critical result are refined. At 50%, half of the elements are refined, and at 100% all elements are refined.

Frequency Mode

It specifies which vibration mode to use as the basis of the refinement process. Note: This option is only applicable to Modal Frequencies analyses.

Results for Baseline Accuracy

The choices depend on the simulation type, and this setting is not supported for Modal Frequencies studies. You can specify the desired result on which to base the convergence test regardless of whether you are using a refinement preset or custom settings. The available options are as follows:

• For Static Stress studies:

  • von Mises Stress: This option is the default for assessment of the mesh/results accuracy. von Mises stresses are compared for each iteration. This option is appropriate when you are comparing equivalent stresses to the yield strength of the material as a failure criterion.
  • 1st Principal Stress: Choose this option to base the mesh/results accuracy assessment on the 1st principal stresses. This option is appropriate when you are comparing principal stresses to the ultimate tensile strength of the material as a failure criterion and the critical stresses are tensile (positive).
  • 3rd Principal Stress: Choose this option to base the mesh/results accuracy assessment on the 3rd principal stresses. This option is appropriate when you are comparing principal stresses to the ultimate tensile strength of the material as a failure criterion and the critical stresses are compressive (negative).
  • Displacement, Total: Choose this option to base the mesh/results accuracy assessment on the total displacements. Generally, displacement results converge more easily than stress results do. Therefore, comparing the stress results between iterations is generally more conservative.

• For Thermal studies:

  • Heat Flux: Choose this option to base the mesh/results accuracy assessment on the heat flux results.
  • Temperature: Choose this option to base the mesh/results accuracy assessment on the temperatures.

• For Thermal Stress studies: The choices for this analysis type combines the previously listed and defined Static Stress and Thermal options.