Use the mesh convergence settings to refine a mesh during analysis, either globally for an entire part, or locally in areas of complexity with more mesh errors. Click Convergence Settings in the Mesh panel of the Autodesk Inventor Nastran ribbon. To restore default refinement values, as shown in the figures below, click the Reset button at the bottom of the dialog.
Global Refinement
This type of convergence results in a uniform mesh size throughout the model.
Maximum Number of Refinements specifies the maximum number of h refinement cycles for convergence. Default value is 5, and increment is 1. Refinements can cease before reaching this number if the stop criteria is reached.
Stop Criteria (%) sets a minimum percentage value for the difference between subsequent refinement results. If the value is less than this minimum, the refinement stops. Results to converge are von Mises stress.
Error Threshold (0 < value < 1) is a value between 0 and 1 that stops the refinement if the calculated strain energy error is less than the specified threshold value. Trial and error is generally used to arrive at a suitable value.
The strain energy calculated based on the following equation and compared with the error threshold value.
Error = sqrt(seerr/setot)
seer = Strain energy error
setot = Total strain energy + strain energy error
For setting the error threshold value, it is recommended to run the first analysis with a threshold value of 0.01. After the analysis runs, check the Convergence Plot display on the Results panel; for the next convergence run, set an error threshold value less than the error value shown in the Convergence Plot. Doing this should result in improved global refinement.
Local Refinement
This type of convergence is based on the input refinement threshold value. Here, the critical areas with maximum errors will be subjected to refinement.
Maximum Number of Refinements specifies the maximum number of h refinement cycles for convergence. Default value is 5, and increment is 1. Refinements can cease before reaching this number if the stop criteria is reached.
Stop Criteria (%) sets a minimum percentage value for the difference between subsequent refinement results. If the value in results is less than this minimum, the refinement stops. Results to converge are von Mises stress.
Refinement Threshold (0 to 1) is a value between 0 and 1 that determines the number of elements with maximum errors to consider for refinement. A setting of 0 would include all elements, while a setting of 1 would include none. The default of 0.95 means that refinement is applied to the top 5% of elements with maximum errors.
Refinement Factor (> 1) controls the growth rate of elements in the critical regions for each refinement run. For example, a value of 1.5 means the percent of elements specified in the refinement threshold will increase by 1.5 times for each refinement. Refinement factor works closely with refinement threshold. If the threshold is closer to 1, try a lower refinement factor of 1.25 to 1.75. If the threshold is closer to 0, try a refinement factor of 2.0 or more.
Include in Analysis checkbox
This box must be checked to activate mesh convergence (either global or local) and run refinement iterations.
Notes
- Mesh convergence works only for Linear Static Analysis, it's not supported for other analysis types.
- Mesh convergence works only for Tet elements; for shell elements and 1D elements, mesh convergence does not work.
- It is recommended to use parabolic mesh for refinement.
- For local refinement, the default mesh size is recommended; for global refinement, start with a coarse mesh size
Convergence Plot
After running an analysis that includes mesh convergence, this plot is included in the Results panel of the Autodesk Inventor Nastran ribbon.
The dynamic plot shows the following details:
- If convergence was achieved, the number of refinements or steps required for the solution to converge.
- The von Mises stress values associated with each refinement.
- The convergence rate in the form of an XY plot and a percentage value.
- The strain energy error, which is useful for determining the error threshold for global mesh refinement.