Converging the mesh

Converging the mesh is the process of iteratively reducing the mesh size, where required, to ensure the proper results are calculated.

As mentioned earlier, the mesh represents your geometry when the analysis is performed. In general, the more elements in a mesh, the more precise a solution will be – as the finer mesh is better able to capture the details of the geometry and represent the stiffness of the model.

Why not just use a really fine mesh and be done with it? A single solution gives you a single data point, which may be accurate or could be flawed due to something like a few poorly shaped elements or a singularity. Performing two iterations might provide reasonably different results, but which is correct? Continuing to refine the mesh to find three or four results should provide a trend.

Note that there will be a practical limit where further mesh size reductions add no benefit to the solution. At this point, you are adding elements and taking time to analyze a model with no significant change to the results.

The goal is to find where the percent change in stress or strain between changes in mesh sizes reaches an acceptable limit. Remember there are already many other assumptions in play – about the geometry, boundary conditions, material, the finish – so don’t fall into an “analysis paralysis” trying to reduce it too much. You are finding the best solution for a given set of assumptions and conditions. Keep the goal in mind – you are minimizing the mesh-related change in results.

Any referenced datasets can be downloaded from "Module downloads" in the module overview.

Converge the mesh – Exercise

  1. Open the Arm_Converge.ipt part from your working folder. 
  2. In the Environments tab>Begin panel, click Autodesk Inventor Nastran. 
  3. In the Autodesk Inventor Nastran tab>Solve panel, click Run. 
  4. When the Nastran Solution Complete message displays, click OK. 
  5. Note that the Max result is about 60.42 MPa. Zoom in to the area to see that the stress in that area is on the edge between two elements, as shown below.



  6. In the Results panel, click Return to return to the setup environment. 
  7. In the Mesh panel, click Convergence Settings.
  8. In the Convergence Settings dialog box, set the following and click OK: 
    • Convergence Type: Local Refinement 
    • Maximum Number of Refinements: 5 
    • Stop Criteria (%): 5.00 
    • Refinement Threshold (0 to 1): 0.90 
    • : 1.50 
    • Select Include in Analysis 



  9. In the Solve panel, click Run.
  10. When the iterations are completed and the Mesh Convergence message displays, click OK.



  11. If the Convergence Plot graph closes, reopen it by clicking Convergence Plot in the Results panel. Note the results from the different solutions, then click the X in the top-right corner to close the graph.



  12. Save the model.