Refining the mesh

The accuracy of an FEA solution is highly dependent on the quality of the mesh. If the mesh is too distorted or coarse near stress concentrations – the results can be skewed. Inventor Nastran provides users a variety of mesh controls and settings to refine the mesh to an acceptable level.

Review and impact the element quality

Once a mesh has been completed, the FEA program should be able to provide information on the quality of the elements. That is, for instance, if you have quad shell elements, you would like them to ideally be uniformly square vs. very long and very narrow rectangles.

In Inventor Nastran, you can access the option to Check Quality For Mesh from the Mesh Model node in the Model Tree.



The checks that can be performed for tetrahedral elements are shown below.



The program will indicate if there are elements that fall outside the ideal ranges. If so, the easiest way to change up the elements is probably to re-mesh the geometry – and that can be done on a global or local level.

Control the global mesh size

Most FEA programs will choose a default mesh size; however, this should generally be considered a starting point. As was just discussed, if the element quality needs to be improved – or if you are working on ensuring a converged mesh (discussed a little later) – one of the easiest things to do is to just change the global mesh size. 

Many FEA programs will allow you to adjust the size by a percentage or by an actual element size (absolute mesh sizing). It might be convenient to consider a known dimension of your model and set the absolute mesh size in comparison. For instance, if your geometry is 1″ thick and you know you want to perform the first analysis with three elements through thickness, then you can set the mesh size to around 0.33″. 

When changing the global mesh size, keep in mind that you are impacting the overall mesh of the model. When the object you are meshing is a solid, if you are reducing the global mesh size, the internal elements are also being reduced. If you have a part with a very large surface area or a very large volume, small changes to the overall mesh size can result in surprisingly large increases in element and node count. 

When globally reducing the size of mesh does, or will, result in too many elements to practically analyze within a reasonable amount of time, consider switching to a local mesh refinement.

Local mesh refinement

Most FEA programs will allow you to select a face/surface, edge, or vertex and specify that you want to increase the mesh density in that region. You can repeat this process in different regions of the model to obtain the finer mesh in just those locations where you need. 

In addition, you generally have access to advanced mesh controls that allow you to control mesh items, such as:

  • Controlling the growth rate from the smaller elements to the unrefined larger elements.



  • Controlling the placement of the midside nodes (or creating curved geometry).



While examining the model globally, these controls act locally at regions that meet the conditions for refinement.

It is worthwhile exploring the advanced meshing features and local controls to refine your mesh. These can help you get an improved mesh where needed, without impacting the mesh count as much as global refinement.

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

Refine the mesh - Exercise

  1. Open the Arm_Refine.ipt part file from your working folder. 
  2. In the Environments tab>Begin panel, click Autodesk Inventor Nastran. 
  3. In the Autodesk Inventor Nastran tab>Mesh panel, click Generate Mesh. 
  4. Once the mesh is generated, in the Mesh panel, click Mesh Settings. 
  5. In the Mesh Settings dialog box, change the Element Size (mm) to 110, then click Generate Mesh.



  6. Once the mesh is generated, click OK to close the Mesh Settings dialog box. 
  7. In the ViewCube, click the FRONT view and zoom in to the hole. 
  8. In the Mesh panel, click Mesh Settings. 
  9. In the Mesh Settings dialog box, click Settings. 
  10. In the Advanced Mesh Settings dialog box do the following: 
    1. In the Midside Nodes area, select the Project Midside Nodes option. Click OK. 
    2. Change Max Element Growth Rate to 1.2.



  11. Select OK. In the Mesh Settings dialog box, click Generate Mesh. Note that the mesh now conforms better anywhere that the geometry is curved. 
  12. Click Ok in the Mesh Settings dialog box. 
  13. From the Mesh panel, click Mesh Control. 
  14. In the Mesh Control dialog box, in the Face Data area, click inside the Selected Faces field. 
  15. Select the faces shown in the image below (face<4>, face<18>, face<19>).



  16. Change the Element Size (mm) to 25 and click OK.



  17. In the Mesh panel, click Generate Mesh. 
  18. In the Nastran Model Tree, right-click on Mesh Control 1 and select Edit.



  19. In the Mesh Control dialog box, change the Element Size (mm) to 10 and click OK. 
  20. In the Mesh panel, click Generate Mesh. 
  21. Save the model.