Hi Jimmy,
I will try to answer your question in two parts, since static stress and modal computations can be quite different.
For a static stress analysis, there are a couple things you can check for results validity and mesh independence:
1) The reaction forces need to be equal (in magnitude) and opposite (in direction / sense) to the applied loads. You can check this by accessing the Reaction Forces dialog via the right mouse click context menu on a constraint in the browser. This is the first thing I check. It can also indicate whether the model is constrained properly in the case of a zero reaction load appearing in a particular direction, when it is expected to restrain loads in that direction.
2) As you mentioned already, the mesh refinement can be a major influence on the stress results (most notably at and near a stress singularity / sharp 'inside' or re-entrant corner in the geometry). However, the Displacement results should remain mesh density / refinement independent.
That is to say, the convergence plot of the maximum stress can be diverging, yet the displacements converge. This is indicative that you have a stress singularity in your model and the stress results are 'meaningless' at that particular location in the model / simulation.
After a solve (whether or not a non-zero h-refinement is conducted) I usually launch the Convergence Plot to view the stress and displacement solution step results, to ensure I have a converging solution or if a model singularity exists that I need to either ignore or correct.
In some cases, you may be able to 'cure' a singularity by adding a small fillet at the sharp inside corner...
For a modal analysis the displacements are relative. That is to say, the actual displacement result values are meaningless (e.g. x.xx mm) since those would depend on time-varying excitation loads in 'real-life' are which are not possible to include in a static stress analysis. These 'displacement' results are to give a general indication of the relative displacement magnitude of that particular part of the model, for that particular mode shape.
However, we allow you to converge results on a particular modal frequency. In the Convergence Settings, if you set the stop criteria % small enough (after solving) you can use the Convergence Plot to convince yourself that further mesh refinements will not change the computed frequency (image attached to show an example). This is the approach I would take for those two mode shapes you mention vary with changing the mesh density.
I hope this helps answer your questions! As always, please keep the questions and comments coming 🙂
Best regards, -Hugh
[Edit: fixed a typo / moved a paragraph around for better reading]
Hugh Henderson
QA Engineer (Fusion Simulation)
![Autodesk Design & Make Report](https://forums.autodesk.com/t5/image/serverpage/image-id/1350519iCB55845EBFC43016/image-size/large?v=v2&px=999" "Autodesk Design & Make Report")