I have a very simple geometry which I have applied forces to on some of the openings and on the internal walls. I have repeated the simulation with a finer mesh on each iteration but I fail to get the stress results to converge, I have read some of the online articles on what metrics to look out for to determine if the mesh quality is sufficient and I think my mesh is generally ok, except my skewness.
Would it be possible to get advice on if my CAD model is the issue which is not giving me mesh independent result or is it my mesh quality that’s the issue?
For mesh convergence analysis, we do not generally refine all the mesh, but instead identify the location of interest and refine the mesh around this point. locally. Please try and implement such strategy in your model.
I would also keep the following into mind:
As you have a thin-waled model, you need more points across the thickness to properly capture bending deformations. Please specify manual size for your base mesh, so that you have at least 4 points across the thickness. You can achieve this with your 2nd order mesh + a maximum edge length half the wall thickness.
Your multi-part assembly needs bonded contacts, which are automatically created. As the mesh is non-conformal, these contacts can create stress concentration points. To avoid this numerical artifact, please fuse all the parts together. You can do so in the CAD Edit Mode with a Body - Boolean - Union operation.
So I have made the body unified and removed the contacts, I have set the mesh to manual with a maximum edge length of 10mm, which is half of the thickness of the 20mm plates.
But I’m not sure what I need to do to check if the stress values are mesh independent, how do I refine the mesh further to check this?
Also I note my maximum skewness is quite high, should I be concerned about this?
Don’t worry about the skewness for FEA simulation, just the aspect ratio.
To measure the convergence of stress, pick a point with high stress and use a Result control item - Point data at that location and measure the von Mises stress. Then repeat with a local refinement of the mesh.
I’ve set my mesh settings as advised and my plan is to reduce the local element size by 0.001m for result validation, but it’s taking quite a while for each iteration to simulate, am I going about this in the correct way or do you have any suggestions that I can be more efficient?
Only suggestion I have is to apply the mesh refinement only to a small region, perhaps using a Region Refinement in combination with a Sphere primitive, centered at the point of interest. If the sphere is relatively small, your mesh size shouldn’t increase too much at each iteration.
The radius of the sphere looks to big for me, considering it should cover a stress concentration region, which in principle is small.
If the mesh is too large, your simulations will run out of memory. You will need to compromise on convergence, or reduce the mesh size (maybe pulling back to 1st order).
