Hi Jason,
I can reproduce the issue with the models you provided. There are a few issues going on, which I'll try to explain, some might seem rather surprising. This is not an issue with our particular software, all FEA packages behave similarly in this regard.
1) You've noticed that the maximum stress at the sharp corner is different for the two models. Even though the models appear identical, in fact they are slightly different. They are dimensioned slightly different and the collection of lines were created slightly different. Although this doesn't seem to matter, it actually does in CAD / FEA. Each sketch line has a direction, as does each edge. Even though the CAD models look the same, internally they are not.
2) The stress results are highly dependent on the mesh. Since (internally) the models are slightly different, the meshes are slightly different, and thus the stresses slightly different. Reason being is that meshing algorithms start at one "end" of the part, and starts discretizing the model into finite elements by splitting edges, etc. If the parts are (internally) slightly different, the meshing algorithm may start at a different end and the meshes will be a little different. Notice that the number of nodes and elements are not exactly the same between the two models.
Even the processor can play a role in the resultant mesh, as you have noticed. An x64 machine will have more digits than an x86 machine in the calculations, so the mesh will end up different, which again...you can witness by the different numbers of nodes and elements, even if it is the same exact model (file).
3) If we are comparing the stress results at a singularity, or stress concentration, it is not a valid comparison. In "real-life" the part has to be manufactured, and the sharp 90 degree edge couldn't exist without some small fillet, whether machined or cast, one reason, since cutting tools do not have a perfectly sharp 90 degree profile.
In a singularity case, even in real-life, the closer to the root of the sharp inside corner, the higher the stress goes, until an infinite stress is reached. This makes sense, since stress (or pressure) is force divided by area, and as the area gets infinitly small, the stress (or pressure) gets infinitely large. This is the case with FEA.
There are p-refinements and h-refinements. With a p-refinement, we increase the degree of the polynomial of the element. Meaning, P1 is a linear approximation, P2 is parabolic, P3 is cubic, etc. h-refinement means we increase the number of elements by creating more, smaller and smaller elements. If we increase the number of h-refinements, you'll see that at a singularity, we can never converge, we will always diverge. This is why we need to add some size fillet to inside sharp corners so we don't get misleading, diverging results. Also, for the fillet face, the mesh should be refined enough so you get at least two "rows" of elements. Meaning we need nodes near the midpoint of the fillet arc. Also, elemnts with a high Jacobian, or aspect ratio should be avoided since they are too distorted. This gets into shape function theory, which is beyond the scope of this thread so far...
An article describing the situation of stress singularities is here: http://www.tech.plym.ac.uk/sme/mech335/feaerrors.htm
Here is an article describing this scenario. Please see "Part 3: Building Better FEA Models" http://machinedesign.com/article/good-solid-modeling-bad-fea-1115
Our suggestion in this case is to add a small fillet (I used 0.5 mm) and use convergence with h-refinement = 3 and Stop Criteria = 3% to get comparable results between different machines.
I hope this helps!
Best regards, -Hugh
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")