I don't know the direct answer to your question, but I'll try to add some light, if possible.
- If this is axisymmetric, I strongly recommend you move to an axisymmetric model. This will allow you to refine the mesh a lot further. It will solve much faster. It will also automatically slice the model.
- It's not enough to refine the mesh as much as you can. You have to compare the solutions at different mesh sizes and satisfy yourself that the solutions are not changing. Convergence is much more sophisticated than that, but I don't want to dig into it.
- The solution at the reentrant corners has no physical interpretation. Please do not use it for anything or compare it to anything. It will not converge.
- The solution at the fillets is the hot spot stress. You have explicitly calculated what would have been the stress concentration factor in a hand calc. The hot spot stress is real, and physical, but it can usually be ignored in non-fatigue situations.
- If the stress is cycling, and in a pressure vessel it probably is, you are in a fatigue situation. Fatigue analysis is a whole layer of analysis that I can't lay out in a forum.
- Far from the corners is the nominal stress. What constitutes far from the corners is a little tricky. This is the stress your should compare betwixt the two solutions. It should be pretty close, unless the fillets are really big, in which case, you have different geometries and it's not clear to me how they should relate. I'd need to take a pretty hard look at it.
- Look in Roarke to see if you can find a case to model this by hand.
PS: There is no such thing as a sharp corner. Using Axisymmetric and/or submodeling, you should be able to explicitly model the machined corner. .0002 in radius is a reasonable guess. There are other ways to get the stress at the corner, such as linear extrapolation of the stress walking up to the corner before it goes non-linear.
If you were able to refine the mesh at the sharp corners the stress would continue to rise towards infinity. (Assuming that you run a linear analysis.) The fact that it happens to be less with the particular mesh you have is immaterial. As several people have pointed out, you need to run progressively finer meshes near the high stress points to make sure that you are getting converging values of stress for the filleted part.
did lisa and solidworks sim come out with similar results? i can't tell
have you already done mesh convergence checks?
if you ignore stress at first, are the displacements converging? what do the displacements look like? are they reasonable?
you will want to do some more research on singularities or have someone take a look at your setup. we do this for customers quite often as part of our mentoring service.