You get a few stress singularities on the edge between the face with fixture and the face with load. It seems like the results converge for the rest of the part, but stress hot spots will never reach convergence. In reality these hot spots will converge, but in the software they will increase exponentially in value with finer mesh.
Here we see that the curve is rapidly increasing after refinement. I made a Iso-clipping plot to show that it only occures on a few points along the edge mentioned.
In this case, you should add the part that the rightmost fixture represent to make your study more realistic. It is not recommended to have fixtures close to areas in intrest of stress calculations. This will make the model less rigid, and would help you to get rid of the singularities.
So a better approach is to make the part closest to the force area. First I extrude to component the holds the shaft, as a separate body. Create a small fillet on the inner edge of the hole to remove the sharp edge (it will cause stress singularities as well).
Then in the study I add component control and make a global contact set with No Penetration. For meshing you cannot use p-adaptive mesh when there is this type of contact set. But h-adaptive is fine, and also the adaptive mesher I would recommend to use in most cases anyways. I would use the curvature based mesher to get better mesh for the fillet face. Click run a few times to go through some loops and the result is converged von mises stress.
Most of the times I don't use adaptive mesh, but create a couple of duplicated studies with mesh control to increase the accuracy of stress calculations. Compare the results and decide if the stress changes is small enough.
On a side note I recommend that you check out the new webcast series on youtube; Simulation Step-Up from SolidWorks.
Yeah great thanks a lots