With your mesh improvements are the displacements converging? If so, probably singularity. Looks like a standard case to me.
It sounds like you have some physical testing data or hand calcs, do the displacements match? I'd so, probably another indication of singularity.
Jared said the magic word. You have to check whether the stress is converging. Run the simulation at 3 or 4 element sizes which drop by the same factor, (e.g., [.8, .4, .2, .1]. As the element size shrinks, the approximate error must also shrink. The approximate error is the difference between the calculated stress at each element size.
So [s(.4) - s(.8)] > [s(.2) - s(.4)] > [s(.1) - s(.2)]
If this relationship is true, your stress is likely real, and you have to decide whether it matters. Sometimes high, very localized stresses are real but won't cause failure. On a shaft, though, they may lead to fatigue.
If this relationship is not true, but the stresses are all very close to each other (within a few percent), the stress is still likely real. If this relationship is reversed, the stresses are not real, and you have a singiularity. But there should not be a singularity at a fillet.
Jared and Mike are right about what you should do to check this out. Just looking at your pictures, I would expect to see a substantial stress concentration, because you have a very small fillet compared to the shaft diameter and a large step in the diameter, so I suspect that the stress you are seeing is real. Because the stresses are not that high and are localized, I would not expect you would be able to see the permanent deformation that is taking place. I also wouldn't expect any cracks, as 304 that soft should have more than 50% elongation.
You mention "For the mesh control of 0.1mm and 0.5mm, results are almost the same".
Are you talking about stress? If stress continue to rise with finer mesh then it's probably a singularity, if not, you need to look more into this.
First of all, you have fixed the complete back surface on the connection plate which makes it stiffer than what you would see if you used bolt connectors. This can affect the result and is one way to proceed with the analysis. Otherwise you should include the "next level" of parts, use contact, and try again.
If you still see high stress concentration you should do a NL analysis (plasticity von mises) to decide if you can live with it or not.
Localised yielding can occur without any cracks or visible problems on the part if the material is ductile. The load will be redistributed to the surrounding structures when the stiffness of the material change due to yielding.
But if you have cyclic loading, there is a risk for fatigue, and ductile behaviour is also highly dependent on temperature.
Followings are the results I got with mesh controlls.
No Control (4mm element size) - Max Von Mises Stress 41.5 Ksi, Max Displacement 0.03218mm
0.8mm Mesh Control - Max Von Mises Stress 47.3 Ksi, Max Displacement 0.03219mm
0.4mm Mesh Control - Max Von Mises Stress 46.6 Ksi, Max Displacement 0.03220mm
0.2mm Mesh Control - Max Von Mises Stress 48.1 Ksi, Max Displacement 0.03220mm
0.1mm Mesh Control - Max Von Mises Stress 47.5 Ksi, Max Displacement 0.03220mm
Does this mean the stress is real?
I have a feeling that there is a high stress concentration at the fillet as shown in the FEA but doubt whether the value shown by SolidWorks is accurate.
It looks like your stresses converge with reduced mesh size so the stresses in your model are real. But, as Mikael Martinsson said above, because you fixed the entire back of the flange your model may be stiffer than if you attach the flange to the wall with bolts. Thus, you may be seeing higher stresses in your model than in reality.
Try using a virtual wall and bolt connectors with the designed preload to constrain your part instead of the 'fixed' constraint on the back surface of the flange.
only way to know if it is accurate is to test it or compare against a known solution.
have you done the test that mike suggested yet?
looks pretty converged to me but I would suggest evaluating what mikael has said as well as peter. it is a good exercise to see how the BC affects both displacements and results. it is one of the main topics we teach in our one-on-one mentoring.
Well, it looks like converging stress then.
I don't know the dimensions on the part, but you mention d=17 mm for the axel.
48 Ksi (331 MPa) is your maximum stress in the radius.
Stress concentration factor used in hand calculation, can give you a hint.
If I guess that you have r=1 mm and axel d=17 mm then r/d = 0,06
If i then guess that the larger D is about 2,5 x d then the Kt for this case is about 2,2
This means that the bending stress in the axel should be about 22 Ksi (150 MPa).
Now, since you use the continous plot instead of the discrete it's hard to say if this is right since 20 to 30 Ksi = green blurr.
But if you have all dimensions, you could verify your results with hand calculation of a cantilever beam in bending.
Here is a link with several stress concentration cases: http://www.mae.ncsu.edu/eischen/courses/mae316/docs/Appendix_C.pdf
Mikael, thanks for your link. I manually calculated the stress concentration and the value is 45.8 Ksi which is almost similar to the FEA value.
I also ran with bolt connections and a vertual wall but results were almost same to the previous values.
So I'm pretty convinced that this is a real stress. Thanks everyone for helping me in this.