9 Replies Latest reply on Apr 8, 2013 11:48 PM by Nilanga Gamage

    High Stress Concentration of a fillet

    Nilanga Gamage

      Hello Everyone,

       

      I have done the FEA for a loading fixture and found high stress concentration at some areas as shown below. (Shaft Diameter is 17mm)

       

      Material - 304

      Yield Strength - 31.5 Ksi

      Load - 250 Lbf (1112N)

       

      Max Von Mises Stress is 47.6 Ksi and it's larger than the yield strength of the material.

      sdfsdfd.JPG

      I also used the following mesh control for this

       

      Mesh Type - Curved Based Mesh, Max element size: 4mm, Min element size: 0.8mm

       

      0.1mm mesh control at the fillet as shown below.

      Mesh Control.JPGsdfsdfs.JPG

      For the mesh control of 0.1mm and 0.5mm, results are almost the same. When I see through Iso Clipping, I could find that it's only the outer surface of the small fillet where the stress is greater than 30 Ksi as shown in the above figure.

       

      I know I can eliminate this by adding a lager fillet but I doubt whether this is really happening in the real world. I am already using a machined part with this configuration. I have also applied loads little larger than 250Lbf to the part cannot see any cracks or permanent deformation of the .

       

      I need to know whether FEA shows approximately real values or this is a stress singularity that can be ignored. Pls advice me.

       

      Thanks,

      Nilanga

        • Re: High Stress Concentration of a fillet
          Jared Conway

          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.

          • Re: High Stress Concentration of a fillet
            Mike Pogue

            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.

            • Re: High Stress Concentration of a fillet
              Jerry Steiger

              Nilanga,

               

              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.

               

              Jerry S.

              • Re: High Stress Concentration of a fillet
                Mikael Martinsson

                Nilanga

                 

                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.

                • Re: High Stress Concentration of a fillet
                  Nilanga Gamage

                  Thanks everyone,

                   

                  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.

                   

                  Any idea?

                   

                  Nilanga

                    • Re: High Stress Concentration of a fillet
                      Peter Biggert

                      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.

                      • Re: High Stress Concentration of a fillet
                        Jared Conway

                        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.

                        • Re: High Stress Concentration of a fillet
                          Mikael Martinsson

                          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

                        • Re: High Stress Concentration of a fillet
                          Nilanga Gamage

                          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.