12 Replies Latest reply on Mar 26, 2013 10:16 AM by Jim Montgomery

    Modeling Fillet to reduce Stress Concentration

    Alec Chalmers

      I am attempting to model an cylindrical End Cap that is part of a titanium pressure vessel that has failed several times at pressures below what FEA predicted. The first parts were fabricated without fillets and failed catatrophically at the inside sharp corner. Of course the simulation results indicate a large stress concentration at this corner and I had indicated that a fillet would be required to avoid this concentration. I have now added a fillet in my model and still get very high stresses in the fillets and especially the tangent lines. What is the best method to model this type of feature in Simulation?

        • Re: Modeling Fillet to reduce Stress Concentration
          Jared Conway

          What does the mesh look like in that area? If it is a true singularity, the high stress will always exist. The only thing you can do is minimize it by using smaller elements and reading the stress 2-3 elements away from the singularity.

          • Re: Modeling Fillet to reduce Stress Concentration
            Bill McEachern

            I don't do this a lot but there are special shapes for end caps on pressure vessels. I would assume they are best being elliptical - that is to say the radius at the connection to the cyclindrical section is smallest there and extends to large and larger radii at the center. You sould google it. Well, this is from wikipedia entry:

            Theoretically, a spherical pressure vessel has approximately twice the strength of a cylindrical pressure vessel with the same wall thickness.[1] However, a spherical shape is difficult to manufacture, and therefore more expensive, so most pressure vessels are cylindrical with 2:1 semi-elliptical heads or end caps on each end.

              • Re: Modeling Fillet to reduce Stress Concentration
                Alec Chalmers

                I was treating titanium alloy Ti-6Al-4V as a ductile meterial, but it acts more like a brittle material. Does anyone have experience designing for titanium? From researching stress concentration factors some of the literature suggests that the most accurate method to mesh an inside radius is using 2D elements as this is an axisymmetrical shape. The standard Simulation add-in we have does not include this option. Otherwise there are several methods to calculate a stress concentration factor and make sure that the nominal stress near the fillet be low enough to avoud yielding at the radius surface.

              • Re: Modeling Fillet to reduce Stress Concentration
                Alec Chalmers

                Here is a JPEG of the Von Mises stress plot of the fillet being studied; notice the high stress valuea at the tangent lines of the fillet? I don't believe this is realistic, is there any way to avoid this?

                 

                LM End Cap, FEA.JPG

                 

                Thanks,

                 

                Alec

                • Re: Modeling Fillet to reduce Stress Concentration
                  Alec Chalmers

                  More information on this simulation; this is the result of 2 successive runs using the h-adaptive convergence option set at the max 5 loops, during the second run the simulation dialog indicated that the adaptive convergence had reached its goal. Here is a view of the mesh in the fillet region:

                   

                  LM End Cap, FEA.JPG

                  The mesh is tightened considerably in along the tangent lines of the fillet as represented in the previous VM plot.

                    • Re: Modeling Fillet to reduce Stress Concentration
                      Jared Conway

                      alec, can you post the model so that we can take a look at the BCs for the problem? or can you describe how the problem is setup?

                       

                      depending on the problem setup, if what you're seeing is a true singularity, the only way to deal with it is to improve mesh in the area and read results a few elements away.

                       

                      if the problem is because of a BC, you could move the BC away by adding another component to your model.

                        • Re: Modeling Fillet to reduce Stress Concentration
                          Alec Chalmers

                          Jared - this model is divided into a quarter of the full 360 deg axisymmetric part to take advantage of symmetry. The part is fixed on the inside flat surface that is tangent to the fillet radius and a hydrosttatic pressure of 6600psi is applied to outside flat surface that encompases the full diameter and the outside cylindrical surface immediately adjacent. The smaller diameter cylindrical surface is prevented from radial movement with a On Cylindrical Face fixture. The static study is run with the FFEPlus solver with h-adaptive convergence selected and the max 5 loops. I foud that the study had to be run twice in sccession to reach the h-adaptive goal, but the VM stress never converged, as indicated by the high values at the tangent lines. In the end, I am taking the average of the values near the fillet to consider when applying a stress concentration factor which in this case is around 3. I was hoping to find a  method that would approximate the results of manually calculating the stress concetration, I believe from reading that it possible with the 2D elements but I don't have access to that option.

                            • Re: Modeling Fillet to reduce Stress Concentration
                              Jared Conway

                              Hi Alec, can you post your model or a picture showing the setup? I'm not completely following but from what I understand, where you're seing the stress is not abnormal from an FEA perspective, they are at the edge of very stiff boundary conditions. What are they in real-life? Are they infinitely more stiff than the pressure vessel? Do they rigidly stop at the geometry you've selected?

                               

                              Regarding 2D, are you talking about 2D analysis or are you talking about shell analysis? Are you potentially talking about stress linearization in the pressure vessel study?

                                • Re: Modeling Fillet to reduce Stress Concentration
                                  Alec Chalmers

                                  To get a better grasp of the actual boudary conditions a more detailed model of the assembly of the end cap with the pressure vessel tube should be created with no penetration contact. I was trying to get a quick model and had iignored the stress concentration until failures in testing occurred. By 2D I meant using the 2D simplification option offered in the Simulation Pro version of this application, which allows much smaller mesh size without pushing the size of the model beyond the limits of most workstations.

                            • Re: Modeling Fillet to reduce Stress Concentration
                              Billy Wight

                              From the screenshots, it seems you do not yet have mesh convergence.  You're seeing higher stresses at the fillet tangent lines because SolidWorks is putting smaller elements there than it is in the centre of the fillet.  Try applying a local mesh control on the fillet and turning off h-adaptive.  Keep reducing element size at the fillet (and any other high stress areas) until the stresses no longer change.

                            • Re: Modeling Fillet to reduce Stress Concentration
                              Jim Montgomery

                              Alec,  Have you tried looking at the stress continuity across individual elements in the region of interest?  If it's discontinuous across adjacent elements then you'll probably need a finer mesh.  If not, maybe the element size is mathematically fine enough.

                               

                              This thing is a pressure vessel?  It looks like its meshed with tets.  How thick is it, could you use quad shells? 

                               

                              I ASSUME (always bad) that the structure is of uniform thickness in the region of interest?

                               

                              And my fav; got any failed parts????  What's the damn thing look like post real life badness?  What's the mode?