15 Replies Latest reply on Jun 20, 2018 11:08 AM by Bill McEachern

    Solidworks simulation

    Chuho Lu

      In solving an interference problem I saw the resulting stresses are beyond the material yielding.

      I switched the modeling to nonlinear by assigning the plasticity-von Mises to the material, the analysis failed.

      Can Solidworks simulation handle this kind of problems?

      Any helps are appreciated!

        • Re: Solidworks simulation
          Ryan Dark

          Hi Chuho,

          Yes, SOLIDWORKS Simulation can handle such problems but typically it is more difficult to stabilize a system to solve in nonlinear analysis than it is in static linear.  You may want to post up a Pack and Go .ZIP of your files with the static and nonlinear setups in them and people on the forum can help find why your particular nonlinear study is failing to solve.

            • Re: Solidworks simulation
              Chuho Lu

              Ryan,

              Thanks. I have attached the zip file.

              I could not include the cwr files in the attachment because of the file size.

              The model basically includes the small interference between shaft and sprocket hub, and bigger interference between pins and shaft/hub before loading apply.

              The pins are type of C-pin in another C-pin with No-penetration fit.

              Material: Pin-55Si7, Shaft: 42CrMo4 and Sprocket: C45.

              The sprocket's teeth (120 degree) subject to a total normal force to the teeth of 35kN while the shaft is fixed.

              I use bilinear modulus for the material to capture the plastic behavior,

              Please let me know if any further information is need. Thanks again.

              Chuho

            • Re: Solidworks simulation
              James Riddell

              There is more to non-linear analysis than just changing the material properties.

              I presume that you do have a Simulation package that includes non-linear, correct?

              Can you describe your set-up in more detail?  Are the parts interfering prior to the start of analysis (i.e. interference fit bushing/bearing) and thereby under initial stress?  Or are you looking at a non-penetration connection that gives high stress?

              Is there a quick hand calculation you can do as a sanity check?  Is it a mesh refinement or geometry anomaly?

                • Re: Solidworks simulation
                  Chuho Lu

                  James,

                  Yes, my Simulation package has the non-linear module.

                  After running the linear static, I made a study copy to the nonlinear static analysis.

                  I then choose plasticity-von Mises model, give each material a tangent modulus.

                  In solution set-up, choose autostepping with initial time increment 0.01, use large displacement formulation and Direct sparse solver.

                  Also choose "Force" control, "NR" iterative technique, and set the step/Tolerance options to be 1, 20, 0.001, 0.01, 1.

                  The parts have initial interference between the hub and shaft, and between pins (in Pins) and hub/shaft. I have attached the model to my previous reply to Ryan. Hope you can open it.

                  I was not able to make a quick hand calculation for a check.

                  Thanks again!

                  Chuho

                    • Re: Solidworks simulation
                      Bill McEachern

                      In my experience the shrink fit doesn't work in with an NL solve or at least I have never gotten it to work. You may have better luck by applying a force or pressure (get an idea of what's required from the linear analysis by looking at the contact pressure plot - then double the peak value it has to be sufficient so that the parts come out of contact) to the part that doesn't go beyond yield (i.e. has a linear mat model) and then relaxing the force to engage the contact. I have not looked at the model. I would use initial steps of 1 (time curve would go from 0,0 to 1,1 to 2,0). Auto stepping on. Everything else at the defaults.

                        • Re: Solidworks simulation
                          Chuho Lu

                          Bill, thank you for the suggestion. Chuho

                            • Re: Solidworks simulation
                              Janko Stellaard

                              The model is unstable due to unconstrained parts (rigid body motion).

                               

                              In the static study you have applied soft springs to stabilise the model. This option constrains all rigid body motion of unconstrained parts by the use of very soft springs.

                               

                              In nonlinear this option isn't available, and that is why your nonlinear study fails.

                               

                              You should check all the constraints in your static set-up and get it to work without the soft springs option.

                                • Re: Solidworks simulation
                                  Chuho Lu

                                  Thanks for the comments.

                                  I did check "Use soft spring to stabilize model" in static study and experience no problem to obtain static solution.

                                  I also added necessary constraints to the model in the nonlinear study to avoid rigid body motion, but solution fails.

                                    • Re: Solidworks simulation
                                      Janko Stellaard

                                      yes, but uncheck the soft springs option in the static study. If it works then switch to nonlinear.

                                        • Re: Solidworks simulation
                                          Bill McEachern

                                          Janko,

                                          have you ever successfully solved a interference fit contact with the NL solver? If so you are a better man than me or at least more persistent. I have not attempted it in a few years but prior to that I had no luck.

                                            • Re: Solidworks simulation
                                              Janko Stellaard

                                              Bill,

                                              I assumed that it should/would work, but you made me doubt that. So i have tested it. In the attachment there is a file with a working nonlinear study in combination with the shrink fit contact.

                                                • Re: Solidworks simulation
                                                  Bill McEachern

                                                  I could not open it so I take it is in the 2018 version. Any chance you could run it in an earlier version?  I know it could be asking a lot so no issue if its too much trouble.

                                                    • Re: Solidworks simulation
                                                      Janko Stellaard

                                                      I performed a nonlinear study with a shrink fit  on the wheel assembly model from the exercises of the Simulation Basic training manual. I have used 1/8 model, so there is only symmetry, no other fixtures. \

                                                       

                                                      It works fine with the initial model. When I increase the overlap between the bodies I get solver messages that plasticity in the first step is detected and the loads should be applied gradually. I guess that in case it is better to start with a prescribed displacement in several steps, and then change the prescribed displacement to 'off' to reach a new equilibrium.

                                                       

                                                        • Re: Solidworks simulation
                                                          Bill McEachern

                                                          I modeled up a shaft and hole using quarter symmetry and it worked similarly in 2017. Making smaller steps doesn't do anything to get the error message to go away as it solves the plasticity with out issues so there is no reason to cut the increment near the final aspect of the shrink. I would have to run the same problem in Abaqus to find out what they are concerned about with respect to results. So I would say it still doesn't work even though it now solves. I would suspect that is you try it with out having it modeled with quarter symmetry it might have trouble. I would suggest that the OP try it with artificial restraints to ensure it is not sloppy and see if that works with the plasticity error. Then remove the restraints in a subsequent step - that was supposed to have been implemented a while ago where you can deactivate a restraint but I haven't tried in quite sometime and it never worked when I did.

                                                          The other option is try it the other way and skip the shrink fit contact definition and just use the surface to surface contact with a squeeze and then a let go in two steps.

                                                  • Re: Solidworks simulation
                                                    Chuho Lu

                                                    Just did it. Got the same results. It's OK for getting the static solution but not NL part. Thanks.