17 Replies Latest reply on Feb 4, 2015 1:40 AM by Mike Pogue

    torque simulation gets multi results with different fixtures

    Jing Liu

      I am trying to run a simulation on this small assembly: a copper stud inserted into a plastic housing (nylon 6/10), with no other restrains. Apply torque on the stud and run the simulation to see how much stress is generated by the stud on the housing.

      assem.pngassem section view.png

       

      1. I set a global non-penetration contact

      2. these following two surfaces are set as pin connectors

      stud face.pnghousing face.png

      3. 3.5 Nm torque is applied on the stud as:

      torque.png

      Now here comes the questions:

      when I set the fixtures like the following (the 4 side surfaces and the top surface of the plastic housing):

      fix all surface.png

      I got the result as the following (the max stress is about 197MPa):

      fix all result.png

       

      when I fix only the top surface of the plastic housing, like this:

      fix top surface.png

      I got the result as the following (the max stress is 350MPa):

      fix top result.png

       

       

      which one makes more sense? is there any other problem with my simulation input?

       

      thank you!

        • Re: torque simulation gets multi results with different fixtures
          Bryan Kohn

          The fixture should represent how the part will be mounted in the real world when it is being used. Think about how the part will be installed and identify the surfaces or edges that will be supported. Then apply your fixtures to those surfaces or edges. Hope this helps!

            • Re: torque simulation gets multi results with different fixtures
              Jing Liu

              thank you for your reply, Bryan. the plastic housing is clamped from both left and right surface and the stud is inserted into the housing without any other restrains, then the torque is applied to the stud. the result of the real test is: when 10 Nm torque is applied to the stud, we got safety factor of 1.9 for the plastic housing. I am trying to get the same or close result in my simulation.

            • Re: torque simulation gets multi results with different fixtures
              Mike Pogue

              I don't think either is reliable, but the first is better, because the second is almost certainly a phony singularity cause by the fixed surface touching cells that have to deform to react the contact. Even in the first one, though, you should do a convergence study, at least, before you buy off on the results. Even then, I'd take them with a grain of salt.

              • Re: torque simulation gets multi results with different fixtures
                Jared Conway

                1. don't look at stress to start, look at displacement

                2. why are you using the pin connector?

                 

                and like what was mentinoed above, use the restraints that match the physical situation

                  • Re: torque simulation gets multi results with different fixtures
                    Jing Liu

                    thank you for your reply, Jared.

                     

                    As I described above, the experiment was carried out as : the plastic housing is clamped from both left and right surface and the stud is inserted into the housing without any other restrains, then the torque is applied to the stud. the result of the real test is: when 10 Nm torque is applied to the stud, we got safety factor of 1.9 for the plastic housing.

                     

                    1. What information should I look for when looking at the displacement? I mean, how should I interpret the plot of the displacement?

                     

                    2. for the pin connector, to be honest, I am not sure about this part. I am still struggling with the parameters setting up for the simulation for this project. Let me modify the input as the followings:

                         a. Global non-penetration connections

                         b. fix the left and right side of the plastic housing

                         c. set the bottom face of the stud as: fixture->on flat faces->normal to face 0mm

                         d. set the surface of the stud (shown as the following pic) as: fixture -> on cylindrical faces -> radial 0mm, axial 0mm

                                   stud face.png

                         e. torque applied to the stud as 10Nm

                    *************************************************************************************************

                    Here are the results I have got from the above inputs:

                    1.the displacement:

                    disp.JPG   dis2.JPG

                    2. the stress:

                    stress.JPG

                    3. the safety factor:

                    fos.JPG

                     

                    the satety factor plot doesn't make sense at all

                      • Re: torque simulation gets multi results with different fixtures
                        Peter MacDonald

                        I'm not sure if you really want that radial fixture on the stud. It'll surely reduce the effect of the torque.

                         

                        For displacement, you should monitor the maximum displacement whilst refining the mesh. Once the maximum stops changing your solution has converged, i.e. your mesh is suitably refined. Monitoring max stress is more difficult due to the frequent occurrence of singularities which provide false stresses.

                        • Re: torque simulation gets multi results with different fixtures
                          Jared Conway

                          I'm not clear on where you are still stuck or how you are having trouble looking at the displacements.

                           

                          I recommend you post your models and elaborate further on the trouble you're having.

                           

                          I also assume that you aren't getting any errors when running simulations that you are ignoring.

                            • Re: torque simulation gets multi results with different fixtures
                              Jing Liu

                              Thank you for the suggestion, Jared. Here is the assembly file that I used for this simulation.

                                • Re: torque simulation gets multi results with different fixtures
                                  Jared Conway

                                  what exactly is the open issue?

                                    • Re: torque simulation gets multi results with different fixtures
                                      Jing Liu

                                      Hi Jared, it looks like I am having more open issues than when I first posted this problem here because I have received so many suggestions and comments. Anyhow, my open issues currently are :

                                       

                                      1. I have eliminated the pin connector and attached my model. Do you think I have the right inputs for all the boundaries, connectors, loads, etc... ?

                                      2. As Peter suggested above, I used three different meshes to run the simulation and the max values of displacement are different. And I couldn't run it with a finer mesh(the calculation corrupted). What should I do? How can I tell that the solution has converged?

                                       

                                      Thank you!

                                        • Re: torque simulation gets multi results with different fixtures
                                          Jared Conway

                                          1. only you can tell us what the right setup is. do you have a detailed description of what the device is, what your goals are and what assumptions you are ok with and expected results?

                                           

                                          2. i'm not sure whaty ou mean by corrupted but how different are the displacements? are we talking 1% or 10%?

                                          • Re: torque simulation gets multi results with different fixtures
                                            Mike Pogue

                                            Jing,

                                             

                                            I feel your pain. Convergence is a very sticky issue in some geometries, which is why some very smart people ignore or wave their hands at it.

                                             

                                            The solution has converged when the solution becomes insensitive to your choice of mesh size. If you get dramatically different solutions at different mesh sizes, then none of the answers can be shown to be correct. You can check this qualitatively, by comparing the solution at different mesh sizes and deciding that the difference is acceptable, or you can check it rigorously, using the Richardson extrapolation.

                                            Where qex = the "exact" solution, qh1 = the solution at mesh size 1 (h1), qh2 = the solution at mesh size 2, etc. If you were to use this equation, you'd have to produce 3 solutions, at 3 different mesh sizes h1, h2 and h3. h1/2 has to equal h2/h3, for instance, you might make solutions at .1 , .05 and .025. I usually do 4 solutions, and compute 2 Richardson extarpolations from them. The second step is to compute the convergence parameter, P. Assuming the solution is converging like 1/h^P, you can convert P as the slope of Log(h)/Log(qh-qex). If P is negative, the solution is NOT converging. If P is positive, the solution is converging, and qex is the answer.

                                             

                                            Now, if the solution is not converging because of singularities, you have to move far enough away from the singularity that the solution is converging at the point you measure. You cannot compute the stress at the singularity directly. What you can do, if this is not a fatigue situation (which it isn't), is extract the linear component of the stress, by plotting the stress leading up to the singularity, like this. The linear extrapolation evaluated at the singularity, is the nominal stress, subject to some sensitivity study.

                                            linear.PNG