9 Replies Latest reply on Jun 23, 2013 2:29 PM by Jared Conway

    FEA is taking a long time to solve (more than 8 hrs). Please suggest on how to speed up the process of solving

    Sandeep S

      Hi all,

       

      I have 3 plates of .016" thickness stacked one over another, fixed at the bottom (fig 1) and pressure(15 psi) is applied on the top face(fig 2), and no penetration contacts with COF of 0.1. Since it a very thin plate,i am using non linear analysis because the plate exhibit geometric non linearity and cannot be run in linear study. Also i have used solid mesh as i require the solid deformed model after the analysis in solidworks 2012 sp 5.

       

      Number of elements: 31,000

      Number of nodes:  64,000

      Degree of freedom: 180,000

      Solver used: Direct sparse.

       

      My system configuration and model in consideration are as shown below. Please suggest on how i can speed up solving time.

       

       

      1.JPG

       

      2.JPG

       

      4.JPG

       

      Thanks in advance

      Sandeep

        • Re: FEA is taking a long time to solve (more than 8 hrs). Please suggest on how to speed up the process of solving
          Jared Conway

          in hours does it solve or is still stuck at a certain percentage solved?

           

          also, your model was not attached. please use pack and go to create a zip of your assembly and the part files.

           

          for the size of your problem, i wouldn't expect it to take 8hrs. but if you have a missing BC or a bad input, that might cause issues.

            • Re: FEA is taking a long time to solve (more than 8 hrs). Please suggest on how to speed up the process of solving
              Sandeep S

              Hi Jared,

               

              As mentioned by Roland, i had initially run FEA for the assembly with 0.25" mesh (took abt 4 hrs to solve and Max deflection - .068" @ 15 psi center pressure) and also with 0.20" mesh (took abt 8 hrs to solve and Max deflection - .064" @ 15 psi center pressure) . I wanted to run the analysis with 0.1" mesh size to see if the results(displacement) are converging, With FFE plus solver, the run goes on and on without giving results and with direct sparse solver, it gets stuck in first step. Please have a look at the attached model used for FEA and suggest on how to reduce the solving time.

                • Re: FEA is taking a long time to solve (more than 8 hrs). Please suggest on how to speed up the process of solving
                  Jared Conway

                  thanks for the model. some comments:

                   

                  i see why you chose the symmetry that you did and why 2d won't work for you. my question, how important are the chamfers? can you give us a synopsis of the analysis you're trying to run and what you want to learn?

                   

                  from a setup perspective, it looks fine. going back to the chamfers, is there contact that might happen between the top plate and the chamfer? if so, the contact isn't accounted for.

                   

                  errors on 0.1" element size, it looks like you've played with the settings for the nonlinear solver. for example the singularity elimination factor is set to 0 instead of the default of 1. when you're running analyses, you should go with the defaults to start and adjust if suggested by the solver. (my guess is a previous analysis suggested this and you made the switch then)

                   

                  specifically on the 0.1" element size, did you look at the mesh? it skips your chamfer completely. you're going to need to come down to an element size much smaller than that to capture the chamfer. this goes back to the question above, what are you trying to learn, how important is it?

                   

                  if this was me and i needed to get this done for myself or for a customer, the first thing i'd do is see how far i can get and how much i can learn from having the components bonded together. this is going to solve quickly and will likely teach you a lot about what is going on. remember, in the analysis world, sometimes you have to settle for some trend studies. elimination of the chamfer is probably where i'd start as well. the other thing this study will tell me is what size element i need to get displacement convergence.

                   

                  from there, i'd ask myself how important is the deformed shape. if you have to keep the chamfer, you're stuck with a solid in the middle but the top and bottoms could be shells. the shape of this part is going to be pretty simple to model. maybe you can just model it maually based on what you learn about the displacements.

                   

                  another thing would be to understand the problem by breaking down the loading conditions. run one at a time. i think that will also solve quicker. reduced loads would be good again to understand trends.

                   

                  you might also want to check what happens with a linear solver. if it doesn't solve with linear, you're going to have little chance in nonlinear. (there are some that just won't in linear, but this is a good way to get started, sometimes just with a lower load to make sure your method works)

                   

                  if you can't do any of this, i think you just have to wait for the simulation to complete. you might be able to play with the different contact types, or play with the COF, play with solvers, play with settings, but in the long run it is what it is.

                   

                  something to note, depending on how many DOF you have when you run the problem at the high mesh level, if you're over 1 million and have less than 16gb of RAM, you will likely have a problem. the solver will go on and on and then fail and tell you to switch solvers. then if you switch, will do the same thing and tell you to go to the other solver. direct sparse is probably best for this case for the contact.

              • Re: FEA is taking a long time to solve (more than 8 hrs). Please suggest on how to speed up the process of solving
                Roland Schwarz

                Moving contacts take many iterations to converge. This will greatly increase the solve time.

                 

                Build and solve a smaller, coarser version of your model to be sure the setup works. Then increase size and number if elements.