15 Replies Latest reply on Feb 19, 2015 5:20 PM by Jared Conway

    simulation of bodies penetration

    Ben D.



      is there a way in Solidworks Simulation to perform a material penetration test? The simplest example would be a hardness test: a sharpened steel balk is being pushed into the aluminum plate. Is there a way to see this deformed aluminum plate, and other parameters? If so, what would be the settings for this kind of study?


      This is what I would like to do:




      Thank you for your advice

        • Re: simulation of bodies penetration
          Andrei Popov

          I think it is possible such a simulation in Nonlinear package, you have to define a contact condition between the two bodies. I would draw a circle where the contact will be on the target body firstly.

          This circle would be used when you define a Mesh Control select the area where you want the mesh control has to be applied, so that you can modify the mesh settings in the area of contact without changing too much the overall mesh, which can be quite coarse at the edges of the plate, but need to be refined in the contact area.

          Then when you define the contact condition to Non-penetration you have two options surface-to-surface and point-to-surface which you can find in the Advanced Options. Non-penetration means that the mesh nodes of the steel balk does not penetrate into the target mesh.

          My contact simulations worked best with point-to-surface but I never did a penetration simulation.  2015 SOLIDWORKS Help - Node to Surface Contact

          You may try both types of contacts, you can change that option in the solver options.

          Before running remember to supress or delete the bonding contact condition which is by default in the contacts definition branch, this in case you want to have initially a gap between the steel balk and the aluminium plate and as the simulation progresses the gap decreases until they come into contact.

          Also when select the materials I would select the creeping since the aluminium will creep under the steel pressure.

          Here is atutorial about setting contacts on youtube: SolidWorks Simulation - Nonlinear Rubber and Contact (1 of 3) - YouTube

          here are explained the settings for the solver: SolidWorks Simulation - Nonlinear Rubber and Contact (2 of 3) - YouTube

          I would use direct sparse solver with simplified option for incompatible bonding contact.

          If you select 'more accurate' the solver will switch automatically to surface-to-surface condition.

            • Re: simulation of bodies penetration
              Andrei Popov

              I remembered my issues with contact problems, I am not so sure you will succeed but it worth a try. The reason why I say that is because your problem is a compression loading and locally can lead to numerical instabilities (basically the solver will see two or more nodes as "buckling" and it will stop the simulation when the buckling condition is reached). You may try different control schemes, but I had great difficulty finding one that works In compressive loads. If I remember correctly the arc-length control is not compatible with contact condition problems, only force control is allowed. But maybe it will work if you have a hard material that penetrates into a soft material which is in your case.


              2015 SOLIDWORKS Help - Incremental Control Techniques

                • Re: simulation of bodies penetration
                  Ben D.

                  Hello Andrei, thank you so much for the input. I am trying to work on your suggestions. I am trying different versions of connectors, meshes and other configurations, but this simulation takes so much hours ... I leave my computer over the night performing calculations, and find an error every morning. I will try to work more on this simulation, and come back a little later with the resume of the results. Thanks again for now for your advises!

                    • Re: simulation of bodies penetration
                      Andrei Popov

                      Hi Ben D,


                      The reason it takes so long to solve is that you use a very refined mesh where you don't need it, as I see in the pictures you posted. I would do a very coarse mesh anywhere else except near the point of contact. This is the reason why I told you to add a new surface by drawing a circle on the face you want to puncture so that you create a mesh control in this area. The idea is to have a mesh like in the in the arrazola.pdf posted by Shaodun Lin, very refined in the contact area but very coarse everywhere else, so that you save a lot of solving time.

                      another option would be to do the same as in that pdf, an axisymmetric 2D model which will reduce the number of equations a lot.

                      you can set plastic deformations when you select the material and you define the stress-strain curve. Also you can select strain control in the solver options to see the plastic deformations, but basically you must change the compression problem in a tension/shear problem like in the pdf I mentioned earlier. But you cannot see the fracture as in that pdf, because solidworks won't change the geometry of the mesh.

                • Re: simulation of bodies penetration
                  Jared Conway

                  can you see the deformed plate? yes


                  can you see it get ripped? no

                  • Re: simulation of bodies penetration
                    Shaodun Lin

                    Hi Ben D:


                    To reduce processing time maybe you should consider perform the simulation with 2D profile?


                    The problem you tried to simulate is highly non-linear, very large strain deformation, I am not sure how well SolidWorks simulation can handle this kind of problem.

                    To make the thing easy, reduce number of mesh by using a 2D profile first.

                    • Re: simulation of bodies penetration
                      Shaodun Lin

                      Hi Ben D:


                      I attached my file here for your reference, it is in SW2015 version.

                        • Re: simulation of bodies penetration
                          Bill McEachern

                          If the tip is a point you will have a very tough time trying to get the contact established. Blunt the tip with a small flat - something you can resolve with a mesh not some super tiny thing.

                          • Re: simulation of bodies penetration
                            Ben D.

                            So I followed the advice from Shaodun Lin, with 400N load this is what I got:



                            Seeing that no important information of stress is available through the height of these relatively high models, I made them a little lower:



                            Then I tried to achieve as much deformed lower plate as I could get. I made sequence of tests by incrementing the load by 100 N in each step. At 800N was the last load that it ran (at 900 N the simulation started to fail). These are the results with the load of 800N


                            The zoomed image at the intersection area:



                            So, I was interested if it is possible to make a destruction simulation. I made a really thin lower plate, and changed the fixtures from the bottom edge to the side edges of the lower plate. The simulation failed even with much smaller loads, these are the last results it could calculate:




                            Just for the interest, I changed the sketch to the punch type shape, and ran the simulation. It failed at a certain point (I think the material should start separating at this same point), this is the last view the simulation generated:



                            So, it looks like non linear simulation is able to run as long as the ultimate tensile strength and the model properties reach the limit of deformation, and should start cracking. After passing the limit of material damage, the simulation fails. Is this correct? Is there any other way to simulate, lets say, a punch through a sheet of metal, where some material is cut-away from the base plate?


                            I just thought that seeing the quality of the material cut in such simulation would help the punch designers to develop quality tools, and I am wondering if this is possible with SW Simulation? If not, is it possible at all, using other specialized simulation products, like Ansys or other?

                              • Re: simulation of bodies penetration
                                Shaodun Lin

                                Hi Ben D:


                                Just like Jared Conway mentioned in his reply, you can simulate the material deformation, but you are not able to see material being ripped apart after stress level pass UTS.


                                ANSYS is able to define the behavior of mesh after UTS,


                                Alternatively, you can use Abaqus, it has many success story of using this to understand the cutting edge / punching die design.




                                You may also consider Advantedge or Ls-Dyna

                                  • Re: simulation of bodies penetration
                                    Ben D.

                                    Shaodun Lin, thank you for your information links. It is exciting to read about other products and their possibilities. Maybe one day I will get a chance to try them in practice


                                    I do have one more question about the material deformation. May I ask if you, or somebody else here in the forum, have some more information about material models types? You can pick it in SW material selection interface in non-linear analysis, choose between Linear Elastic Isotropic, Plasticity vonMises, Tresca, and others. I didn't study these subjects in my university, and solidworks help is pretty frugal in the manner of explaining them. Despite of mathematical formulations and short description, there are no comments about the differences between them, applying and using them in practice. Maybe some information could be sheared about the composition of these model types, usage, application, and differences between them?


                                    Thank you in advance