4 Replies Latest reply on Dec 14, 2011 2:23 PM by Akash Vandakudri

    How to reduce penetration in solid works analysis

    Akash Vandakudri

      Hi,

       

      I am doing nonlinear FE analysis for press fit and coining process. I see whn I complete both the analysis, some parts do have penetration within the adjacent bodies.

       

      I tried changing the friction, but still every thing looks same. In Ansys, there was some thing call nomal stiffness and penetation tolerance and which would control the penetration.

       

      Let me know about it, if there is any setting in this solid works simulation (FE analysis), As I need to solve problem and if penetration exist then there is no point in increasing the load and also there will be chew in resultant force. As much of the force is decipated due to this.

       

      Is mesh an important criteria in this issue. As if you reduce mesh size will it reduce penetration and increases the contact pressure in that region..

       

      Regards

      Akash A vandakudri

        • Re: How to reduce penetration in solid works analysis
          Brian Zias

          Hi Akash,

          There are many factors that could be coming in to play here:

          1.  Make sure that the deformation scale in your result plot is 1.  This is under the plot Definition.

          2.  Mesh density is very important with this type of problem.  Make sure you're using High quality elements and you have sufficient elements to capture the curvature of your bodies.

          3.  Make sure and use "surface to surface" option in your local Contact Set.  This is the most accurate formulation, albeit slowest.

           

          If this doesn't help, can you post a screen capture of a section view or similar?

           

          There are also lots of solver settings in the Advanced Options that could come in to play depending how 'fast' this part is contacting.

           

          Brian

            • Re: How to reduce penetration in solid works analysis
              Akash Vandakudri

              Hi Brian,

               

              Thanks for your interest in this topic of dicussion.

               

              Regarding the listed points which you have mentioned, I have done the same way.

              1. Make sure that the deformation scale in your result plot is 1.  This is under the plot Definition. 

              The deformation scale is in true scale, as the problem is nonlinear,with large deformation and large strain, hence the plotting will be in true scale

              2.  Mesh density is very important with this type of problem.  Make sure you're using High quality elements and you have sufficient elements to capture the curvature of your bodies.

              The problem is highly nonlinear. It have frictional contacts, with metal plasticity, with large deformation and high plastic strains. I solved the problem with corse mesh and I get through the analysis with some penetration, but with fine mesh, the problem does not converge and exit with vauge warnings. This is been considered as solver issue with solidworks corp.

              3.  Make sure and use "surface to surface" option in your local Contact Set.  This is the most accurate formulation, albeit slowest

              I am using surface to surface to surface contacts only. Since this type of contact is best for this kind of problems.

               

              Since I have two analysis back on back to finish: First loadcase : shrik fit and then followed by coining process.

               

              Kindly let me know if there are any penetration contact algorthim in solidworks which can reduce penetration completely.

               

              Regards

              Akash A B

               

                • Re: How to reduce penetration in solid works analysis
                  Brian Zias

                  Akash,

                  I'd like to know more about your response to #2, since running high quality and fine mesh is going to be essential to getting a good contact force result.  What solver warnings are you getting?  You mention this is considered a solver issue - have you submitted this to your VAR and gone through their support and received that as your answer?

                   

                   

                  You are already using the proper algorithm if you are using the Surface/Surface contact set.  Here are some tips with the setup of those sets:

                  •   You shouldn't create many No Penetration contact sets with only one Source and one Target. Instead, you should create fewer No Penetration contact sets. In each of them, include all the faces that make physical sense to group together. This will be the case for instance for contiguous faces on the same part. Also, if a part A touches simultaneously parts B and C, then is probably makes sense to define a single contact set for it. 
                  • When defining local contact between faces that belong to components with considerably different moduli of elasticity, use the surface with the higher modulus of elasticity as the Target. In general the stiffer face should be the Target.

                  • In general, the Source entities can be faces, edges, and vertices except for the Node to Node and Surface to Surface option which allows faces only for the Source. Target can only be a face.

                  • Target face(s) should be flatter, larger than Source entities.
                  • Target face(s) can be meshed coarser than Source entities.

                  • There is no need to cut Target faces with split lines to make them smaller. Doing so doesn't increase analysis speed.

                  • There should be no 90° angle on Target faces if contact is expected in or around the corner area. If that is the case and you can't switch Source and Target entities, you should create a reasonably large round to cut the sharp angle. A very small round would create more problems. An alternative is to create two sets.

                  • Although possible, it is not generally recommended to define an entity as Source in a contact set and as a Target in another contact set. In complex models, it may lead to contact failure.

                   

                  In the end however it will still come down to using a good mesh to properly capture the contact forces, but give these suggestions a try and see if there is any difference.  Also, try using Direct solver.  I hope this does help.

                    • Re: How to reduce penetration in solid works analysis
                      Akash Vandakudri

                      Hi Brian,

                       

                      I am facing a problem in finer mesh with my problem. It gives me problem like listed below:

                       

                      1) Incremental strain is too high - when in advanced setting i have already given high value 10 to 100000

                       

                      2) Out of balance force - When I have already constrained properly and given 0 for singularities problem in advanced setting

                       

                      3) Check ON large displacement and strain

                       

                      4) Given all contact setting as I you have given in detail above.

                       

                      5) Time setting - Auto time stepping, min 1e-6, Max 0.001, initial Increment 0.001, End time 1.0

                       

                      6) Loading- Initial zero load for shrink fit and then curve based forced displacement on the tool.

                       

                      7) Material -Plasticity -vonMises - Yield stress and Tangent Modulus

                       

                      I am not only the one who is having problem in such nonlinear analysis but many others.

                       

                      Solidworks Corp have documented the problem as SPR 632740 and they need to resolve as soon as possible. They consider this as a bug in solver.

                       

                      SO for the same reason I am not able to use finer mesh. I had meshed with size of 0.05mm and it stopped as usual at 16% and didn't go ahead. But with slightly coarse mesh it solves completely.

                       

                      I am using Direct solver rather then iterative, as it is better in handling singularities and solves/converges faster.