11 Replies Latest reply on Oct 23, 2012 8:29 PM by Jerry Steiger

    contact set trouble

    Jong Lee

      Hi, I am modeling polymeric window frame and doing structural simulation.  In predicting deflection under uniform pressure, global bonding option would not provide accurate result (too small deflection).  I changed to no penetration then gave me serval different error messages such as surface-based contact normal not found.  I checked out discussions on this issue but did not help me to solve my problem.  Shortly speaking, polymeric window frame has gaps between components everywhere and reinforced beams are used inside polymeric frame to reduce the total deflection of window frame.  I think global bonding option is inadequate approach to my situation as it assumes that all components touching each other would act as one.  What will be best practice to do simulation for the structure with gaps and movement inside space but no penetration?  This is very important for making decision on continuation of using Solidworks or changing FEA software companywide.  I really need your professional advice.

       

      J Lee

        • Re: contact set trouble
          Anthony Botting

          Hi J. I see no-one responded so I thought I'd take a stab at it.

          You are using a good approach with no-penetration contact elements, but it is intrinsically difficult in any FEA software because it's a nonlinear condition. At the start of the analysis, the software has to apply very small forces and then iterate to determine if any boundary contacts have closed. When it finds closed contacts, it has to stop and reformulate the stiffness matrices of all components because the boundary conditions have changed. Then, it increments the force a little bit more, searches for new or changed contacts, and so on. If some of the materials are soft compared to others (i.e., polymer frames, aluminum or steel interface material properties differ widely), then the software has options to turn-on a "large deflection" or "large strain" options to formulate the matrices yet again, and calculate deformations properly (takes more time to run) - so, this is really a difficult problem. I have used ANSYS and COSMOS/SolidWorks Simulation on similar problems - and the issues are identical.

          Anyway, a best practice is to start out simple and progress to more complex. Use nonlinear static study because you have a lot more control than the default linear static study. A very small section of the model is appropriate, and set-up the contacts while keeping all materials the same (such as using aluminum), and  use a very shallow loading rate (shallow ramp). The goal here is to get the contacts to work properly. Once they are working properly, then change the materials in appropriate components to the polymer, and try to run again. At this phase you may see "large deflections" or "large strains" manifested as long run times, as the software has to iterate and reform stiffness matrices at appropriate steps along the analysis. Having done this on a small, representative section of the structure, you will have gained much valuable information on the behavior of the structure under load, the typical run times, and typical computer resource requirements (i.e., memory needed) and you could use what was learned on a larger section, and hopefully up to a representative symmetric section that could simulate what you need to see.

          This "baby-step" approach seems the best way to go as each engineering analysis is unique. Hope that helps.

            • Re: contact set trouble
              Jong Lee

              Thanks Tony.  I agree with your theory and apparoach to my problem.  I am well knowledgable on how this window is tested and what boundary conditions are correct.  But in the linear static analnysis including large displacement theory, the FE solution was not even 1/10 of the experiemental data.  I played with various BCs, contact conditions, and anything that SolidWorks offers with linear static package for more than a month, but nothing makes close solution to what we expect. Like you proposed, I started with simple and easy model and got to more complicated ones, but when it came to a full model with every part in, the solution became way too small.  Also, I might have abused my workstation by runing anlalysis back to back and some times I had it ran two analyses simultaneously. Then, the FE program did not even update the input information or implement changes in BC or contact set but spitting same solution over and over again.

               

              This case of window is the worst one in terms of accuracy in prediction as compared with two other types of windows I developed.  However, this window is the most important one to solve due to its popularity and huge volume of sale.  My question is how much difference would nonlinear approach make in predicted deflection.  Ten times higher? or more?  Otherwise, it may not provide what we need to see.  I tried several plate theories to get close-form solutions but none of them got close to even 50 % error range to test data.  Polymeric window frames are lower in MOE than that of glass, thus there is a significant rolling on the side frame under pressure even with complete fix in the transitional degrees of freedom in all three axes.

              How does the gap element work between components?  It seems that my setting on a reinforced beam(rebar) within plastic frame does not move in the way I expect. It is supposed to move as soon as the plastic frame touches surface of the rebar due to the presence of room in between and takes control of deflection of the frame from then on.  So it should touch the bottom face of the frame under the load, but the resulting deformation does sho such action.  What do I need to look at to make this happen in my model?   

                • Re: contact set trouble
                  Jerry Steiger

                  Jong,

                   

                  I would not expect that your polymer material is being stressed enough to require a nonlinear material model. Usually I only run into those kinds of stresses in snap fits, or directly underneath a screw head, or in drop tests. If your stresses are high enough to get into significant nonlinear behavior, then I would expect you to see really bad creep or stress relaxation behavior.

                   

                  One possibility is that you are in fact seeing significant stress relaxation. If you are using a modulus based on a fast application of the stress, but your material is creeping very quickly under the applied loads, then the apparent modulus is going to be much smaller than the modulus used in your analysis.

                   

                  From your description, I don't think that the following is really your problem, but I'll throw it out anyway, just in case. Many years ago we had an analysis done on polymer snap domes for a calculator. The polymer layer was clamped between the printed circuit board and the plastic front case. Because we thought that our boundary conditions were in between fixed and floating, we had both analyses done. We expected the results to come out close to the fixed condition. The actual results came out much closer to floating, about 10% of the fixed calculations. We made a test fixture out of steel that truly clamped the edges of the dome. The results matched the fixed edge condition. Our plastic front case was barely restraining the edge of the dome. The moral of the story is that boundary conditions can make huge differences in the results.

                   

                  Jerry S.

                    • Re: contact set trouble
                      Jong Lee

                      It does have snap fits and direct screw connection.  Stress may be applied high enough to show nonlinear behavior because some windows show more than 6 in in deflection without glass breakage. I agree that boundary conditions can make great difference.

                      My  question is why one model (fixed window - not much flexible) works fine while the other one (sliding window-very flexible) does not.  

                        • Re: contact set trouble
                          Jerry Steiger

                          J,

                           

                          Are you saying that your global bonding solution matches fairly well with the experimental results for the fixed window but not for the sliding window?

                           

                          That doesn't seem to unreasonable to me, but it is just a gut reaction, not something I really understand. If the reinforcing pieces in the fixed window are very tightly constrained, with little movement possible, then bonding all of the pieces together might not be a very bad assumption. If the reinforcing pieces in the sliding window are more loosely constrained, or the outside restraining pieces that limit the movement of the window allow more movement, then global bonding would probably be a very bad assumption.

                           

                          I have to agree with Bill, that switching to another solver may not be an easy way out. I mostly use ANSYS for analysis and often run into problems when there is a lot of relative movement possible between the pieces. Of course, that could be my fault, as I am a designer, not an analyst, and struggle with the software.

                           

                          Jerry S.

                        • Re: contact set trouble
                          Jong Lee

                          Jerry,

                           

                          Vinyl frames of the windows deform (rolls out) a lot more than you can imagine.  In testing, the mid section of the window or door can deform up to 7 inches especially using composite polymeric beam as reinforcement without glass breakage due to rolling of the side frames. This is for the case of better thermal performance of the windows. I am not running my project for this particular case, but I still have pretty large deflection that no theoretical approach can predict.  I started nonlinear analysis but I faced a lot of errors including the nstar solver being crashed in the begining of the analysis or I can not complete meshing in either standard or curvature method.  Should I expect those troubles?  How do I check out the error messages in this analysis?  My test scheme is  positive 10 psf, neg 10 psf, pos 20 psf, neg 20 psf, pos 30 psf, neg 30 psf and each loading will be 10 sec ramp, 10 sec stay, 60 sec unloading.  Can this be arranged with your nonlinear package?

                           

                          I am using both global and local bonding setting but still I can not figure out the contact set to make sure the reinfored beam slides inside the vinyl frame without penetration and restrains window's bending.

                           

                          Jong

                            • Re: contact set trouble
                              Jerry Steiger

                              Jong,

                               

                              I am not familiar with how SolidWorks Simulation handles this type of analysis,as I normally use ANSYS. I expect that they are roughly similar.

                               

                              As I said, when the pieces being analyzed can move quite a bit relative to one another, it seems to be difficult to get the solver to  complete in ANSYS, so I am not surprised that you have trouble in SolidWorks Simulation.

                               

                              You might try setting up the problem with frictionless contact initially, as friction makes solving more difficult. Once you get it to run without friction, you can try adding just a little friction (ANSYS says that a coefficient of friction of 0.2 or less will have less problems than larger values), eventually working your way up to the expected friction.

                               

                              I often have to play with the stiffness of the contact to get it to solve, making the contact less stiff than  the default. I then try increasing the stiffness until it either stops solving or my penetration comes down to a reasonable level.

                               

                              I often have to work a lot with the mesh to get a working result that seems reasonable. Sometimes that means small elements, sometimes it actually means larger elements.

                               

                              You should be able to ramp the pressure up and then ramp it down. You won't see the actual effect of the time spent in the ramps and the dwell stage, just the deflection at the given pressures. I suppose you couild run a transient analysis that actually took into account the movement over time. I've never tried that.

                               

                              Jerry S.

                                • Re: contact set trouble
                                  Jong Lee

                                  Jerry,

                                   

                                  Thanks a lot for your efforts and kind advice which is very encouraging to my modeling effort.  I am curious why fixed window model can predict higher deflection than this slider model although the one is larger in size and span. It is just ten times higher in prediction.

                                  • Re: contact set trouble
                                    Jong Lee

                                    Jerry,

                                     

                                    I was checking my fixed window model I did earlier and I found I did uncheck draft mesh quality when I got a pretty good result.  I did same mesh option with other two slider and hung models and ran the simulations in linear static analyses.  It took a while (about 12-24 hrs mainly probably due to some unrestrained contact surfaces) until I got the results which  turned out pretty accurate as compared with experimental data.  I was really surprised at the difference in results between draft mesh quality and high waulity mesh.  I did it this way after I read nice comments from Jerry.  That was a really good advice.  I really appreciate that.  This made a great turn in my work and my boss starts to having a hope that we can rely on this software to save R & D cost for numerous testing works that can be significantly cut down by simulation.

                                    I will continue to share the progress of my work on this forum.  Thanks again.

                                     

                                    Jong

                                      • Re: contact set trouble
                                        Jerry Steiger

                                        Jong,

                                         

                                        Wow! At first I was also surprised that shifting from Draft Quality made such a big difference, but then I got to thinking that your parts  probably have fairly thin walls. Are you using solid elements or shell elements? If you are using solid elements, then you perhaps you were only getting one element through the wall section with draft quality and more with high quality?

                                         

                                        Whatever the explanation, I'm really glad that you are getting usable results.

                                         

                                        Jerry S.

                            • Re: contact set trouble
                              Bill McEachern

                              I would agree with Tony, blaming your lack of an experiemntal match on the code at this point is not a prudent way to go. Depending on how the thing is putogether your polymeric materials mybe more relevant than the contact aspect of the problem. Polymers tend to have non-linear stress strain relationships and typically they get softer as loaded. If you just used the material stiffness off the data sheet it may explain part of your descrepency. Contact is tough, non-linear contact tougher still. 

                               

                              If you get another code and you model it the same way you will likely get a very similar answer and I doubt you would look that good to your boss or whomever signed the check for the second code all that happy. Matching experiemntal data requires that you understand all the phenomena in the test article and that you understand with some fidelity how you translate all that into a simulation. Expecting a simualtion code to just pop out a right number when you don't have the right level of appreciation of what is actually going on is unrealistic.