5 Replies Latest reply on Aug 9, 2007 3:45 PM by Troy Higgins


    Kinjan Patel
      After running a normal stress analysis, I noticed that the localstress was very high over 250,000 psi for a 36,000 psi material. In real life situaion the material would yeild and distributethe stress.  In cosmos that is not the case, so I triedrefining my mesh in that region, but that didn't seem to help.

      My question is how is one to know when the local stress is high andshould be ignored when interpreting the results?

      Also can anyone recomend a good basic FEA book or site that talksabout this types of issues.

      Thank you
        • LOCAL STRESS
          genexxer genexxer
          Is the force applied on multiple faces/edges?

          The stress would vary with geometry and boundary conditions as the mesh is loaded. One thread here talks about applying force loads to multiple faces/edges. Check the reaction loads to ensure they are close to the applied loads.

          If reactions and loads tie, try this: produce a plot on screen of the deformation at scale of 1:1. If the deformation is visible to the naked eye, then use the nonlinear static solver in a new study. I guess the deformation is visible since it is so far past yielding. This will better approximate the stress as the geometry changes under static load. This is a time intensive solver so it may be useful to back off on those mesh refinements for the first time.
          • LOCAL STRESS
            Peter Gillespie
            I, too, would be interested in learning more about this topic. I come across it fairly often, usually in compression, and am not sure how to interpret it. A stress that is well beyond yield (10x yield). Deformation in that area shows to be negligible, so it doesn't seem to be a non-linear issue, although it could be.
              • LOCAL STRESS
                Vince Adams
                First thing to remember is that with a linear material model, stresses approaching yield can not be taken at face value. That statement must be left general in the absence of a stress-strain curve. Even if you can't solve for a nonlinear material model (based on the CW product you own - Advanced Pro is req'd for this) you should always try to get your hands on as representative a SS curve as you can. Most steels are very linear until yield whereas many other materials deviate from linear at a much lower stress... not just plastics! Once the linear range of the SS curve has been passed, locally, the stresses will calculate unreaslistically too high. This is the nature of linear static FEA.

                The other thing to think about is unnatural stress risers in your geometry or as caused by your loads & restraints. Two extreme cases, a point load and a sharp inside corner, will report increasingly higher stresses as the mesh is refined locally. This is because the true stress estimate on, say, a point load is F/A. When A goes to zero, stress goes to infinity. These are called stress singularities. Another common culprit for stress singularities is the region adjacent to a fixed restraint. In this case, the stiffness changes from infinitely stiff to something more realistic. This unreasonable change in stiffness, thus a nearly infinite change in local strain, will also converge to an infinite stress.

                That said, which of these, if any, was the cause of your problem? It can often be more than one effect. You'll have to review your model or post some screen shots if you want some additional discussion.

                How important are these stresses? I strongly advise against simply ignoring hot spots caused by singularities. As I often say in training, "red spots are red flags!" These are telling you that something in your model doesn't match reality. You need to understand why before dismissing the problem. If you can convince yourself that these unrealistic stress risers don't have any real impact on the data of interest, note that in your report and move on. If you can't state confidently that they have no bearing on the decisions you need to make from the data, take some time to add more "reality" to the problem. Add a fillet to a sharp corner - I've had detailed scans of parts with corners that appeared sharp to get the true fillet in that area. Replace a restraint with an equivalent load, or even better, contact with the restraining part. If you believe the linear material assumption is invalid and you need to know how nonlinear you went, you'll need to try a nonlinear material solution.

                Hope this helps! I regularly get questions about hot spots and stress singularities so maybe this will clear up some of the confusion.

                  • LOCAL STRESS
                    Pete Yodis

                    Thanks for the information. It is always very helpful. Is there anything related to this in the Cosmos Companion series webcasts? If not, could I request some content that deals with these issues? Sounds like local mesh refinement and some convergence studies would be on the list of things to do to help analyze this situation (I think your suggestion of placing a fillet if one is not already present falls somewhat under local mesh refinement). Are there any other methods you would suggest? Studies where you half the loads on the model and look at the results, make several changes to the surrounding geometry and re-run and look at the results, etc... - anything that might help shed some light on how the model is being solved to arrive at its answer. Thanks for being involved here.

                    Pete Yodis