4 Replies Latest reply on Mar 17, 2009 12:35 PM by 1-9DZR23

    Understanding Local Peak Values

      I've attached a typical result from a face contact test. The loading face (not shown) is larger in diameter than the die face (shown). Loads are extremely high as is common in this application. I'm having trouble deciding if the high local peaks (400ksi+) often found radomly at vertex nodes can be ignored in favor of the results shown in the color chart. These appearent singularities are a common occurance especially on complex geometry.
        • Understanding Local Peak Values
          Mike Lowinske
          In my experience with FEA, using triangular meshes like COSMOS does results in erroneous results around sharp edges as opposed to using quadrilateral meshes like better FEA programs can do. Like you said, the tri meshes produce a singularities on sharp edge. I usually ignore them.
            • Understanding Local Peak Values
              Thanks All, Seems like there's agreement that under certain conditions, peaks can be largely ignored but a radius properly meshed will yield more consistent results. My results are based on h-adaptive mesh convergence. As I recall, the polynomial adaptive convergence was very similar. I agree that a sharp corner increases the modeling error but I have seen similar results on small radii at the tangent of the radius. Often model errors are generated by small radii as a result of oblique tetrahedrons combined with peaks at the tangent. I will experiment with a radius and increase mesh density as needed and see if results are more consistent.

              Regards,
              Dave Trent
            • Understanding Local Peak Values
              Dave,
              if your objective is to determine the maximum stress, then the decision to analyze a model with sharp corners is a very serious mistake. According to the theory of elasticity, stress in the sharp corners is infinite. The finite element model does not produce infinite stress results due to discretization errors, and these errors mask the modeling error. However in the vicinity of sharp corners, stress results completely depend on mesh size. These results are totally meaningless at these locations.
              If your design intent is to determine the maximum stress you must include a fillet, no matter how small it is.
              If you want to check if your FEA model is correct check the convergence of the displacements results. Usually they converge while the stress behave differently.
              Hope it is clear and helpfull
                • Understanding Local Peak Values
                  If the high nodal stress is distributed on more than four or five elements, i will consider for failure criteria. If it is concentrated on one or two element, i will ignore it.

                  We normally dont use model with sharp corners. As Gianluca commented, we normally use fillets on sharp corners.

                  I suggest you to probe the stress results on all the nodes [Two to three layers]close to the high stressed node. If the difference is huge say above 20% then ignore the high stressed node. If the difference is less, you should include for failure criteria.

                  Correct me if i'm wrong.