9 Replies Latest reply on Mar 28, 2008 2:12 PM by Ian Hogg

    point loads

    Pete Yodis
      Can anyone verify that the method described in this link is a valid and accurate method for evaluating point loads on an object? Would you expect the deflection values presented by Cosmos to be in accordance with reality?

      http://www3.me.iastate.edu/me415_gassman/COSMOS03.pdf
        • point loads
          Ian Hogg
          Hi Peter,

          Point loads are not what I would call realistic. Mathematically, these are singularities and in analysis lead to artificial stress concentrations. Everything in the real world is applied over a contact area (ie not at a point). The size of the contact area obviously changes with material stiffness of the contacting parts. The size of the contact area also indicates the sixe of the mesh in that area to give an accurate stress distribution.

          There is no way you can trust the results in the area of the load as shown in the exercise. If you don't care about the area of the load application, I suppose you can use it to see the load/deflection of the overall model, but you will need to adjust your legend scales to filter out the results of the load point.

          Hope this helps answer your query.

          Cheers,

          Ian
            • point loads
              Pete Yodis
              Thanks Ian,

              Thats what I kind of expected to hear. I have a situation where I want to evaluate overall deflection of a model and also somewhat close to the area where this force is being applied to a small surface. I am seeing some higher than what I expected stresses directly under this load and I am thinking through how would I better model the situation. If I can't come up with a better model for evaluating this, then I am trying to determine at what distance away from the force can I beign to trust the deflection numbers.
                • point loads
                  Ian Hogg
                  Hi Peter,

                  How is the force being applied to the geometry in real life. You may want to conside modeling the geometry of the part applying the load (if there is one) and use contact to appropriately distribute the force over the surface.

                  As far as deflections go, are you seeing significant deformation around the point of applied load?

                  I suppose another question to ask is if the parts are plastic or metal. That will also determine how far out the results are in the area of load (linear vs nonlinear elastic properties) and how the stiffness of the structure will effect local deformation.

                  If this really is an area of interest, then more accurately modeling the load application method is the way to go.

                  Cheers,

                  Ian
                    • point loads
                      Pete Yodis
                      In real life this is a hardness check on the part. The force being applied is from the 15N scale Rockwell tester. The load is 15 Kgf or 147 Newtons. I have applied this load to a circular face on the model that I split. The diameter of the circular split face is .060 inches - which is the size of the head of the tester. The part being analyzed is made from steel 4340 BD material and the surface is harndened via ion nitriding to a supposed 88N minimum. I have applied mesh controls to the split surface for a mesh size of .005". I thought I read somewhere that local mesh controls only reduce mesh size on the surface and not throught the volume of the part. I was thinking I might need to refine the global mesh size to get through volume control of the mesh underneath the load. I realize the the load application in real life will deform the material in the part and the FEA solution will not capture that and give answer based on a linear elastic solution. I am more looking for a comparison of having one area of the part supported while under the hardness test vs. another area of the part supported while under the test. I am trying to get a feel for how much of a difference there might be between the 2 situations.
                        • point loads
                          Ian Hogg
                          Hi Peter,

                          As long as you are evaluating modeling this just to get a feel for the influences of the supports on the deformation, you should be able to get relative results within reason.

                          I'm a little rusty on my hardness test, but I thought in most cases you had a sample you placed in the device and it was predefined area of support around the impact tool.

                          In any case, surface mesh refinement does impact element size in the neighboring region, based on aspect ratio and number of layer settings. So if you pick a face and see an element size, it will transition over some distance to the global element size in the rest of the solid.

                          If you are sticking to linear, and just want to get an idea of the relative influence of the supports on deformation etc, then your approach of the split surface should work fine (you can guesstimate the surface stress just based on Force/Area too). You can do a couple of variations on split area size to look at sensitivity also.

                          Cheers,

                          Ian
                            • point loads
                              Vince Adams
                              Great conversation! Let me add this... We can talk about 100 different options and 90 of them may be the same and as good as you need them to be. However, the only way to know for sure in a scenario with interactions you've never modeled before is to try the least ambiguous method, contact. Granted, in some cases, this may be prohibitive due to resource requirements but these are fewer than you might imagine, especially with the speed of CW these days.

                              You can even explore interactions (Loads/Restraints/Contact) with a draft mesh to see if there are differences in the result of interest. If you feel that a contact interaction is sufficiently different than an applied load, such that you'd make a different decision based on the results, opt for the contact in the final model. After this, if the problem comes up again, you'll know where to start.

                              Having helped design engineers work thru load and restraint scenarios for many years, I can say with absolute confidence that trying the different options and comparing the results beats talking about them & then guessing hands down.

                              Good luck!!!

                              Vince
                                • point loads
                                  Pete Yodis
                                  Remodeled for contact conditions (no penetration). Modeled the diamond head as a round sphere. Material of the head - diamond (nice and stiff). I am running scenarios of the solution where I am changing local mesh controls, changing global mesh size, and then running h-adaptive (p-adaptive won't run with contact sets) - and of course changing the locations of fixed supports on the part itself. The conclusion I am coming to is that I need more computing power

                                  I'll post back later today.

                                  In the meantime.. My comment about local mesh controls affecting the surface of the mesh, but not the interior volume - comes from here on page 5...

                                  http://www.capinc.com/pages/su...s/KAPVolumeMeshing.doc
                                    • point loads
                                      Pete Yodis
                                      For some clarification on that information just posted - concerning an update with 2008... page 2...

                                      http://www.capinc.com/pages/su...APMeshArchitecture.pdf
                                      • point loads
                                        Ian Hogg
                                        Hi Peter,

                                        Yes, in this instance where the back surface is so close to the surface you are putting the mesh control, it does not have enough depth to transition nicely from the global element size to the local element size.

                                        The approach of doing multibody solids is useful in some instances. For the example sited in this article, I would have just put a split face on the back surface and given it a similar element size to the first face.

                                        It really is subjective to the particular geometry and what you're interested in when determining how to get a localize mesh that meets your goals.

                                        The reality is that while changing global element size is convenient (and works in most cases even with small features) it is computationally expensive. You are throwing alot of elements in areas that are of no interest. That's the challenge with the automatic transition option as well. The h-adaptive method is nice since it places elements where the stress gradients are high, but it is subject to being able to mesh the model. I haven't played with it enough on more complex geometry without local mesh controls to see how robust it is. Something to keep in mind.

                                        Cheers,

                                        Ian