25 Replies Latest reply on May 7, 2015 9:23 AM by Harmon Amakobe

    Non-Linear Beam Analysis - Plastic Deformation

    Harmon Amakobe

      I am attempting to create a simulation study that would match real world results for an aluminum profile that we have designed (96" long, 6063-T5; fixed on both sides and has a 200 lb concentrated load in the middle). We have the real world displacement data for the described loading situation, and I want to get close to it in a reasonable and reproducible manner.

       

      Aluminum Validation - Beam.JPG

       

       

      I have attempted modelling the profile as a beam, and running the simulation in the von-Mises plasticity material model, but that fails almost immediately, stating that the iterations are not converging.

       

      Beam Error.JPG

       

      I also modelled it as a solid, fixed both end faces and tried both a concentrated force (at a point) and a force at a face made by a split line, and received the same error (albeit with a  longer solve time). 

       

      Aluminum Validation - Profile.JPG

       

      I've attached screenshots to show how the profile looks, and the loading situation. I can't help feeling that I am missing something fundamental to how I am supposed to set this up. Please help!

       

      PS. The only successful runs I've had were through the solid model, utilizing the "Plasticity - Tresca" material model, though I haven't the slightest idea why and it makes me question the validity of those results (along with the fact that the resultant displacement implies that it is significantly stiffer than it's real world counterpart, which is not expected due to the way the test was conducted).

       

      PPS. I did try to increase the convergence tolerance, from the default 0.0001 all the way up to 10, but it always fails.

        • Re: Non-Linear Beam Analysis - Plastic Deformation
          Jared Conway

          I would recommend starting simple.

           

          Does it solve with linear.

           

          Does it solve with nonlinear solver but linear material.

           

          Then you can start diving into nonlinear materials. If it works without the nonlinear material, I'd look at the definition of your nonlinear material.

          • Re: Non-Linear Beam Analysis - Plastic Deformation
            Mark Ankrom

            You said it runs with linear material - does it exceed the yield stress ?

             

            Even if it shows yielding at some stress concentrations (end conditions or at applied load locations) it may not require a non-linear analysis to match the test data. This local yielding is small by comparison to the bending of a long beam.

             

            What test data are you trying to correlate (displacements, strains, etc.) ?

             

            I have found many of my problems with correlation are test setup (fixed ends aren't really fixed, load cell is misinterpreted, displacement transducers locations not same as in model, strain gages not reading correctly, etc.). This is an open section and will twist if not loaded thru the shear center.  Did the load application restrain the twist ?

             

            Do hand calcs of the test data correlate to the model and test data ?

             

            Mark

              • Re: Non-Linear Beam Analysis - Plastic Deformation
                Harmon Amakobe

                Mark,

                 

                I am attempting to correlate displacement data. I remember it yielding during my earlier runs, which along with a small permanent set during actual testing, led me to conclude that it might be going through some plastic deformation. However, I just now did a quick run and it's not yielding (which also makes sense since it's only 200 lbs). The deformation is calculated at around 1.1" whilst real world measurements set it at around 1.4". This is an aluminum reinforcement piece inside PVC railing, it is bolted to posts on both sides and is tested along with the full railing assembly (the 200 lb concentrated force placed at the top midspan). Common sense tells me that the additional resistance provided by the layers of material around it, along with the multiple balusters on the bottom should make it stiffer, not more flexible than my simplified testing model. I'm trying to reduce further complexity by testing only the engineered aluminum, and not the full assembly.

                 

                1.JPG

                  • Re: Non-Linear Beam Analysis - Plastic Deformation
                    James Riddell

                    Harmon Amakobe, based on the above picture, I would suggest that you do not have the correct restraints on the ends.  (I presume you are trying to model the fat, drunk guy at the party leaning on the railing.)  A more forgiving restraint would give you more deflection obviously.

                     

                    Also, have you tried your analysis with a standard C channel that has the same moment of inertia values as the shape you actually have?  That might give you more reproducible results.

                      • Re: Non-Linear Beam Analysis - Plastic Deformation
                        Harmon Amakobe

                        Haha James Riddell, yes, you presume correctly. In response to your previous comment, I do not expect the said fat, drunk guy to permanently deform aluminum railing. However, when I saw that my results had some localized yielding, I thought that they might affect the results in a way that stopped the railing to stop deforming prematurely; so I tried to move to an analysis that goes past yielding. I had figured that the fixture was a bit too unrealistic, but could not think of a better way to do it. Mikael Martinsson, had a great solution below (didn't think to restrain edges), and I think that it may be the way to go. I had also thought to do hand calcs, or a simplified model of it as a C-channel but it didn't occur to me to simply use the same moment of inertia values (I was having difficulty visualizing how to accurately simplify it), so that helps a lot and I thank you. Such a simplification will help further with the validation.

                         

                        I do have a follow up question regarding your comments about stress strain data, however, as I have other specimens to validate which do go past yield. I have not had as much trouble with those, but in the interest of being as accurate as possible, I'd like to ensure that I understand the type of data that needs to be input for non-linear plasticity. Could you elaborate further on what the appropriate interpretation is?

                          • Re: Non-Linear Beam Analysis - Plastic Deformation
                            James Riddell

                            If you go to 'Simulation Help', search for 'Input for Stress/Strain Curves' for the definition(s)/requirement(s) for input.

                             

                             

                            Analysis Options
                            Material ModelSmall Strain, Small DisplacementSmall Strain, Large DisplacementLarge Strain, Large Displacement
                            Non Linear ElasticTrue Stress, Engineering StrainTrue Stress, Engineering StrainN/A
                            Elasto - Plastic von Mises Plasticity, Tresca Plasticity, Drucker PragerTrue Stress, Engineering StrainTrue Stress, Engineering StrainTrue Stress, Logarithmic Strain
                            Hyper Elastic: Mooney-Rivlin, Ogden Blatz KoEngineering Stress, Stretch ratioEngineering Stress, Stretch ratioEngineering Stress, Stretch ratio
                            Super ElasticTrue Stress, Logarithmic StrainTrue Stress, Logarithmic StrainTrue Stress, Logarithmic Strain
                            ViscoelasticTrue Stress, Engineering StrainTrue Stress, Engineering StrainN/A
                    • Re: Non-Linear Beam Analysis - Plastic Deformation
                      Mikael Martinsson

                      I've looked at your file, and the first thing I notice is that the general stress in your linear simulations are well below yield with your setup. So Non-linear shouldn't give you the desired result since it follows the linear solution up to yield.

                       

                      I'm not sure that I understand your test setup, but using fixed fixture on two surfaces is very hard to replica in the real world. Like supergluing the surfaces against a infinitly stiff wall. If I try your setup but with only the 2 bottom edges fixed (like a hinge), I get the result below. If I look at X displacement the result is 1,43 inches. But observe, that the part, due to its shape, is allowed to twist since the load is not thru the shear centre. This is probably not the case with the real product since the "ladder steps" would minimize that behaviour.

                      Skärmklipp.PNG

                        • Re: Non-Linear Beam Analysis - Plastic Deformation
                          Harmon Amakobe

                          Mikael Martinsson,

                           

                          Thank you! That seems to be exactly the type of result I'm looking for. I will explore further, but I imagine that this solves most of the problems. As far as the twist goes, I've had trouble trying to locate the force at the shear center; I tried to locate the center of mass, and use it as a reference point to locate the force, but SolidWorks doesn't seem to allow you to use the center of mass reference point in that way. Do you have any tips on properly locating the force through the program? 

                            • Re: Non-Linear Beam Analysis - Plastic Deformation
                              Mikael Martinsson

                              Finding the shear center is not so easy. On my picture above it is on the left side of the part. On a simpler U-beam you could calculate it, but I don't know any way to find it in Solidworks. To locate a force on a point that isn't on the part you need to use a remote load/force. So if you want to add a load in the center of gravity, first you calculate it, to create a reference point. Then you add a coordinate system in that point and finally add a remot load/force.

                               

                              I would use a simpler approach in this case and do split lines for each "ladder" step and restrain these surfaces from movement in the normal direction. Not perfect, but good enough i think.