8 Replies Latest reply on Aug 5, 2010 2:06 PM by Ryan Werner

    FEA on weldments -- changing structural members

    Jim Andrews

      I've been using COSMOS/M since the early 1990s, but recently joined the 21st century and started using SolidWorks + Simulation.  I am not very proficient at either.  I would appreciate it if someone could walk me through a roadblock I've encountered.

       

      I am analyzing a welded structure with beam elements.  Ultimately, I want to optimize the structure for cost, but for now, just assume that there is one particular structural member which I would like to change based on the FEA results.  For instance, let's say I have a 4 x 4 x 0.25 square tube that is a bit highly stressed, so I'd like to change it to 4 x 4 x 0.375 and rerun the analysis.

       

      Is there an easy way to make this change without having to redefine all my loads and boundary conditions?  Thanks in advance for any help . . .

       

      ja

        • Re: FEA on weldments -- changing structural members
          Anthony Botting

          Hi Jim:

          Yes. Use Weldments. You get this functionality for free PLUS section libraries. Just draw a stick figure (2D or 3D Sketch) of neutral axes like you did in COSMOS/M. Use the Weldment toolbar to create the beam. It will prompt you to pick from a library of cross sections, then click the neutral axis lines and voila - it builds you a beautiful, mitered weldment frame automatically trimming corners, too. Very nice. Weldments are specifically designed for parameter change (i.e., swap the section for another one), and BEAM elements were specifically designed to use Weldments (although you can now use other solid bodies). This is wonderful software. COSMOS/M user since 1990. - Tony

            • Re: FEA on weldments -- changing structural members
              Jim Andrews

              Thanks Tony.  Here's the deal:  I AM using a weldment.  I just don't understand how to effect the change in a structural member.  It seems like once I make the change in my Feature Tree, the model won't run again.  Am I doing something wrong?  (Obviously!)

                • Re: FEA on weldments -- changing structural members
                  Jim Andrews

                  Just to be a little more specific:  at the very least, it seems that a simple change in a structural member results in (a) lost material properties, (b) loss of the mesh, and (c) redefinition of joint numbering.  The latter typically causes boundary conditions to get scrambled.

                  • Re: FEA on weldments -- changing structural members
                    Anthony Botting

                    Thank you for letting me know. I just tried it in SP3 of SW 2010. It's not quite 'parameteric'. First duplicate the existing study. Next, change a cross section. You have to fix the duplicated study material properties for each beam by dragging and dropping the materials from the other study (you can do that in one shot with shift-select and drag). Next, edit joint group and click 'calculate'. Contact definitions may need to be re-edited. Then make sure to re-mesh, before running.

                     

                    Note: I believe there are MANY enhancement requests asking for the rather non-parametric nature of BEAM studies to get fixed.

                      • Re: FEA on weldments -- changing structural members
                        Jim Andrews

                        A-ha!  So I'm NOT losing my mind!  Thanks.

                         

                        I'm having some problems with a c-channel . . . any tips on getting joints to play nicely with each other?  I get the feeling it has something to do with the neutral axis not lying within the material of the structural member.  Is this a notorious problem with channel structures?

                          • Re: FEA on weldments -- changing structural members

                            Hi Jim,

                             

                            I feel your pain.  Simulation renumbers the joints every time you change the members, so you have to "edit joints" and  recalculate after any member changes.  Any loads or restraints attached to joints then have to be reattached.  Sometimes you just have to "edit definition" and check that they are still listed.  Other times you have to reselect the joints.  It is especially annoying since the software still "knows" where they are as the graphical symbols for loads or restraints are often still in the right place even when the joint numbers don't show up under "edit definition."  One of my VAR's support people listed this as a "feature" when I reported it as a "bug!"  Him: "Simulation helps you to reattach the load/restraint to the joint by showing you where Simulation thinks it is."  Me: "If Simulation knows where it is, why can't Simulation re-attach it?  I can always change it if I decide Simulation has made a mistake!"  The best way to work around this problem is to apply loads and restraints to members rather than joints whenever possible.  Sometimes I use "dummy" members for this purpose.

                             

                            Regarding getting channels to intersect, I have found that beam structures work best if you draw your structural member sketch lines so that they intersect.  Note that when modeling structural members in weldments, you can pick the point on the cross section which is pierced by your sketch line.  I try to pick a point close to the neutral axis, but it is not absolutely necessary.  You can also increase the "joint clearance" to get Simulation to find joints when your sketch lines or the neutral axes don't intersect.

                             

                            Regards,

                             

                            Dave.