6 Replies Latest reply on Apr 4, 2011 5:11 PM by Omid Khandan

    Fixed-pinned column buckling analysis help

    Omid Khandan

      Hi all,

       

      I am working on some column buckling analysis in SW simulations and needed help with the fixed-pinned geometry analysis.

       

      My problem is pinning the column on the top because I have a wedge tip (like a piece of pie). I have tried applying a roller to different parts of the column but my simluation result for the critical buckling load does not correspond very well with simple Euler's buckling analysis equations:

       

      P(critical)=(pi^2*E*Iz)/(K*L)^2

       

      where K = 0.699 for fixed-pinned geometry.

       

      Again, my results correspond well with the fixed-free simulations, but are not working out for the fixed-pinned geometry, I think due to the wedge shape of the tip and incorrect restrictions on the model.

       

      I have attached the model. The wedge tip is where the force is applied, and where the column is pinned. The bottom flat end is the fixed end.

       

      Thanks for your help in advance.

       

      Omid

        • Re: Fixed-pinned column buckling analysis help
          Anthony Botting

          Hi Omid:
          I got a difference from your formula of less than 3%. I used the BEAM functionality because it's fairly easy to apply the boundary conditions. You may have already tried this but, right click on the solid body in the simulation tree and choose "treat as beam". Next I assigned a pinned end to the wedge tip. I attached a screen shot of the joint settings in the fixture property manager. Essentially I just restricted translations in-plane (relative to the selected plane), but allowed a vertical translation of the joint (there is a purple-colored, downward unit load arrow there, too). I also allowed rotations about the joint with the exception of axial rotation. This solves in just a few seconds (presumably because it's using BEAM elements which solve super-fast). I hope this helps a little. - Tony

            • Re: Fixed-pinned column buckling analysis help
              Omid Khandan

              Thanks a lot Tony. I actually didn't know about the BEAM feature in SW. This helps a lot. Although I am having trouble applying the load on the edge of the wedge tip. Can you please show a print screen of the applied restrictions to the force?

               

              Thanks,

               

              Omid

                • Re: Fixed-pinned column buckling analysis help
                  Anthony Botting

                  Yes here is one. I just put a unit load on it, normal to the front reference plane. The "Joint" as they call it, is the olive-colored sphere (it is where the fixtures and loads terminate). The color olive is used to show that the joint is not attached to any other joint (SW  uses a fuscia color to show when a joint is attached to another joint). These "Joints" actually have six degrees of freedom: three rotations and three translations. It turns-out, the joint is actually an end node of the beam element. The beam element for this case is an idealization, because it extracts the cross-section of the column (as a constant cross section) and does not take into account the wedge-shaped end that is on your model (hence the joint terminates a little early inside the end of the column where the constant cross section ceases to exist). So, perhaps another try using solid elements would represent the geometry better. With solid (tetrahedron) elements, we could get the actual cross section near the wedge-end modeled more accurately, but I don't believe the results will be closer to the analytic calculation- I'm assuming the analytic calcuation assumes constant cross section, too. It's worth a try, though.

                  • Re: Fixed-pinned column buckling analysis help
                    Anthony Botting

                    Hi Omid:
                    One thing I left out - you have to set the eigenvalue extractor to go to six modes for the BEAM model (which presumably correctly approximates the closed form solution). The result varied by only 1.7%. I tried this on a solid model, too, and it found the correct bending (buckling) direction by solving only to the second eigenvalue. However, this default solid mesh produced a solution that was about 10% difference from the closed form solution (assumed constant cross section). I conclude the solid mesh is likely to be more accurate (subject to a convergence check) because it models the geometry more accurately than the BEAM model. I sure hope this helps. -Tony