4 Replies Latest reply on Mar 20, 2011 12:22 PM by Jerry Steiger

    Need help to properly apply boundary condition

    Devi Prasad Samal
    Devi Prasad Samal Jan 27, 2011 1:58 AM

      Hi Experts,

       

      I have a simple question to ask...

       

      I am trying to silmulate a analysis of Base frame of a flat bed trailer. I have uploaded the pic.

       

      As in the picture i have fix the king pin location from front & axle location from behind. u can see the green arrows to see the fix location.

       

      and then add a load at appropriate position.

       

      But after running the simulation, what i find that stress is developed near axle position where i have fixed the assembly.

       

      But in real life normally base frame has more damage at goose neck position.

       

      What i am doing wrong? do iahve to take the suspension type boundary conditon or what.

       

      please advice...

      • 1029 Views
      • Categories: Simulation
      • Tags:
        • Re: Need help to properly apply boundary condition
          Anthony Botting
          Anthony Botting Feb 4, 2011 10:35 AM (in response to Devi Prasad Samal)

          HI Devi:
          I would be tempted to try an elastic foundation support at the suspension locations. Alternatively, build-in some parts to represent suspension support springs (with appropriate stiffness) and use no-penetration contact between the supports and the frame. Then ground the supports. Either method can help the frame to flex a bit more at the suspension supports, perhaps more like real life. The issue is that "fixed" boundary conditions are infinitely rigid and can cause a lot of stress. Be aware that no-penetration contact makes the problem nonlinear (the solver has to iterate and stiffness calculations have to be re-done at appropriate intervals), so it takes longer to run. The elastic foundation support method is more straightforward and should solve very quickly. Hope that helps. -Tony

            • Re: Need help to properly apply boundary condition
              Devi Prasad Samal
              Devi Prasad Samal Feb 21, 2011 1:24 AM (in response to Anthony Botting)

              Thanks for the reply, and sorry for my side for the late update...

               

              yeah i am sure what u write is the good way to have a real time simulation.

               

              But actually i am asking that is it possible that stress will developed at goose neck position?

               

              because in real life normally frame are collapsed at that location.

               

              regards

              devi

                • Re: Need help to properly apply boundary condition
                  Anthony Botting
                  Anthony Botting Feb 22, 2011 5:35 PM (in response to Devi Prasad Samal)

                  Hi Devi:
                  You mentioned that it collapses. In that case you'd need to run a buckling analysis. The structure can collapse with low stresses in that area (relative to the rest of the structure) if the slenderness ratio is high enough compared to the load. This "Buckling" module is very non-conservative because it uses Euler/Bernoulli linear buckling theory, but it can be used to investigate possible failure modes other than material stress failure. Hope that  helps.

                  • Re: Need help to properly apply boundary condition
                    Jerry Steiger
                    Jerry Steiger Mar 20, 2011 12:22 PM (in response to Devi Prasad Samal)

                    Devi,

                     

                    Perhaps I am blind, but I don't see any fixed position at the front end of the frame.

                     

                    Fixed points or faces are very easy for the Simulation software to solve with, but they are usually a very bad approximation to real life. The springs in your suspension allow the frame to rotate freely, unlike the fixed faces. That completely changes the deflections and stresses in the frame. If I were working on this in ANSYS, I would use spring elements and fix the other ends of the springs. That would be a much better approximation to the real  situation.

                     

                    You mention collapse. If you are trying to simulate what happens under extreme loads that could actually cause your frame to fail, then you will need to run a nonlinear analysis, with large deflections and nonlinear material properties (probably simple elastic-plastic would do).

                     

                    Jerry Steiger