9 Replies Latest reply on Aug 15, 2011 3:19 PM by Michael Feeney

    Buckling of a cylindrical rod

    Marleen Offringa

      I really hope someone can help me with a problem I'm having with Solidworks simulation.
      I'm a student Industrial Design and I'm designing a toy for children. The toy consists of rubber stiks that children can connect to build structures. I'm facing some problems with simulating the behavior of a stick. A stick is 600 mm long, has a diamter of 30 mm and is made of rubber. I want to know wat will happen when de stick bends in a certain situation: when someone is holding the stick at the ends and moves the hands toward each other. How far is it possible to bend it and will there be buckling or just bending? I've tried to do this by fixing one end and putting a force on the other ,but it never bends far enough. I think I need a moving force or something but I really don't know. Can someone help me? Is this possible with Solidworks simulation? If yes, how? If no, is there an other way to do it?

       

      Edit: Here is the image on another server: JPG & PNG.

        • Re: Buckling of a cylindrical rod
          Michael Feeney

          Can anyone else open up that image?

          • Re: Buckling of a cylindrical rod
            Anthony Botting

            I cannot open it, either.

            Marleen can you send a "*.png" format or *.bmp? Maybe there's something wrong with the web server.

            You should be able to do the analysis in simulation, but the behavior is highly dependent on the boundary conditions. Is the stik hollow inside? The reason I ask, are you seeking localized buckling where the wall could collapse? If the stik is solid and you run buckling on the unit, it would likely just bend (this is a valid buckling mode) - the software will give you the shape and the load factor. Just multiply the load factor times your load value, and that's the load that would cause the stik to "buckle" (for a solid it would likely just bend). Typically I like to use a force value of one (1) so you can observe the load factor, and you're done. Try it with one end fixed, then try it with one end pinned (as on a swivel), and you can obtain upper and lower bounds of the problem. Beware, however, the Buckling Module is non-conservative, giving the 'best-case' answer for exact boundary conditions (load down the exact center of the stick, absolutely rigid end conditions, or absolutely pivoted end conditions). That is, if the student holds the stik off-center just a bit, the answer will be wrong. Or if he/she holds it horizontally instead of vertically, I assume there would be a weight deflection that will affect the answer.

            Also, if the unit is hollow, it could "buckle" in overall bending before the wall collapses, depending on the thickness of the wall. In that case you could tell the solver to find 2, or 3 buckling modes - the second one may be the wall collapse if it's stiffer than the bent shape of the stik.

            You can use the Non-linear module to investigate end-condition offsets and see how it affects the answer, too.

            Hope that helps a little.

            Tony

              • Re: Buckling of a cylindrical rod
                Marleen Offringa

                Thanks for your answer!

                I'm wondering how I can actually make this simulation work. What are the steps I have to make to achieve the stick to bend the way I want. I'm only able to make it bend a little, but not to bring the ends together. The stick is solid, I'm trying to find the perfect thickness for it.

                Can you open the image already?

                stick_bending.png

                  • Re: Buckling of a cylindrical rod
                    Anthony Botting

                    Hi. Yes, i can open the image now.

                    You will need to resort to the Nonlinear Module. It will automatically update the structure stiffness as the rod bends around. Make sure to access the Properties of the study and check the option "Update load direction with deflection....", so your applied force will follow the tip. You will need to assume the localized strain is "small" meaning strain will follow the "engineering strain" definition (the software has "large strain" option only for plasticity models).

                    The structure is likely to get very stiff as it bends around, so you may have to run several cases with different applied force to get the rod to bend all the way around.  There is a built-in tutorial showing how to do this. Go to menu "Help/SolidWorks Simulation/Tutorials", then find the "Nonlinear" section, and the tutorial is called "Rolling a sheet into a ring".  I hope this helps... Tony

                      • Re: Buckling of a cylindrical rod
                        Marleen Offringa

                        Hey. Thanks a lot. The tutorial was very useful. Still I'm facing some trouble with getting the rod to bend the way I want. In the tutorial the sheet rolls perfectly into a ring, how exactly does that happen? In what step do they make sure that the sheet does not just bends over, but rolls exactly in the right direction?

                        Now my rod is bending like this and I want it to bend like I drew it(or like the sheet in the tutorial)... Marleen.

                        rod.png

                          • Re: Buckling of a cylindrical rod
                            Anthony Botting

                            Hi Marleen:

                            is the "Update load direction with deflection...." turned-on the the Properties of the study? It is supposed to allow the applied force to follow the tip as it bends around. I believe it only works if the force is applied normal to a flat face (you may have to create a cut in the model perpendicular to the rod axis to make a flat face). This should cause it to curl around but I believe (from your drawing), you want it to stop at 180 degrees, then bring the ends together.

                            In the tutorial -from theoretical calcs, they figured-out the turning moment that would cause the ring to rotate 2(pi) radians, however the turning moment can only be applied (out-of-the-box) onto the edge of a shell mesh. Since you have a solid mesh, you could try the "Torque" command (you'll need a reference axis) on an end face of the rod to get it to curl to 180 degrees, then turn on a force to cause the ends to come together. So you would have two loads: 1) ramp-up a Torque from 0 to  0.5 seconds and hold the value constant through end of analysis (usually one second). 2) Another load (force) is zero from 0 to 0.5 seconds, turns-on at 0.5 seconds and ramps up to full value at 1.0 seconds to push the ends together.

                            You probably don't know the torque value to cause it to rotate by 180 degrees, so will need to try several values. Once you get that, try copying that study to a new one, and add a second load to cause the ends to come together.

                            Let us know if that helps a little.

                            Tony

                              • Re: Buckling of a cylindrical rod
                                Marleen Offringa

                                Thanks! It is approaching what I want to achieve. I hope I will succeed today, I'll let you know.

                                  • Re: Buckling of a cylindrical rod
                                    Marleen Offringa

                                    Hi. It is working. Now I'm comparing some different materials, but the running of some simulations take very long and sometimes they fail. What can I do to make them run better?

                                      • Re: Buckling of a cylindrical rod
                                        Michael Feeney

                                        Hi Marleen,

                                         

                                        I hope all is well with your project. In my experience there isn't much that one can do to speed up nonlinear analyses. Assuming your mesh is converged, perhaps reducing the number of elements (checking to make sure that the results don't deviate from the converged solution) or using simpler elements could be an option. On the other hand, for large displacements and rubber-like materials...the computation time is usually long. You can reduce the iteration time as well (which means you would only simulate the rod bending some distance z versus some distance <z.

                                         

                                        Have you considered simply asking the manufacturer for rubber samples to doyour own "tests" on the material? This is going to be a toy for a child...couldn't very basic "experimental" tests be done instead of an FEA simulation. Nonlinear analyses with complicated materials can take a lot of tweaking and prior experience to yeild accurate solutions. I would think you just need to select a material that can support X amount of weight with Y amount of deflection, etc. Perhaps you are doing the FEA as a supplement or simply for fun, but with all due respect, it just seems a bit impractical to me.