9 Replies Latest reply on Jul 24, 2014 3:08 PM by Jared Conway

    Modal Analysis frequency value differ solidworks and ansys

    Kumar Dandapani

      Hi Friends,

       

      I am doing modal analysis for cantilever beam i am getting frequency two times same value. Why i am getting Every frequcensy two times sam value?. Please help me to solve this. Thanks in advance.

       

      Regards,

      A D Kumar.

       

      Note: For the same problem in ansys getting one time only the frequency value. for your reference i enclosed web link

      http://www.mece.ualberta.ca/tutorials/ansys/IT/Modal/Modal.html

        • Re: Modal Analysis frequency value differ solidworks and ansys
          Nicholas Luyster

          Hi Kumar,

           

          It's hard to say what's going on without seeing what you have done in SolidWorks.  If you have a cantilever beam though and the frequency is 2 times what it should be, I'm getting that an improper restraint is to blame.  Check your fixtures and see if you have an immovable fixture where you should have a completely rigid fixture.

           

          All the best,

           

          Nick Luyster

          SolidWorks Simulation Training

            • Re: Modal Analysis frequency value differ solidworks and ansys
              Kumar Dandapani

              Hi Nick Luyster,

               

              Thanks for your Reply, Kindly check my model which i attached. I have defined one end is fully fixed other end is free. In this situation i am running Frequency analysis. I am not getting any error like what your saying improper restraint. So please check my model and weblink which i mentioned in my post. I am getting first and second frequency value remains same like that its replicate for 3&4, 5&6th... So please review and help me.

               

              Elastic Modulus 206800e6 N/m2.

              Density             7830 Kg/m3

               

              Dimension width 10mm thickness 10 mm and length 1000 mm.Thanks in advance

               

              Regards,

               

              A D Kumar.

            • Re: Modal Analysis frequency value differ solidworks and ansys
              Jerry Steiger

              Kumar,

               

              I assume you mean that the frequency calculated for each of your modes is twice the frequency that ANSYS calculates?

               

              I would first check that your material properties, particularly Young's Modulus and density, are the same as used in ANSYS. Then I would check to make sure that your dimensions, l, w, and t, are the same. (Actually, w shouldn't matter.)

               

              Jerry S.

                • Re: Modal Analysis frequency value differ solidworks and ansys
                  Kumar Dandapani

                  Hi Jerry,

                   

                  Thanks for your Reply, Kindly check my model which i attached. I have defined one end is fully fixed other end is free. In this situation i am running Frequency analysis.So please check my model and weblink which i mentioned in my post. I am getting first and second frequency value remains same like that its replicate for 3&4, 5&6th... So please review and help me.

                   

                  Elastic Modulus 206800e6 N/m2.

                  Density             7830 Kg/m3

                   

                  Dimension width 10mm thickness 10 mm and length 1000 mm.Thanks in advance

                   

                  Regards,

                   

                  A D Kumar.

                    • Re: Modal Analysis frequency value differ solidworks and ansys
                      Jared Conway

                      Your model isn't getting attached.

                       

                      It would be helpful to list your outputs and your expected outputs so that we can verify we are looking at what you want us to look at.

                        • Re: Modal Analysis frequency value differ solidworks and ansys
                          Kumar Dandapani

                          Hi Jared,

                           

                          Thanks for your Reply, I have defined one end is fully fixed other end is free. In this situation i am running Frequency analysis.So please check Frequency Value and weblink which i mentioned in my post. I am getting first and second frequency value remains same like that its replicate for 3&4, 5&6th... So please review and help me.

                           

                          Elastic Modulus 206800e6 N/m2.

                          Density             7830 Kg/m3

                           

                          Dimension width 10mm thickness 10 mm and length 1000 mm.Thanks in advanceCompare.JPG

                          EXpected to get same frequency value with ansys and solidworks.

                           

                          Regards,

                           

                          A D Kumar.

                            • Re: Modal Analysis frequency value differ solidworks and ansys
                              Shaun Densberger

                              There isn't anything wrong with the SW answer. You're geometry has symmetry (it's a 10 mm x 10 mm square), so there is going to be mode sets that has the same eigenvalue (ie frequency), but orthogonal eigenvectors (ie mode shapes). The ANSYS source you've provided has, for whatever reason, omitted the other parried mode.

                               

                              Let's assume that the cross-section of this beam is in the XZ plane. The first mode will have a mode shape characterized by the beam oscillating in the x-direction, and the second mode will have the beam oscillating in the z-direction. However, both the first and second mode will have the same frequency. In fact, which mode is calculated as the first (either x-direction or z-direction) is arbitrary.

                      • Re: Modal Analysis frequency value differ solidworks and ansys
                        Shaun Densberger

                        Hmmm, this is interesting. When I solved this with default settings (i.e. 5 modes) I get:

                         

                        Mode No.Frequency(Hertz)
                        18.305
                        251.922
                        352.021
                        4145.55
                        5145.55

                         

                        Now, this fits with the results from ANSYS, but what's interesting is that Mode 2 isn't ~8.3 Hz and that the solver doesn't get this until I request at least 7 modes. It's well documented that the accuracy of the lower modes increases with the more modes requested from the solver, but I'm surprised that it flat out missed a mode.

                         

                        Anyways, I can easily replicate the values from ANSYS, so my assumption is an error in your set up.