26 Replies Latest reply on Jun 27, 2013 9:07 PM by Alexander Quek

    Deflection for model

    Alexander Quek

      Hi All,


      Hitting a brick wall here, hoping some of you might be able to help me out. Think this should be rather straight forward but somehow seem to be getting errors where the cut-extrudes are.


      Just want to test for deflection when a load in placed on the model with fixtures placed 2920mm apart.


      Load points.jpg

      Any help will be greatly appreciated.

        • Re: Deflection for model
          Mike Pogue



          I'm guessing you can't mesh this? That's not too suprising, given the number of tiny features. If you want to mesh the entire model, either supress tiny features or turn up the tolerance, which will allow the mesher to ignore them. I'd probably not mesh the entire model, though. This looks like a (pseudo) plane strain situation. Even though you can't take a 2d section, you can cut out all but the smallest repeating section and you should get the same answer. This will let you use much much smaller elements, which will increase your odds of success.


          I'd probably do some combination of the three.

          • Re: Deflection for model
            Jared Conway

            what errors are you getting?


            assuming you're having trouble meshing, +1 for mike's response. needs to be simplified. shells, symmetry, 2d...something. or you're going to have to have a megapower computer to solve the problem.

            • Re: Deflection for model
              Alexander Quek

              Hi Mike and Jared,


              Thank you both for your replies and suggestions, am rather new to Solidworks simulation and trying it out with trial and error process.

              Yes, am having heaps of trouble trying to mesh the model and it would give an error at each and every extrude cut or boss.


              Would try out the suggesstions pointed out.

              • Re: Deflection for model
                Alexander Quek

                Hi All,


                Did a revamp of the model and strip it down to it's bare minimum.

                Am able to mesh model and achieve simulation results.


                My question here, would the strip down (after simplifying) simulation model produce the same results as the actual (before simplifying) model?

                But since we can't mesh the actual model we wouldn't know?


                BEFORE Simplifying

                Actual Model.png

                AFTER Simplifying

                Plain Model.png

                Simulation Test Results

                Deflection Test.png

                  • Re: Deflection for model
                    Mike Pogue



                    I don't know the answer, but my suspicion is that if you remove a bunch of holes and stiffening ribs you change the result in unpredictable ways. You have also probably eliminated most of the buckling modes.

                      • Re: Deflection for model
                        Jared Conway

                        I'm with mike here.


                        one potential solution, build a smaller version and test simplified vs full and see what the deflection differences are. that will help you understand what the potential for error is between the models.


                        it also looks like you're using solids. take a look at beams and shells, you might be able to get this problem down to a reasonable setup with them.

                      • Re: Deflection for model
                        Bill McEachern

                        In your simpifications you need to try and approximate the stiffness. So stiffening ribs are not likely something you can ommit. The holes...maybe turn to slots or remove and add a stress riser of 3 if they are not near a boundary. What elements did you use? Shells? The analysis looks like it may require a non linear solution but it depends on the deflection - if it deflects more than about 1/2 the strucural depth then NL effects are emerging to a significant degree. Are the segments structurally connected? What does the response of one look like compared to you simplified version of one?

                        • Re: Deflection for model
                          Brian Zias

                          How much RAM do you have on your computer? Since you are interested in displacement, you might be able to get away with "Draft" elements for a first pass. Also, looks like you can use Symmetry down the long axis to cut the problem in half. Finally, be sure you're using the Curvature-Based Mesher, which can adapt itself to feature size...   See if that will mesh using finer settings. No guarantee and I have to echo the other suggestions, but maybe these brute force tips will get you through this one and allow you to compare simplified to non-simpliieid.




                        • Re: Deflection for model
                          Alexander Quek

                          Hi All,


                          Thank you for the insightful and interesting methods, gladly appreciate each and everyone of them.

                          Have made some changes to the model which produced some advancement from where I first left off.


                          Have remodel this part in 'sheet metal' module and the ribs/extrusion are made using a 'form tool'. In addition to that have added in a 2mm radius on each of the corners of the profile.


                          Any further comments will be much appreciated.


                          Have look below:


                          1) Added 2mm Radius on the coners

                          Addition of Radius.png



                          2) Able to mesh the model but far from perfect

                          Completed Mesh.png



                          3) Trying to simulate this part placed on supports that are 40mm from either end, used 'split line' to draw the 40mm and  add in a roller/slider fixture. Problem we see here is the missing mesh in-between the fixtures from both ends.

                          Problem 1.png



                          4) Same issue as stated in number 3; missing mesh

                          Problem 2.png

                          • Re: Deflection for model
                            Alexander Quek

                            Hi All,


                            Once again have made another attempt on this with the suggestions all of you have given.

                            This time, have drawn up the model in 'Solid' then 'Shell' it in mid plane.

                            Assigning shell thickness in simulation and meshing this time round is a breeze incomparison to what was previously done with a solid or sheetmetal model.



                            All the errors that were pointed out previously doesn't exist anymore:




                            Looking at results:




                            The displacement calculated in simulation is a far cry from an actual test done.
                            Actual: 8mm

                            Simulation: 1mm


                            Just wondering could I have missed out anything here or done something wrong?

                              • Re: Deflection for model
                                Jared Conway

                                alex, draft or high quality elements?


                                are you confident that the loads and restraints in simulation match up to what you did in your physical test? (assuming here that the components also match up)


                                before you answer those, you might want to do a couple of quick checks with hand calculations. if you estimate the stiffness of your beam, does a hand calculation match the deflection you get in the physical test? does simulation match under those same conditions?

                                • Re: Deflection for model
                                  Patrick O'Hern

                                  When you did your physical test, were both ends of the beam held tight in a fixture, or were they able to "float"?  It looks like you have both ends fixed in your simulation, which would limit the amount of deflection as the material has to stretch in order to deflect down. 

                                    • Re: Deflection for model
                                      Alexander Quek

                                      Hi Patrick and All,


                                      Yes, you are right when you say that physical test was done without fixtures held tight on both ends. Bascially, test specimen was placed on supports on both ends.


                                      Please see pictures below for steps taken in Solidworks to create simulation:



                                      1) Halved model in shell

                                      1 Half Shell Model.png



                                      2) Added 'Split Line' for use of Roller/Slider fixture as supports on both ends

                                      2 Split Line.png



                                      3) Selection of shell model in simulation to assign 1mm thickness in total

                                      3 Shell Definition.png



                                      4) Edges selected for symmetry

                                      4 Symmetry.png



                                      5) Roller/Slider fixture on face where 'Split Line' was added in image 2

                                      5 Roller Slider Fixture.png



                                      6) Translation fixture added on selected face, model can only move in Y axis

                                      6 Translation Fixture.png



                                      7) 10kg or 101N Force added in total on selected faces

                                      7 101N Force.png



                                      8) Isometric view of Forces, Fixtures and Symmetry on model

                                      8 Force Fixtures Symmetry.png



                                      9) Mesh settings used

                                      9 Mesh Settings.png



                                      10) Isometric view of simulation result

                                      10 Isometric View Displacement.png



                                      11) Side view of simulation result

                                      11 Side View Displacement.png

                                        • Re: Deflection for model
                                          Jared Conway

                                          "placed on supports on both ends"


                                          would you agree that means that the contact between your part and the supports would be a line vs the flat that you have created with the split line?


                                          and that also at that line contact the component can rotate/pivot on that line and that the component could slide?


                                          if so, you might want to reevaluate that boundary condition. by setting a roller slider all that you've done is set the nodes on that face to zero in the normal direction. so it will slide but only on that face and only in that plane. it will also remain flat.


                                          you might also want to think about what your z direction restraint is doing on the back face.


                                          consider a similar analysis on your load. you might want to see what happens if you apply the displacement you want at the symmetry face and see what load it requires. do you think your load creates that wallow in the middle at the center? (red)


                                          a couple suggestions on this model:

                                          1. could it be be made quarter symetric?

                                          2. i might be reading your screenshots wrong, but what about applying your x directino restraint at the symmetry plane?

                                            • Re: Deflection for model
                                              Alexander Quek

                                              Hi Jared,


                                              Thank you for your suggestions given.
                                              That has definitely helped me understand better in thinking where and what fixtures to use.


                                              If I have understood you correctly:


                                              1) Y Axis fixed on the "Supports"


                                              Y Axis Fixed.png


                                              2) On Symmetry Plane, X and Z Axis Restrained


                                              Symmetry Plane Fixed X and Z Axis.png


                                              3) Results




                                              P/S: Reading from other posts and from other sources on net, since we are using half model, the Force applied will also need to be halved.

                                                • Re: Deflection for model
                                                  Jared Conway

                                                  Getting there. How did you choose the rotational restraints?


                                                  Is it deflecting the way it did in your physical test?

                                                    • Re: Deflection for model
                                                      Alexander Quek

                                                      Hi Gared,


                                                      Tried re-evaluating the fixtures.


                                                      Symmetry plane:

                                                      Shell Models.png

                                                      Symmetry Fixtures.png


                                                      Fixtures on "Support", by looking at part physically placed on supports:



                                                      • Translate freely in the X and Z axis
                                                      • Restraint in the Y axis.



                                                      • Rotate freely in the Y axis
                                                      • Restraint in the Z axis.

                                                      Not so sure about the X axis. Looking at it, I don't think the part will be able to rotate freely in the X axis. But when I tried applying a restraint on the X axis for rotation, I get an error stating there isn't enough fixtures.


                                                      End up using these settings:

                                                      Y Axis Fixed Only Z Rotation Fixed Settings.png



                                                      Y Axis Fixed Only Z Rotation Fixed Isometric View.png

                                                      Y Axis Fixed Only Z Rotation Fixed.png


                                                      Although this time round, the results for displacement at 7.15mm seems more realistic and closer to the actual test done, the fixture for rotation on the X axis still puzzles me. Can only guess that if a restraint is applied to the rotation on the X axis, the part will not be able to produce a deflection and be fixed as a flat piece.


                                                      Any further critique will be appreciated.

                                                        • Re: Deflection for model
                                                          Jared Conway

                                                          the x rotation, i don't think you should need to restrain that but then you have no restraint in the X direction which might cause things to get upset. but i don't think that restraint will cause things to be "incorrect" either. i'd continue playing with different settings on a simpler model to see what you get.


                                                          on your symmetry plane, consider locking down a point in the x direction and seeing if it runs.


                                                          but it looks like you're getting pretty close.

                                                      • Re: Deflection for model
                                                        Patrick O'Hern

                                                        You currently have your force evenly distributed across each beam.  Is that how your physical test was set up, or did you have a single load in the center?