17 Replies Latest reply on Apr 8, 2013 3:38 PM by Jared Conway

    Problems with bearing contacts

    Unspecified Unspecified

      My assignement evolves around the strength and stiffness of a structure of agricultural machine. I included the shafts in the frame analysis because i expect they have a significant effect (i could easily exclude the shafts and not have this problem at all). The shafts are attached to the frame with self alligning ball bearings which I simulated with two spheres, one is attached to the end of the shaft and the other one to the frame. They moved freely in the assembly, everything was fine, but when I did the analysis (static study), the spheres just won't move in relation to each other as expected because of the shaft flex under it's own weight. I tried defining the bearing connector but the manager won't accept the spherical faces (even tough the Solidworks Help says it should).

       

      I tried following this video:

      http://www.youtube.com/watch?v=NKlz39qWSz0

       

      I deleted the inner ring of the so called spherical bearing (just a hollow cylinder with the outter wall shaped like a part sphere)

      I supposed that clicking on the button for Self allignement would solve my problems but i get the message "Material not defined for one or more shells" which from past experiences could mean a bunch of problems in the model, one of them could be the gap in my model, which i clearly have, because i erased the inner ring. But the model in this video also has a gap and it is supposed to work.

       

      I also tried with cylindrical faces instead of spherical to fill the open space between the shell of a shaft and the inner surface of the outter ring but the same error massage is still there.

       

      I'm now pretty lost and i haven't found any similar problems anywhere else.

       

      I attached the model (I have 2011 version).

        • Re: Problems with bearing contacts
          Jared Conway

          Which study should we be looking at?

           

          What I would suggest is starting simpler. If you're going to constrain the assembly with a bearing, you can use a bearing fixture. On the shaft it would be a cylindrical splitline that defines where the bearing connects to it from another component. The other component is the "environment". Do that on both ends of the shaft with a gravity load and see if you can get it to run. You'll need to make sure that you stabilize one bearing so that the shaft doesn't rotate.

           

          Then once you have that, add the second shaft.

           

          Then you can add the first part of your housing. To connect the housing to the shaft, you'll use a bearing connector. The components need to be connected with a circular shell edge or cylindrical solid face.

           

          Try that and let us know where you get to.

           

          Note, I couldn't find any spherical faces. Can you send a screenshot of what you're talking about?

           

          Thanks.

            • Re: Problems with bearing contacts
              Unspecified Unspecified

              First of all, thank you for the answer.

               

              Yes, there are no spherical faces in that model because i transformed them in cylindrical because i kept getting the "face should be cylindrical or something" error when selecting the faces/edges in bearing connector. It doesn't matter which of the studies, they all have the same model, just different loads. Sorry if it is confusing, i was using a mix of English and Slovenian for file and study names.

               

              I contacted my mentor about this and he said that i should not use any contacts because they are supposed to mess up the results in FEA, I think it's because of boundary conditions and incompatible mesh?

               

              So i will try to make a node/point in the middle of the pipe/shaft on the section where the middle of the bearing is and connect it with truss elements to the edges of the inner spherical face of the outter ring. The trusses should be very stiff as I assumed the bearings to be nondeformable. This will allow the shaft to rotate freely in all three axes of rotation but not allow any lateral movements. I will let you know if this is possible in Solidworks.

               

              The other option yould also maybe be to use sliding frictionless contact for the spherical faces. I'll see.

               

              Bellow is the sketch of my plan with truss elements.Photo-0044.jpg

                • Re: Problems with bearing contacts
                  Jared Conway

                  what you've shown there is almost exactly what a bearing fixture does. i would highly recommend you setup a simple model and check it out. no contact is involved, so there might be a misunderstanding there. even the bearing connector is there to eliminate the need to develop contact between a bearing type connection that would otherwise be modeled with contact. And it would be strange to see incorrect results from contact.

                   

                  the method you describe looks like what you'd do in something like ansys or abaqus, building elements individually. you can do that, you're just going to have to think i through in advance (truss will have to be a weldment for example). but one of the beauties of SolidWorks simulation is that we have smart fixtures and BCs that allow you to automate the creation of these types of restraints that would otherwise have to be built manually.

                    • Re: Problems with bearing contacts
                      Unspecified Unspecified

                      Ok, I'll make a simple model and try the bearing fixture and the manual solution and compare results.

                        • Re: Problems with bearing contacts
                          Unspecified Unspecified

                          I realized Solidworks doesn't have truss elements built in. I'm a little lost as how to make this happen (idea, described above). Should i start with a sketch of a point and lines connecting it to the circle? if i want to add elastic properties to the lines to make them beams/trusses, how do i do it?ok i can define a section for the bemas and apply material but then it becomes a 3d part....

                           

                          The question is, how to connect nodes to the trusses, beams if they are not lines?

                            • Re: Problems with bearing contacts
                              Jared Conway

                              by default, solidworks weldments are beams, but if you edit their definition, you can turn them into trusses.

                               

                              to build beam/truss structures, you create a sketch and populate them with weldment profiles. there are tutorials for both in the standard tutorials that come with SolidWorks. it is also taught in the introduction to solidworks and simulation classes.

                               

                              to make them elastic, you'd apply the appropriate elastic modulus or use a spring element.

                               

                              if you make a solid using this method, you can right click and turn them into beams.

                               

                              With all that being said, if you haven't done so already, it would be good to do a search in the Solidworks KB for "bearing" and browse through the solidworks help. What you're trying to do is exactly what the bearing connector/fixture does.

                                • Re: Problems with bearing contacts
                                  Unspecified Unspecified

                                  Thank you very much for the answer.

                                   

                                  I tried using the bearing fixture with no luck. The study ran, but this is not an appropriate setting for defining bearings in my situation. It only connects the shaft to the sorroundings, and I need to only connect it to the main frame. I also tried with the bearing connector but was not able to make it run, the last error code i got was something about the missing spring third node, which i found no solution for.

                                   

                                  After that I went with the truss idea, which went ok, but I'm still not able to run it, the error message I'm getting is: "Please define bonded contact sets between beam and solid/shell." This is pretty strange because i made simple beams using weldments which all connect in one point (I also excluded joint trimming) and then just mated them to the split points i made on the edges of the outer ring. In the study itslef I defined beams as trusses and the program automatically put joint contacts at the ends of trusses. That's why I'm confused, I have no idea, where should i have bonded contacts in my model?

                                   

                                  For static analyses I don't need the bearings and shafts, I can replace them simply with bearing loads. Because the bearings have a few degrees of freedom in every direction the shafts also don't have meaningful effect on the stiffness of the frame. But I need the shafts in the natural frequency analysis.

                                   

                                  I attached the truss test model.

                                    • Re: Problems with bearing contacts
                                      Jared Conway

                                      hi, can you also upload the bearing connector model? i think that is the one that you'll have the most luck with. my guess is that your mesh was too coarse and/or you didn't have at least one of the bearing connectors set with stabilization.

                                       

                                      Are these all being done on a simplified model or on the full model?

                                        • Re: Problems with bearing contacts
                                          Unspecified Unspecified

                                          I attached two files, okvir_sest_mid_surf_2_test is the full model with bearing connectors and the truss_test is the simplified one also with bearing connectors and bearing fixtures which actually works, but the results aren't correct as the weight of the shaft doesn't transfer on the frame.

                                            • Re: Problems with bearing contacts
                                              Jared Conway

                                              bearing fixtures are with respect to the environment, bearing connectors are relative to the components. since you have both, your shaft is really just supported by the environment. suppress those then you have bearings that are relative between the shaft and the housing. your simulation will fail. if you turn on stabilization on one of them, your simulation will succeed but the results will look a bit wonky. that is because stabilization is a subset of the soft spring command that is really just for troubleshooting. the reason this succeeds is because there is a small inbalance in the forces that cause a rigid body motion that rotates the shaft relative to the frame which is a no no for static analysis. so what I did is I got rid of the stabilization in the bearing connector and replaced it with a spring at the bearing connection area. that bearing was given 100lb-in stiffness in the shear direction. run that and you've got a solution that looks pretty reasonable. now the question will be is that ok from a restraint perspective or not. If not, you'll have to play around with some conditions that hold things together.

                                              • Re: Problems with bearing contacts
                                                Jared Conway

                                                note, i didn't look at your other example with the truss. if there is something about bearing connectors that doesn;'t work and you realy want to use that method, I'll take a look at that one as well.

                                                  • Re: Problems with bearing contacts
                                                    Unspecified Unspecified

                                                    Thank you for the solution idea, I'll try adding the stiffness in the bearing and I'll see what the results will be. I am pretty sure though that this won't be ok with my mentor who wants a very "pure" model, trusses were his idea and I think they should work but I'm suspecting I made some stupid mistake. So if you'll have time, please have a look at it.

                                                      • Re: Problems with bearing contacts
                                                        Jared Conway

                                                        What does pure mean? What is unpure about he bearing connector? Have you taken a look at the swx kb? I think you will be very surprised at how close it is to what your instructor suggested. Bolt connectors, bearing connectors...etc are short cuts to using the methods like your instructor suggested.

                                                         

                                                        The only thing I can think of is the extra spring connector. But like I said, there are many ways to eliminated it so that you can get a static solution.

                                                          • Re: Problems with bearing contacts
                                                            Unspecified Unspecified

                                                            Don't think that i don't agree with you, but he is my mentor and I have to listen to him. Also, shortcuts aren't in his vocabulary. Ok, I understand how the connector works, but the model of the frame still doesn't behave like it's supposed to.

                                                            The truss sollution on the other hand eliminates all the problems (in theory), I already have it built but I think I made some stupid mistake and I don't have years of experience from Solidworks.

                                                              • Re: Problems with bearing contacts
                                                                Jared Conway

                                                                How does it not behave properly? Please upload the model.

                                                                 

                                                                Regarding the other method, if you get it right. You are still going to have a rotational stability problem, how are you going to deal with it? Or, it is going to be infinitely stiff. If that is the case a self aligning rigid bearing with one of them being fixed will be the same.

                                                                  • Re: Problems with bearing contacts
                                                                    Unspecified Unspecified

                                                                    I tried the "stabilize shaft rotation" on one of the bearings in both the test model I made for the bearing connector and the full model. In the test model, the simulation ran but the results are strange as the shaft left the assembly (I attached the model so you can see). In the full model, whatever I do, the simulation fails at 18.2% and I get the "Error in defining Spring third node". I searched the web and this error occurs in some bearing and bolt connector cases. That is why i have no idea how to resolve this using the Bearing connector. Can you also explain why the shaft rotation is such a big no-no, I couldn't find any info regarding this.

                                                                      • Re: Problems with bearing contacts
                                                                        Jared Conway

                                                                        see comments above about what stabilize shaft rotation means and how it may affect the results and what i recommended to deal with it.

                                                                         

                                                                        as for rotation, you're attempting to do a linear static stress. the emphasis on static. as soon as you add rotation you don't have a static analysis anymore and you have invalidate the underlying fundamentals for the analysis. if you can't control it, you need to move to a motion or dynamic analysis first but generally you can make it static. for example what is the worst case? if one of the bearings seizes? start with that kind of boundary condition.

                                                                         

                                                                        it might be helpful to post a picture of what you're seeing and what version/service pack you're using. the model as received ran without issue in 2013 sp2.0. but it does have the assymetric results that i mentioned above which need to be dealt with using another BC other than the stabilization.

                                                                         

                                                                        your full assembly is a long ways from being ready to be analyzed. maybe your latest version isn't uploaded? what i'd suggest is excluding all the components except for the ones involved in the bearing connector connection. fix something and get that part running. taht will help you minimize what you need to troubleshoot so you can focus on what you need to focus on to get it running. once you get it running you can start adding more parts. some examples of things that are going to be an issue are shells right on top of other shells without the appropriate contacts applied to them. overlapping solids and shells. start simple and then add as you get more experience and as things start working.

                                                                         

                                                                        on your truss example, it looks like you're trying to use component contact (bonded) between the beams and the other components. you'll need to use contact sets for this because automatic bonding (component contact) only applies to certain elements. you'll have to check the help based on the version that you're using. just to try it out, i excluded most of the truss elements and used a contact set, it still had trouble running because of stability. but once I changed to beam elements instead of trusses, it ran. so adding all of you trusses should help deal with that once the right contact is applied. similar to above, i'd start simpler because it will make it easier to troubleshoot if you run into problems.