16 Replies Latest reply on Jun 5, 2012 2:24 PM by Rich Jones

    Unable to get the right displacement......

    Avishek Kar

      I have been trying to perform an static analysis on a manhole cover in SolidWorks Simulation but unable to get the desired displacemnt. The desired value is below 1.5mm but after repetitive attempts the best value I got is 1.7mm. Its an iges file, which I have converted to SolidWorks part, using the import diagonistic and feature recongnization tools.

       

      The parameters are as such

       

      Material Used- Ductile Iron.

      The bottom face of the cover is fixed.

      Force = 14300N on the top face of the cover is concentrated in the circumference of a circle of 250mm dia at the centre.

       

      As, I am new to Simulation, there can be some errors. Kindly guide me on this issue. I have attached the files for further reference.

       

      Thanks & regards

       

      Avishek

        • Re: Unable to get the right displacement......
          Timothy Holman

          Hello,

           

          I tried to view your files but when i opened both of them they were empty.  Nothing on the iges and the parts were not with the assembly.

          • Re: Unable to get the right displacement......
            James Canney

            Avishek,

             

            Some questions.

             

            - Why do you think that the deflection should be 1.5mm, your cover is B125 rated so your load should be 125000N on the test block, unless you are allowing for an additional FOS outside of EN124.

             

            - Are you trying to look at the test load or the permanent set of the cover? Depending on which you are looking at then the important things to look out for are the FOS against the Yield strength of the material in the case of permanent set, or the FOS against the Ultimate strength if looking at the full test load.

             

            - Your cover may deflect more than the standard allows during the test, but the recovery of the cover is important once the test load is released, this is why you should look at the FOS against the Yield strength, along with your deflection results.

             

            - Make sure your contact constraints are set up correctly. I would not fix the base of the cover, but I might fix the base of the frame where it would sit on the concrete and then use no penetration contacts between the frame and the cover and the cover and the test block. This is very important to get accurate results.

             

            - One step further would be to model the base of the concrete and fix this on the base, then use no penetration contacts for the rest of the connections, this will give you the most accurate results.

             

            - I would use symmetry to speed up the tests, you should be able to use 1/4 of your model.

             

            I hope this helps a little.

              • Re: Unable to get the right displacement......
                Avishek Kar

                Canney,

                 

                Thanks for your concern. Ya you are right the load is 143000N, I missed one zero. I tried the methods suggested by you, buts it takes hell lot of time, as I still on a learning curve of SolidWorks Simulation, could you please tell me how I can get the symmetry done here. So that I can easily get the analysis done and come up it the right solution.

                 

                One more thing what is this B125 rating which you mentioned?

                  • Re: Unable to get the right displacement......
                    James Canney

                    Your frame has B125 on it and EN124 on it as well.

                     

                    EN124 is a standard - Full title BS EN 124:1994 - It covers gully and manhole tops for vehicle and pedestrian areas, this is a harmonised European standard.

                     

                    B125 is one of the load class ratings in the standard, the rest are:

                     

                    A15

                    B125

                    C250

                    D400

                    E600

                    F900

                     

                    The main point being that the numbers relate to the load in kN that the covers must reach. (There are many exceptions to this as defined in the standard)

                     

                    You really need to read and understand this document, as it covers the design and testing of this type of product in great detail. One other thing from your first post is the load application on the cover, in the standard you will see that the load should be applied through a test block that is placed on the cover, if you apply the load in SWX directly to the cover you will get incorrect results.

                     

                    - Your product is (almost) symmetrical in two planes, you can therefore 1/4 the product and apply symmetry restraints to all of your cut surfaces, remember to 1/4 your applied load as well. There is one part of your frame that does not have this symmetry, if it was me and I was only interested in the cover, then I would ignore this. This will greatly speed up simulation. But depending on your system specs you could well be and hour or two per simulation.

                     

                    - I still don't understand your load, 143000N is not a part of EN124, unless you are looking for additional safety.

                     

                    One final point, and please don't take this the wrong way. As you don't appear to know about EN124 and B125 I am assuming you are testing this on behalf of a client based somewhere in Europe. Be carefull about the info you post on line, I am not sure if it is confidential or not, but I design these types of products as well every now and again and we always interested to know what our competitors are up to.

                      • Re: Unable to get the right displacement......
                        Avishek Kar

                        Yes James you are right its for a client, not based in Europe so no problem of competition. Actually its just a sample given to us for bench marking SolidWorks Simulation. As I am new to simulation, I am facing the problem with it. I followed the instructions given by you but the following message comes each time." Equilibrium satisfaction is not achieved. Do you want to exit?

                         

                        untitled.JPG

                        Kindly help me with this. I know I asking for too much, but I am in some deep sort of trouble.

                         

                        Truly,

                         

                        Avishek

                          • Re: Unable to get the right displacement......
                            James Canney

                            Can you post an image of the whole set up of your test for me? I suspect that you have a problem with one or more of your restraints.

                             

                            If you are comparing actual test data to FEA you will need to be very sure of the material properties that you are using for the FEA.

                             

                            Thanks

                              • Re: Unable to get the right displacement......
                                Avishek Kar

                                Here are the images 1st one the attempt made on the cover only and 2nd one is with ths assembly..1st Cover.jpg

                                2nd attempt

                                assem.JPG

                                 

                                 

                                The 2nd attempt has the following error

                                error.JPG

                                  • Re: Unable to get the right displacement......
                                    Kevin De Smet

                                    Try to put symmetry on all the cut faces, not entirely sure whether you would want to put cyclic symmetry on them all though.

                                    • Re: Unable to get the right displacement......
                                      James Canney

                                      Avishek,

                                       

                                      Sorry I am pushed for time at the moment.

                                       

                                      I would not use circular symmetry, I would add planar symmetry to all of your cut surfaces, the top option in the advanced section of constraints, I would also make sure that I use a test block if testing to the standard, it should be 250DIA with a 3mm radius on the bottom surface, maybe 30mm thick, the test block should also have the symmetry constraints added, apply your load to the top of the test block.

                                       

                                      If I get the chance over the weekend I will give it a try.

                                        • Re: Unable to get the right displacement......
                                          Avishek Kar

                                          James,

                                           

                                          I exactly followed the steps suggested by you, but this I got some errors corresponding to large displacement and ultimately resulting into to the failure of the solution. I am getting clueless about it.

                                          • Re: Unable to get the right displacement......
                                            Avishek Kar

                                            James,

                                             

                                            I know you have crunch of time, but I kindly request you to please check the model for once because I am really not able to get to any where near to the correct answer. I have done lots of R&D on it, but still no solution. I will be grateful to you for your this kind heartedness.

                                             

                                            Regards

                                             

                                            Avishek

                                              • Re: Unable to get the right displacement......
                                                James Canney

                                                Avishek,

                                                 

                                                I finally got the chance to run your model.

                                                 

                                                The reason you are getting the large displacement warning is because the cover deflects a lot. You should read up in the help about Large displacement.

                                                 

                                                I ran the model with ductile iron material and a B125 load, not the higher load that you have described above. I also used mesh refinement on the cover as this is the part that will fail.

                                                 

                                                I also ran the model without large displacement turned on, so my results would be less accurate and overstate performance.

                                                 

                                                I am not going to give you any kind of analysis on wheather the product is suitable or not, but I would guess the the cover might bend around 14mm under a B125 load during the test. So my main question is why you think the cover should only bend 1.5mm? You also need to look very closely at your FOS plots.

                                                 

                                                Are you comparing it to a real live test on an actual part? If so when was the deflection measurement taken, during the test, or once the load had been removed?

                                                Are you comparing it with another FEA system? If so was it set up correctly? What materials, loads, meshes and constraints?

                                                 

                                                I think you need to sit with someone who can go through your analysis and look at all of the deflections, stress levels in certain areas, and the resultant FOS plots, and what you are trying to compare the test data to. Can your VAR give you any assistance?

                                                 

                                                I would post some images but my IT policies wont allow it.