28 Replies Latest reply on Aug 25, 2010 12:15 AM by Satit Nilyai

    Very Large Structural Simulation

    adam nikel

      Ok this structure 72 ft leg to leg, its a massive structure and im having serious problems meshing it even with a heavy duty computer. (the problem is the whole thing is made up of 2 7/8 and 1 in pipe with a .083 wall thickness) I tried mesh control along with a curved mesh instead of a standard and it kinda helps but it randomly doesnt grab certain components of assembly, there 2 legs and 4 top curved peices. no welds, no bolts, were just testing the connection as basically one peice.

       

      I been told try to change the mesh type to a beam mesh, in solidworks 2010 how do u go about that? or even in older versions not much has changed. any suggestions would be greatly appreciated

        • Re: Very Large Structural Simulation
          Don Vanzile

          If you go into the Study and select all of the bodies and right-click, there is an option "Treat as Beam".  Also, try doing a symmetrical study if that's what it is.

          • Re: Very Large Structural Simulation
            Michael Feeney

            As SolidWorks is largely a CAD program, its FEA "simulation" isn't as good as Abaqus. I'm doing a lot of work with similar structures believe it or not. I had to validate my hand calcuations with two software packages, namely, Abaqus and SolidWorks. I am vary familiar with Abaqus, and SolidWorks was pretty easy to pick up. I used SolidWorks because it was available and relatively capable to do the job. My Abaqus sims took 30 seconds to run and my SolidWork sims took 10-15minutes. Herein lies the 2 main issues:

             

            1. The meshing is very automated and has the tendancy to do overkill and bog the CPU.

            2. The model is default 3D solid.

             

            Because SW is .....interesting, it will try to mesh your thin-walled pipe with elements through the thickness. That means the elements have to be SUPER small and thus you would be taking the "elephant gun to kill a flea" route. Now I struggled with this for a while, but finally, with the help of some of the guys on this site, I figured it out. Either, download Abaqus and use that (this will take a bit of learning though) or change your pipes to surfaces and do shell meshing. For thin parts this is standard procedure. So now your asking...how do I do that:

             

            There is a thread I'll link that helps, but basically you go to each part, make a midsurface, delete solid bodies, and then mesh with shells.

              • Re: Very Large Structural Simulation
                Michael Feeney

                Here is the link to the thread I was referring to.

                https://forum.solidworks.com/message/171090#171090

                 

                My tips:

                 

                You have your Assembly with mates and everything is constrained. Now, go to each of your unique parts and create the midsurface (insert--->surface--->midsurface: select the 2 walls you want the surface to be between). Once you have the surface made, look in the tree where your features are for the part and find solid bodies, delete the solid body. Now you will just have a surface (a very thin-walled cylinder for a pipe for instance). Once you have this done for each of your parts go back to your assembly. You will notice all your mates are messed up. The trick I found was, suppressing or deleting the mates and simply fixing everything in place (literally right clicking and fixing the components). You know that this is OK to do because you already made the assembly with the parts in the right place when they were 3D solids.

                 

                That was all prep work for entering the sim module. In the Simulation Module you will now have to establish the standard stuff like material, etc... Instead of the constraints you would normally apply to 3D parts, you need to setup contacts instead. Once you have the boundary conditions and contacts setup, you can then apply thickness to each surface and then mesh with shells.

                 

                If you have any further questions let me know.

                 

                Also, I agree with the symmetry technique....that's FEA 101

                 

                **EDIT**

                This is valid approach, but a roundabout one at the same time. For your particular model use beams and watch the video below.

                  • Re: Very Large Structural Simulation
                    James Denney

                    Regarding your "insert midsurface" technique...how does Simulation handle the following situation? Let's say you have a 12" length of I-beam welded between two 1" steel plates of some square dimension. I want to model this in simulation with beam and shell elements. So, first I decide to insert a midsurface as you describe so I can automate the meshing in simulation. Now, when I insert that midsurface and delete the solid body of the 1" plates, the mates are messed up as you pointed out they would be.

                     

                    So how do I proceed? Theoretically, my I-beam is 12" long and mid-surface to mid-surface of those plates is 13". So do I offset the midsurfaces from the ends of my I-beam by 0.5"? Do I move the midsurfaces to mate with my beam ends even though this does not geometrically represent the real setup of the structure?

                     

                    I guess my point is...converting solid parts to surfaces throws off dimensions in the model, so to speak, depending on how they are originally mated. Any implications to the simulation results because of this? Picking up FEA here on my own, as well, so just something I thought of while applying your technique.

                      • Re: Very Large Structural Simulation
                        Michael Feeney

                        I know what you're are saying. I believe this is taken care of when you define your shell thickness. The parts could appear as though they are not touching, but if the contacts are defined appropriately and the thicknesses are correct, I believe the model will turn out a good simulation.

                         

                        For that particular setup, I would actually be inclined to run the I-beam with beam elements and the plate as a shell or solid.

                  • Re: Very Large Structural Simulation
                    Michael Feeney

                    You could use beams too, like Bill said in that other thread. Both shells and beams are valid. I'm not familiar with beams in SW on the other hand.

                    Perhaps this will help too:

                     

                    http://www.youtube.com/watch?v=jKnfo6I6zJU

                     

                     

                    **EDIT**

                     

                    just messed around with beams. It's quite easy actually. If you have mixed meshing solids and beams or shells and beams, you have to make sure you get the contacts correct (but this is not an issue for you because you will be using all beam elements). My solid model, shell model, and beam model all come out with the same result. I am now thinking that I wished I used beams for my project because it's very easy.

                    • Re: Very Large Structural Simulation
                      Michael Feeney

                      Think you could just send your file? I'll take a quick look at it tonight. It wont take long. Once you see it done...you'll be set for most of the sims you have to do in the future.

                        • Re: Very Large Structural Simulation
                          adam nikel

                          OK that works ill attach it, please i apprecate the help. i just need it to the point well i can add restraints and forces, and run it. can u send me a word documant explainng what you did?

                           

                          and thank you again

                          • Re: Very Large Structural Simulation
                            adam nikel

                            I been working on these thing for at least 5 hours a day for almost 2 weeks now, i having some serious issues. Like i mentioned before i appreciate the help. Im completely self taught in FEA and i never even touched the shell FEA features

                              • Re: Very Large Structural Simulation
                                Ryan Werner

                                In case the shell method does not work out here is an analysis of your assembly using beams.  I played wtih your models and turned them into weldments to help make using beams easier.  You will notice that the joints are not quite perfectly defined but it is a start all the same.

                                 

                                Ryan W.

                                  • Re: Very Large Structural Simulation
                                    Michael Feeney

                                    Thanks Ryan. This is very informative, I haven't played around with weldments. Do you know why he couldn't convert to beams with his original model? I guess when you have a part file that isn't just a pipe or square tube you have to use weldments to make beam elements.

                                      • Re: Very Large Structural Simulation
                                        Ryan Werner

                                        He couldn't do it originally because everything he had modelled was merged into one part.  So in Simulation there was no option to treat as beam because it saw the whole section as a single part.

                                         

                                        I started by separating all of his features and turning it into a weldment but keeping his sweeps etc. for the individual features.  Once I had all the bodies separated and distinct I was able to treat them as beams in Simulation, however, for some reason that I was not able to figure out the neutral axis of the two main arches was screwed up and would therefore not let me create accurate joints.  Since the arches are round without any defined edges in the direction of their neutral axis I was not able to redefine them.  

                                         

                                        So, that is when I just started over with Sturctural Members and re-created the parts.  It worked a lot better in Simulation but I will say still not as well as one would hope.  It was still very touchy to get the joints defined accurately.  For some reason Simulation would randomly leave out some beams one time and others a different time.  I would like to see what a VAR has to say about that one.  I do know that curved beams in Simulation is relatively new (this year or last) so maybe that has something to do with it.  Anyway, with more work you could probably get a better joint depiction.

                                         

                                        The important thing to remember with weldments is that if you are creating one without using any structural members (just extrudes, sweeps, etc.) then you need to hit the weldment button first thing so that it does not by default merge all the bodies as you create them.

                                         

                                        Ryan W. 

                                • Re: Very Large Structural Simulation
                                  Michael Feeney

                                  You should double check this with other people, but I think you need to make new part files. You made them all as one piece. If you make your arch sections with separate parts like:

                                  1. Outer Arch

                                  2. Inner Arch

                                  3. Cross Member

                                  4. Plate

                                   

                                  then you should have the ability to make beams. As it is right now, I'm a bit stumped. I thought you had separate parts that could be converted to beams (which is the right way to go here). This would be a very very very quick problem in ABAQUS.

                                  • Re: Very Large Structural Simulation
                                    Michael Feeney

                                    Do not try to do this with shells.

                                    • Re: Very Large Structural Simulation
                                      adam nikel

                                      Thanks for the help but i cant view or even open any files till i get out of work. they only have 2007 version of solidworks

                                      • Re: Very Large Structural Simulation
                                        adam nikel

                                        no no,      i work two jobs, the place i work during the day does sheet metal work with solidwords 2007. I work as a consultant with my teacher and we use 2010. I just cant open the new files at work because they have 2007 but once get to my other office that where we have 2010

                                        • Re: Very Large Structural Simulation
                                          adam nikel

                                          I apprecaite the help from both of u, me and my teacher are gonna contact CAD dimesions sunday and have them take look at the model and see what they say. ill post what they said up here so you guys can see what they recommended.

                                          • Re: Very Large Structural Simulation
                                            Michael Feeney

                                            Because I was bored, lol. Here is ABAQUS for you.

                                             

                                            Assembly.png

                                            AssemblyZoom.png

                                            Load.png

                                             

                                            Displacement.png

                                            Mises.png

                                             

                                             

                                            The model was made very similar to your model. I can't say the dimension are 100% in agreement, but they are close...and this is mainly to show you how easy ABA is. Symmetry was used. The loading is done through point loads across the top arch (not a pressure load).

                                            • Re: Very Large Structural Simulation
                                              Derek Bishop

                                              Haven't read all the posts and am not sure if you got this working in the end Adam. Here is a model of the structure in 2010 SP4. Could be done in less than 15 minutes with the stress analysis. Defineing geometry takes a bit of time with something like this and my model is done without much care for geometry.

                                               

                                              This is a small structure for SW and could be solved in seconds using beam analysis. 2010 handles curved beams. I had to redefine neutral axes on curved members to get it to run.

                                               

                                              Haven't used Abacus but have used SW Simulation a bit. I suspect both have their strong and weak points.

                                               

                                              Part 1-1.JPG

                                               

                                              Part 1.JPG

                                              Part 1-2.JPG

                                              • Re: Very Large Structural Simulation
                                                Satit Nilyai

                                                Dear all

                                                I simulationed the structure by using sw2010. I also solved the stress&displacement on this structure. Please look attached file.

                                                Note : When I saw the picture of stress&displacement. I think,I am wrong because when I checked I found restraint was at the middel of structure. "chang fix to symmetry" (Mr. Derek Bishop)