19 Replies Latest reply on Jan 16, 2019 2:03 PM by Ryan Navarro

    Too Many Elements?

    William Finch

      I need to run a Static analysis for large structures made out of a lot of these:

       

      The members are cut out of 3x3-inch aluminum angle. The structure is a rectangular box about 72-inch sides, with lots of bracing and supports all over the place.

       

      The small features are important, but the structure is big. If I try to mesh with big elements, the mesh fails. If I apply a Mesh Control and make the elements about the size of those little (1/4-inch) angled members, the element count goes way up (obviously) and either the mesh or study fails (or takes a day).

       

      Is there a way I can run a static analysis just on the above part to get the stiffness matrix (per linear inch)? Then use beam elements, with the newly-found properties, to analyze the entire, larger structure? The solid patches on the ends are for connection and could probably be ignored.

       

      Thanks!

      Yitz

        • Re: Too Many Elements?
          Dan Golthing

          Not sure why you're having a problem.  Even using a solid mesh, this should mesh OK and run fairly quickly. 

           

          do you want to post the part and let us take a swing?

            • Re: Too Many Elements?
              William Finch

              Hello Dan - Thanks!  I posted a zip file with the assembly down at the bottom of the thread.  I set up the fixed geometry and loads, so I think those files are in there as well (I hope!).  As I said, I'm interested in the deflection of the aperture and the sensor as the telescope rotates from horizontal to vertical (aperture-down).  I appreciate any help or advice you can give.

            • Re: Too Many Elements?
              Taylor Duran

              Yitz,

               

              It doesn't look like you modeled the angle using a weldment feature.

               

              Do this, and then make the extrude cut in the member and save as a part.

              Build your structure as an assembly with those cut weldment parts and treat them as beams in your assembly simulation. It will still account for the cuts in the angle with variable moment of inertia, but the simulation will render the beam as a simple cylinder so any stress concentrations you may be concerned with in the angle will be ignored at that level. But like Dan said, if you're only concerned with the individual part you should be able to use a solid mesh without much trouble.

               

              Have you checked to see if Graham Mustoe could help you out?  Go Orediggers!

               

              -Taylor

              • Re: Too Many Elements?
                Ryan Dark

                Hi William,

                Yes, you can use Simulation to create a sort of meta-material definition that represents modified beam here.  What you would do is create a representative model like you have done here but you would extend the cuts from end to end.  You still want a slight amount of material on both ends that makes each end profile still have the uncut beam profile.  From there you will use a solid element mesh, apply a dummy load to one end, and a fixture to the other to bend the model as a cantilever beam.  Run the study.  The result you are looking to extract from the study is the maximum deflection/displacement for use in this cantilever beam equation:

                 

                ...sourced from here (Cantilever Beams - Moments and Deflections).  You will have known values for these variables:

                 

                F = applied force on end of beam (N)

                δ_b = maximum deflection due to bending (m, mm, in)

                I = moment of Inertia (m^4, mm^4, in^4)

                L = length of beam (m, mm, in)

                 

                ...and be able to back calculate the new meta value for E in bending (or E_bending) for that direction of bending.  You may want to assume the other bending direction is the same but you will definitely want to also run an axial pull test in this same manner and use this equation:

                 

                ...sourced from here (Axial Deformation | Strength of Materials Review) to run determine the E_axial with these known values:

                 

                F = applied force on end of beam (N)

                δ = maximum deflection due to tension (m, mm, in)

                A =  cross sectional area of beam (use uncut cross section) (m^2, mm^2, in^2)

                L = length of beam (m, mm, in)

                 

                ...and back calculate E_axial.

                 

                Having calculated E_bending and E_axial meta values you now make a custom orthotropic material using E_bending as E_x and E_y, then use E_axial as E_Z.

                 

                That was a lot of work already but now you have to apply this meta material definition to an uncut beam and test that the meta material values give you the same deflections under the same loading.  In my experience they are close but not exact, so what I typically do is make corrections to E_X, E_Y, and E_Z  by calculating the ratio between the deflection of the cut beam model and the non-cut beam model with the meta material applied.  I multiply that ratio against the meta E values I have already to force the meta E values to give the correct deflection to match the solid-element cut-beam model's deflection.

                 

                Once you are done you should have a meta material definition that lets you use a plain beam element mesh to analyze a much larger structure a bit quicker than if you used a solid element mesh throughout.

                 

                I hope this all makes sense.

                  • Re: Too Many Elements?
                    Taylor Duran

                    Ryan,

                     

                    What is the difference between your solution and just treating the cut angle parts as beams in the simulation in a linear elastic isotropic model? I'm just curious about the accuracy you gain by going this route and the difference of this method vs treating the cut angle as a beam in a linear elastic isotropic model? Is there something going unaccounted for in the simulation if you don't create a custom orthotropic material for beams with significant cutouts?

                     

                    If the cutout pattern in the angle changes, even slightly, you would have to go through the process of defining and verifying the new Ex, Ey, Ez values again so it sounds like a lot of work and it's not clear to me why its needed. Aluminum is an isotropic material, and using a linear elastic isotropic model  with beam elements you get different displacement values with material removed from the angle than you do as a solid angle so the missing material isn't ignored. So why all the trouble to create a new custom material?

                     

                     

                     

                    Thanks,

                     

                    -Taylor

                      • Re: Too Many Elements?
                        Ryan Dark

                        Taylor,

                        Beam elements would not recognize the cutouts.  Beam elements, in simplifying the model, recognize only a constant and tapered profile.  The cuts are complications that a beam element itself could not account for so in order to use beam elements it would need to be accounted for in the material definition as a meta-material.

                         

                        The reason for creating an orthotropic material is that I might expect that the two bending tests would yield different E values than the tension test on the beam.  In the spirit of putting in as much "good" data as possible I would want to express that in the definition of the meta-material in the form of an orthotropic material definition.  This is just a hunch though.  Doing the testing for E in all principle directions will confirm whether to use an orthotropic material or if you can leave it as an isotropic material.

                         

                        Yes, if the cutouts change the testing for E would have to start over and can be somewhat time consuming.  If you are willing to make the meta-material and are okay with it as a simplification of the analysis you could do an analysis of a larger structure based on these custom beams.  That larger analysis has the potential to go fantastically faster than if solid elements were used instead.  So, if you spend an hour calculating/refining the meta-material properties each time you do it but it saves you from having to run an analysis that takes 24 hours to complete, it is time saved in the end.

                    • Re: Too Many Elements?
                      Sergio Monti

                      Hi William, looking at your aluminium angle it seems that the torsion and shear on the single element could be negligible. Then just model a simplified angle bracket having thew same tension and compression behaviour and replace all the brackets with the simplified ones.

                      Hope it helps.

                      • Re: Too Many Elements?
                        William Finch

                        Hi!

                        Thanks for all the responses.  I'm still working on the problem.  Got side-tracked on other fires for a while, but I'm back to working on this (along with some Motion analysis, but that's another story....).

                         

                        Here's a screen-capture of the assembly I need to do a static analysis on.  It's a large-ish telescope and I need to estimate the deflections as it is rotated from horizontal to vertical.  For scale, it's about as big as the freezer in your garage.  That round hole in the front is a meter in diameter.

                        I have attached a zip file of the model, with all the unnecessary bits removed.  I think I save the fixture and loading conditions, so they should be there if you open the model.

                         

                        How do I tackle this?

                         

                        Thanks!

                        Yitz

                          • Re: Too Many Elements?
                            Ryan Navarro

                            Hi William,

                             

                            I had been meaning to respond to this but just wanted to say that that problem size should be feasible using Shell definitions for those various components.  This would keep the accuracy of the cutout geometry vs beam definition.

                             

                            I would manually Define Shell by Selected Faces on the various components. You will then have to go back in and manually apply some or all of the contacts. It will be a bit of setup work but there are some tricks to speed this process up drastically (using Shell Manager or using new "Import Study features" function)

                             

                            These videos from SOLIDWORKS may be helpful. SOLIDWORKS Simulation Step-Up Series: Shell Strategies Part 1 - YouTube

                             

                            shell.PNG

                             

                            To give you some kind of example to show the general process I created a new study and excluded most of your assembly except for the few front pieces and converted those to shells. You can continue on from here including more components, converting them to shells, and applying the appropriate contact/fixtures. Since this is a complex process I like to keep test loads/fixture set up (simple gravity + one fixture) and run the study periodically, until I have all components included and contacts functioning correctly. Then apply real load and fixture

                              • Re: Too Many Elements?
                                William Finch

                                Thanks Ryan!  I work on this problem when I can.  I did Pack-&-Go the model with an "FEA" suffix, so I wouldn't mess up my solid model.  I learned how to create mid-plane surfaces, and trim them up.  I can mesh individual parts, but having trouble meshing the assembly.  I will keep working on it.  Thanks again for your help!

                              • Re: Too Many Elements?
                                Shawn Mahaney

                                Check your mates.

                                I merged everything into one solid, with some difficulty, and edge lines remained on some surfaces that I expected to be smooth.

                                matex.png

                                 

                                The solid mesher had to work a little to mesh this, taking a couple minutes. It finished but had some extremely distorted elements.

                                meshx.png

                                  • Re: Too Many Elements?
                                    Shawn Mahaney

                                    I was already well into this, so I went back and fixed it:

                                    Re-mated everything to use consistent references and/or exact values. Joined everything in a single solid, with a few weld beads added to bridge line-line contacts. Guessed about how the rails are connected. Found a few other modeling errors, ignored. Meshed with a 3/8"-3/16" curvature based mesh. Ran in two minutes on a two year old machine.

                                    result0.png

                                • Re: Too Many Elements?
                                  William Finch

                                  Okay, this is driving me nuts:  When I try to mesh this model, the Mesh Progress starts, thinks a while, goes from 1% to 99% pretty quickly.  And then, hangs at 99%.  The Memory usage is fluctuating a little bit, definitely not increasing.  And, the Elapsed Time is ticking away. 

                                   

                                  Is there any way to tell if the mesh is progressing?...or if it has hit a wall and effectively stopped?

                                    • Re: Too Many Elements?
                                      Ryan Dark

                                      Speaking from memory only right now I believe you can check CPU usage in the Windows Task Manager and if you see it is non-zero for SLDWORKS.EXE then the mesh is still processing.  If CPU usage is at zero it may be bottle-necked somewhere else such as writing mesh data to where you have your files stored.

                                    • Re: Too Many Elements?
                                      Shawn Mahaney

                                      A few points:

                                      - These are not beams, by any stretch. An open-section L-angle is poorly represented by a beam.

                                      - The shell element method looks promising.

                                      - How are these pieces joined? I usually merge solids and put in welds literally. The solids won't merge here as there is lots of line-on-line contact.

                                      - There is no such thing as too many elements! (until the solver hits its compiled limits, over 800,000 second-order tets for the direct solvers) Having learned to avoid a few things that trip it up, the curvature-based mesher is proven to be scary fast. Newer computers have no trouble solving jumbo meshes (if they don't have awful elements) in coffee-break time.

                                       

                                      I made a new part, "joined" the assembly into it, and cut it down to work on just part of it. The join operation left all the bodies separate, as they meet on-edge. One sketch extruded three times made a literal weld shape and let the bodies overlap to be combined. The mesher gave a compact clean solid mesh in no time.

                                      extrude1.png

                                      mesh1.png

                                      • Re: Too Many Elements?
                                        Wayne Jamieson

                                        As Ryan said, try a shell model. I'd always use shells for a model like this. Model the assembly as a multi-body, sheet metal part, and the mesher will automatically collapse to the mid-planes and set the relevant thicknesses for you.

                                        • Re: Too Many Elements?
                                          William Finch

                                          Hi All,

                                          Many thanks to all who have responded!  I'm back on this problem after getting pulled off to fight other fires.  A few notes/replies from what I've read above:

                                          - the assembly will be bolted together.  However, I'm only interested in overall deflection, and not what's happening around the fasteners.  So, combining it into a single solid would be fine.

                                          - I spent some time deleting teeny surfaces that appeared from making surface models from mid-planes.  This seemed to help with meshing somewhat.

                                          Okay.  Here's where I'm at now:

                                          - Having problems with contacts between parts.

                                          - Assuming I want bonded contacts.  They behave as if a single piece.  Right?

                                          - If you have two solid parts, and make shells from mid-planes, there are a lot of gaps.  This is true for edge to edge joints, or edge to face.  I thought SW could make contacts across these gaps automatically.  I have checked the Shell Manager to confirm thicknesses and materials have been defined.

                                          -  I started with a single part - the front plate with a large hole.  That meshed and ran fine.

                                          - Then I added one more part - the little beam across the diameter for the hole.  Now it meshes, but doesn't run.  I think I'm not  doing the contacts right.

                                          • Re: Too Many Elements?
                                            William Finch

                                            YAHOO!  I finally got it to run!

                                            Telescope V1 Top AssyFEA.JPG

                                            I hope to post all the things I did to get this analysis to work.  However, now I am just basking in our collective awesomeness.  Thanks for ALL your help!