26 Replies Latest reply on Aug 11, 2010 3:40 PM by Bill McEachern

    Mixed meshes -- beams and shells

    Jim Andrews

      As I stated on another recent thread, I've been performing FEA with COSMOS/M for almost 20 years, and ABAQUS for a half decade prior to that.  I'm comfortable with COSMOS.  SolidWorks & Simulation?  Not so much.

       

      So now that I've gotten just a little bit proficient at designing a weldment and analyzing it with beam elements, I need to take the next step.  I need to include shells.  Imagine a 3D weldment with thin gussets and skins -- what's the most appropriate way to model this in SolidWorks, and then how do I generate a mixed mesh of beam and shell elements to analyze it?  I want to use shells, not actual 3D (tet) elements for the thin plates.  It "feels" like the shells should be meshed from surfaces, in a planar analog to the lines one creates in a sketch that get meshed as beams.  Am I on the right track?

       

      Any hints would be greatly appreciated, and a link to one or more tutorials would be fine.  I haven't found any that address this specific task.

       

      Regards,

       

      jim

        • Re: Mixed meshes -- beams and shells
          Bill McEachern

          General rules of the road are more or less - beams line up with structural members (or extrusions), shells with surfaces and solid elements with solid geometry. You can use surfaces off solid elements and then the solid is then not meshed as a solid. The safe bet is just put in surfaces where you want to have shell elements and get rid (suppress) all other extraneous geometry.

           

          If you make the edge of the shell coincident with the beam surface you want to attach it to it will (in most cases) automatically bond the two together if you mesh with bonded as the default condition. Otherwise you use a contact definition (under the connections folder in 2010) and make it bonded (must be an edge to surface connection in this mode). If you want all the nodes to line up not sure if that can be done on a beam to shell edge bond but the way to achieve it in other situations like shell edge to another shell face is to ensure they share a common edge of the same length (you can use the split line tool for this - pretty easy effort wise in 2010). In 2010 they use I believe what is commonly known as mortar bonding which is good enough for most things when the nodes don't line up. To do this with a beam you would probably have to split the member at the extents of the shell edge to give it a whirl.

           

          On the confidence side - things are getting very much better. I just read the "What's New" doc for 2011 and it is further evidence that things are heading in the right direction. 2010 was better than 2009. In my opinion things sort of went off the rails when the CAD guys at Solidworks decided to run the FEA shop like a CAD shop. That seems to be getting corrected as near as I can tell.

            • Re: Mixed meshes -- beams and shells
              Jim Andrews

              Thanks . . . I guess the next step for me is to figure out the way to create surfaces and mesh them.  Onward through the fog!

               

              jim

                • Re: Mixed meshes -- beams and shells
                  Bill McEachern

                  On the auto bonding of beam and shells. The face of shell to a beam works most of the time (ex being a stiffened shell). The edge of shell to a beam is not supported. You will have to make a manual connection bonding the beam to the face of the shell (as the target). The span of the joint will be handled reasonably well by the mortar bonding. Same would apply to a beam and a solid.

                    • Re: Mixed meshes -- beams and shells
                      Jim Andrews

                      Thanks, Bill.  I think -- I know -- my questions are even more rudimentary than that.  Say I have a simple rectangular frame (see attached image) I generated from a sketched rectangle.  How do I go about "filling" that frame with a plate?  Do I have to extrude the sketch and pick off one of the surfaces to mesh?  That seems clumsy, although it's probably somewhat consisent with the CAD approach taken by SolidWorks & Simulation.  In COSMOS/M, I would just generate a 4-sided surface using 4 straight curves, mesh the curves with beams, mesh the surface with shells, and merge the nodes.  I'm stumped in Simulation.

                        • Re: Mixed meshes -- beams and shells
                          Bill McEachern

                          I hear you but don't dismay, you are close. Now hopefully you have a plane where you want the plate to go, if not make a plane at the appropriate spot - the plane where the shell element will lie - we are going to create a planer surface hence the need for a plane. Once you have the plane make a sketch, then pick the edges of hte structural members to get the rectangle that will define the surface and then select the planer surface command and check OK. You should have a planer surface now where you want the shell elements to go. the rest is done in a simulation study.

                           

                          Make a new simulation study and you should have in the bodies folder, four beams and a surface. RMB on the surface and define its thickness and shell formulation and under the edit definition tab. Apply a material as well if required (it may already be defined if the part has a material set in solidworks - you can change it then if need be in simulation). Under connection you want to defined a contact set, select bonded, then pick the beam selector, and pick a beam in the upper selection box and pick a the surface in the lower one, push in the push pin at the top and then check OK, repeat for the other 3 sides. (the push pin keeps the dialog open with the same settings and then you can just pick the new geometry entities and hit OK).

                          Then calculate the beam joint - basically for this model it amounts to opening the dialog hitting calculate and closing it.

                          Then apply BC's and hit mesh and run.

                          On a simple model like this Goestar might seem easier but in something complicated this approach is much, much faster in terms of effort. Just to give you some hope I did a sluice gate for a hydro electric installation from imported Inventor solid geometry in ~3 hours - it was a bit rough in spots but more or less a decent approximation of the structures response. In essence the drudgery is far reduced in this approach. Hang in there.

                            • Re: Mixed meshes -- beams and shells
                              Jim Andrews

                              Wow, what a reply!  Thanks so much, Bill.  I am off for the rest of the week, but I have SW at home, and I'll give it a spin.  Thanks again.

                              • Re: Mixed meshes -- beams and shells
                                Jim Andrews

                                Well, I made some progress, but any hints as to where I went south would be appreciated.  I created a 2' x 8' rectangular frame of 4" x 4" x 0.25" box beam, reinforced it with a 1/2" steel plate, got it to mesh and . . . study failed.  Ugh. Must be the contact sets.  Can I get a little feedback on these two screen caps (please excuse the ridiculous mesh density)?  Maybe someone else can see the problem.  (FYI, if I exclude the plate from the analysis, it runs just fine.)

                                  • Re: Mixed meshes -- beams and shells
                                    Bill McEachern

                                    Sorry Jim, been busy.

                                     

                                    That looks like it should have worked. I would try the contacts one at a time. That is to say bond one of the members to the face of the shell and see if it solves. If it does keep going and see the one at a time approach works - four contact sets in the tree. If no then send it into support. What version of software are you running?

                                     

                                    update: I just built and ran an identical model -exactly as you described - worked no problem. I am running swx2010 sp4.0. If you are running sp0 it may have an issue on this.

                                      • Re: Mixed meshes -- beams and shells
                                        Jim Andrews

                                        Thanks, Bill.  It's weird -- I've gotten it to run by fussing with the mesh density.  The thing is, even at its coarsest setting, the mesh density is more than adequate, based on experience.

                                         

                                        For what it's worth, I'm running SolidWorks Pro 2010 x64 SP 2.1.  My FEA package is Simulation Premium.  Surely this can't be the issue.

                                          • Re: Mixed meshes -- beams and shells
                                            Bill McEachern

                                            Well, I am currently working on some beam solid bonding and it has some issues in SP4.0 -that didn't occur in earlier releases........I will let you know when I get it figured out.

                                             

                                            Well, if you select one face and one beam per contact set it seems to work reliably (well, lets say it worked for the cases I tried - pretty coarse mesh)  in the model I am currently working on.

                              • Re: Mixed meshes -- beams and shells
                                Michael Feeney

                                "Otherwise you use a contact definition (under the connections folder in 2010) and make it bonded (must be an edge to surface connection in this mode)."

                                 

                                Should have read this from the get-go....did it and it worked and produced the exact same results as using solid body meshing.

                              • Re: Mixed meshes -- beams and shells
                                Michael Feeney

                                Hello all,

                                 

                                I am currently a graduate student getting my masters degree. This summer I am working at Caltech on a submm telescope project. Among many things, the project has required some FEA frequency analysis. I've been doing research regarding SolidWorks meshing and simulation..and I came across this thread. It sounds like there are a lot of knowledgeable people in this discussion and it seems quite helpful. I'd like to give my two cents on the issues above:

                                 

                                Normally when I do FEA I use ABAQUS [a god-like, efficient, elite FEA package]. For this particular project I am studying a "quadrupod" (tripod with 4 legs) structure. Imagine 4 legs setup similar to a tripod (joined at the top) with a mass at the joining point. The legs of the quadrupod are thin walled pipes. In Abaqus, I ran this structure using wire elements and set up a pipe profile to define it. I created a rigid body with an associated mass for the top joint. Refer to Figure 1. I studied the frequency response of the first mode for a variety of masses. Theoretically the frequency should change as 1/sqrt(mass). This was not the case. The frequency decreases at a much slower rate. Due to the fact that the results were not matching the hand calculation, I did what any logical person would do ...check out another package and see if it agrees.

                                Figure 1.jpg

                                SolidWorks was my next choice. My professors would shun me if they found out I was using the so called "FEA" part of SolidWorks. Don't get me wrong...SW is great for drawing/designing/blahblahblah and has provided me with employment for many years....however as far as I am concerned it is not an FEA tool. I would really like to be proven wrong and become a supporter of SW Simulation, but that path seems unclear to me. Here's what I did in SolidWorks: I created the quadrupod structure as seen in Figure 2. Legs are 51 kg each (carbon fiber). The top plate is also carbon fiber (10kg). Once the mates in the assembly were made and everything was constrained...I opened up the simulation and began setting things up. I did rigid connections for each leg to the plate. I applied fixed boundary condition to the bottoms of each leg. And finally I applied a distributed mass to the top of the plate where the legs meet at the top. I tried meshing with default settings and failed. I refined...and refined and refined.....oh yeah....and refined. finally changing the settings to  Ultra FINE curvature based mesh. I understand that the mesh is very fine as to have enough elements running through the thin wall of the legs. I then ran the simulation and took a nap. 15 minutes later (this is a long time compared to Abaqus which takes 30 seconds) I got the results. They agreed with Abaqus.

                                Figure 2.jpg

                                Now my question. I want to do this with shell elements. I know how to apply midsurface to the legs and create a shell thickness and I can do this for the top plate too. The issue that I have is that I cannot seem to figure out the connection between the legs and the plate. I'm happy doing a solid (plate) to a shell (leg) mesh. I could do shell to shell also....I just need to know how to connect the parts. When dealing with surfaces...you cannot do rigid connection. Even in the assembly configuration I cannot apply any mates to make these surfaces touch. I have tried to select the edge of the cylindrical leg and try to mate it with the top plate...but it just wont work. When I run a simulation without connections, the top plate flies off. I really want to use shell elements so I don't have to do this sim so inefficiently.

                                 

                                How do you connect two shells ...or a solid to a shell to run an FEA analysis? If you say that it's default connected if they are touching then how do you set it up to touch in the assembly module?

                                 

                                Thanks if you read all of this...sorry for the long post.

                                  • Re: Mixed meshes -- beams and shells
                                    Poovaiah Devenira

                                    Hi,

                                     

                                    A solid element would give you more accurate result than shell element. I believe you want to use a shell element as to find an optimum thickness for your structure. If I am not wrong analysis programs are set up to run in shell elements so that the thickness can be controlled (some programs can give the required thickness for a particular force). However my advice is when running SolidWorks, since it’s more like a design validation tool, to use solid elements.

                                      • Re: Mixed meshes -- beams and shells
                                        Michael Feeney

                                        Aside from just saying it...what is your validation for your statement "solid elements give a more accurate result." This is...in many cases not true. Furthermore, I'm looking for advice on shell to shell or shell to solid meshing.

                                         

                                        I've read in many areas of the internet that it is best to use shell elements for thin-walled members such as the legs I have here.

                                          • Re: Mixed meshes -- beams and shells
                                            Poovaiah Devenira

                                            Shell elements are 2D elements capable of resisting membrane and bending loads.

                                            Solid Elements are parabolic tetrahedral elements; parabolic elements yield better results than linear elements because: 1) they represent curved boundaries more accurately, and 2) they produce better mathematical approximations

                                              • Re: Mixed meshes -- beams and shells
                                                Jim Andrews

                                                In many cases, the DOF limitations within a given FEA package preclude the accurate modeling of a large thin shell with solid elements.  I don't think it's correct to say solid elements are "better" -- they're better when they're better, and they aren't when they're not.  It's our job to know which is which.

                                                • Re: Mixed meshes -- beams and shells
                                                  Bill McEachern

                                                  This is misleading. You can produce junk with solid elements just as easily, maybe even more easily than you can with shell elements. Further, in Swx Simulation (Cosmos was way easier to write) you have a choice of linear or parabolic shell elements and you have a thick, thin or laminated composite formulations. The choice of element type is strictly a function of practicality as Mr. Feeney eludes. For high aspect ratio problems shells or beams (or more generally, structural elements) are the way to go and for low aspect ratio problems solids elements (or again more generally, continuum elements) are the way to go. To say one is better than another is crazy talk and shows a fundamental lack of understanding of the method and practical computer simulation. It is up to to the analyst to decide what APPROXIMATION (it is in all caps to emphasize the fact that it is all an approximation no matter what the pretty pictures may convey to bias you to some other realization) is appropriate for a given situation. There are many not that experienced individuals who read theses posts so, I would suggest, that unless you are absolutely sure, it might not be best to make explicit statements about certain things when the real story is far more complex that a simple statement conveys like "solid elements are better than shells". Nothing could be further from the truth.

                                                   

                                                  Mr. Feeney, as a former ABAQUS user myself, there is nothing better or worse about ABAQUS or SWX Sim for the class of problems that SWX Sim can actually solve, which admittedly, is a subset of what ABAQUS can actually solve. There are problems that ABAQUS can not solve that other codes can solve. Every code has their strengths and weaknesses and you figure it out through experience. I have to admit that after attempting a some what complex NL problem in ANSYS way back whenever, I was pretty stunned when ABAQUS pulled it off with out breaking a sweat (SWX sim is still unable to solve the problem). Not sure if ANSYS can do it now or not, probably (it was a shear dominated post buckling problem). I too thought at the time that ABAQUS was pretty awesome. Over time you realize that it is not the optimal tool for every job.

                                                   

                                                  I would advise that your problem, for efficiency seems far more suited to beams than shells for the legs. Bonding it all together, well,  SWX Sim is, I would characterize, as a geometry centric preprocessor and most other codes run a nodal centric preprocessor. So in SWX sim your solutions are mostly found through geometry as opposed to merging nodes that you spend a great deal of time to organize to land it right sport so that when they merge not much else happens. The very big advantage that SWX Sim has is that it removes the burden of drudgery from the analyst to a great degree (yeah, I know it sometime doesn't work the way it is suppose to but that is a separate issue as much as I would like to see it go away as much as the next guy). When it works as advertised and you know what you are doing (you have figured it out) the effort hours to solution with SWX Sim is second to none for the classes of problems it solves. And yeah I know, that isn't always the the easiest thing to figure out and the attitude at SWX certianly doesn't help much in this regard with respect to FEA and simulation in general.

                                                • Re: Mixed meshes -- beams and shells
                                                  Michael Feeney

                                                  I ran the model with all solid elements...and then I ran it with shell elements on the legs and solid elements on the plate. Both yielded the same result. Mr. Devenira what are your thoughts?

                                              • Re: Mixed meshes -- beams and shells
                                                Jim Andrews

                                                Abaqus.  Yep, familiar with it.  Wrote my masters thesis in 1987 on stress analysis of the field coil assembly of an ultra-high power generator using . . . Abaqus.  Had to run the models (literally) on a Cray.

                                                 

                                                I'm not sure why you think Simulation isn't a legit FEA tool.  COSMOS/M most certainly is (was), and that's what Simulation is based on.  My problem with Simulation is mostly getting it to let me do my thing instead of what it thinks I want it to do.  A knowledgable engineer could wrangle COSMOS/M into answering most problems, because the user had direct top-level control of most parameters.  Those parameters seem to be buried somewhere in the basement of Simulation, but so far, I'm finding what I need, if I dig around enough.

                                                  • Re: Mixed meshes -- beams and shells
                                                    Michael Feeney

                                                    Key there..."dig around enough." Haha..I completely agree. I wrote that bit earlier today when I was frustrated. I have spent the last couple days wrestling between 15 minute simulations and trying to connect shell elements. Fortunately now (after reading all of these posts closely) I've learned exactly how to get 1 minute simulations with shell elements. Poovaiah argues that shell elements are not the correct choice here...but I ran both solid and shell and they're yielding identical results. Had this been a stress report I would tend to agree with him...but this is natural frequency (independent of displacement and stress).