I am evaluating Femap / Nastran for a specific class of problems I need to deal with frequently. We have a real need for affordable, relatively easy-to-use FEA software for analysing stiffened steel plate structures, based on imported 3D CAD geometry.
We already have access to FEA software that can generate solid tet meshes from imported solid CAD models, but these meshes are not useful for the very slender geometry we are dealing with (e.g. we might be looking at a steel chute which is 3 m x 2 m x 4 m high, composed of 12 mm thick steel plate, with stiffeners that might be 100 wide x 8 mm thick at spacings of 600 mm, say). To model these sorts of structures with linear-tet meshes capable of capturing the plate bending behaviour typically requires ridiculously fine meshes (characteristic element size of 3 or 4 mm say, to get a few elements through the plate thickness). It is prohibitively time-consuming to generate such fine tet meshes and to solve them for the sorts of problems I deal with.
What we really need is an efficient means of meshing such structures into quad or triangle plate / shell meshes with a typical characteristic element size of 25 mm – 100 mm say.
Our problem is that the source geometry is true solid geometry, so every piece of steel plate is represented by two large surfaces (the +z and –z faces), plus three, four or more “sliver” surfaces around the perimeter. In addition, because the models are generated in steel detailing software, the plates and stiffeners are each modelled as separate solid entities, and the components are actually separated from each other by small gaps of 1 mm – 2 mm say (which are needed as assembly / welding clearances). The fabrications are modelled as “Assemblies”, but we need to analyse them as single “Parts”. With our current CAD and FEA software, It is a very time-consuming and error-prone process to simplify this 3D solid geometry into single-surface representations which are joined compatibly at all plate intersections, suitable for plate / shell meshing.
I have downloaded the trial of Femap, and worked through Examples 8, 13 & 14 to understand how to import CAD solid geometry, and generate a mid-plane surface model form the original solid model. This works fine, and I end up with a nice mid-surface representation of the whole model very easily, but it typically consists of numerous separate mid-plane surfaces (one for each piece of steel), separated by a few mm at each wedded joint.
However, I haven't worked out how to "stitch" the various mid-plane surfaces together to create a single unified mid-surface model which will mesh compatibly at all the joints. This problem didn't arise when I was doing the Example problems, because in each case, the tutorial was working with a single imported solid part, whereas I am effectively importing an entire assembly of parts.
I suspect I am looking for tools called something like "Merge Surfaces", "Graft Surfaces", or similar, but I haven't found a tutorial on how this would be done for problems of the type I am dealing with. Or maybe I should leave my "assembly" as an "assembly" of separate "parts", and apply rigid surface connections between the parts where they join each other?
Can anyone point me in the right direction? I am a complete newbie with this version of Femap / Nastran, but I have quite extensive FEA experience generally, so don't feel you need to "dumb down' your responses - I am just seeking a "fast track" to the best tools available in Femap to tackle this class of problem. If there is a Tutorial / Example of this process that I have missed, that would probably be the best help of all.
Hello!, I understand your needs perfectly, you have basically the following options: 1.- METHOD#1: EXTEND MID-SURFACES TILL INTERSECTION. This is the classical meshing approach, you will have to use command "Geometry > MidSurface > Extend" and select METHOD=DISTANCE and enter the distance value. Using this command repeatedly you will extend surfaces till their intersection easily.
The next step will be to use command "Geometry > Surface > NonManifold Add..", this will assure that all surfaces are connected properly, assuring compatibility of displacements after meshing surfaces with Shell elements.
The hard work here is to extend surfaces till intersection.
2.- METHOD#2: NO GAPS BETWEEN SOLIDS In cases where 3-d solid plates are already touching (no gap exist between them), then the most efficient method is to joint all solids in only one using command "GEOMETRY > SOLID > ADD" and then to use command "GEOMETRY > MIDSURFACE > AUTOMATIC", ¡n this case FEMAP will perform automatically the job of creation of midsurfaces + extend surfaces till intersection. After that phase simply issue command "GEOMETRY > SURFACE > NONMANIFOLD ADD" and you have the model ready for prescribing mesh size in surfaces + meshing.
3.- METHOD#3: EDGE TO SURFACE GLUING. This is impressing method coming from NX NASTRAN solver, the capability to define rigid "T" joints without the need to extend midsurfaces till intersections, then you can run out of problems due to the manufacturing gap of 1 or 2 mm you have between plates. Simply perform midsurfacing of every plate, and then you will have to learn how to define regions & connections using EDGE-TO-SURFACE GLUE joint. Please note you can mesh plates freely, you not need to be worried about intersections, matching meshes, not need at all. The method is faster, not adding extra DOF or extra computational time. And is more efficient & accurate that extending midsurfaces till intersection, so no excuses to use it!!.
Thank you, Blas! That is exactly the information I was looking for.
Method 1 works fine, and is very easy.
Method 3 looks like it is an even better analytical approach for my case, because it leaves the original geometry basically intact, which may make it easier to report back any design changes I am recommending to the CAD designer - I just have to find the "Edge to Surface Glue" tools, and learn how to apply them.
Hello!, In order to be more efficient & extremely productive using method#3 whit assemblies with many components, please use LAYERS. The idea is to be able to fast hide or show geometry and mesh simply switching between SHOW ALL LAYERS or VIEW VISIBLE LAYERS ONLY using the RMB over LAYERS in the MODEL INFO, if not you will became crazy!!. I use LAYERS a lot, this will allow me to hide or show solid geometry, or surfaces, give layers a name in order to manage better your model. Enjoy testing FEMAP!.
Thanks for the additional comments re: "Method 3". I have also been contacted by Femap support (thank you Andy!), and he has demonstrated your "Method 1" on some of my sample geometry, and it worked very well. It gives me the confidence to look at getting Femap for my organisation (and some training!) so that we can use it on our projects.