Random mesh generation failure with pattern shells/solids

[djparsonsK7ZYY]

I have been working on a file for quite some time now, bouncing back and forth between attempting to simulate using solids and shells. I am specifically having an issue with mesh generation on solids or shells where, the mesh will generate properly without loadings (but with contacts and constraints), but once the loads are applied the mesh will randomly decide to fail to generate anywhere from 1/3 to 2/3 of the faces on shells that originally came from pattern solids. I have not had this issue when manually sketching several copies and then generating new solids, but on discontinuous single solids that are "one body". Additionally, when this meshing fails, in-cad then proceeds to remove related contacts, constraints, or loads entirely. Upon reloading the file (which includes a global rebuild inherently), in-cad will throw up part modification related errors that then correlate to the contacts and co that are removed silently. Manually restoring these relations is met with the exact same mesh failure that happened prior, with those relations removed again.
I say random, because every time I delete an analysis and start over, remake the idealizations, reapply the relations and loads, I receive a different set of the pattern solids to have succeeded/failed.

For example, this latest instance has resulted in 3/15 legs in not meshing. Most of the time its a combination of brackets and legs that fail. I have attached the file, please help in any way possible.

[John_Holtz]

Hi @djparsonsK7ZYY

Sorry to hear about the problems. There may be something going on related to a single part model with multiple bodies, combined with creating additional surfaces when using the Midsurface command, but this is just a guess.

Which version of In-CAD are you using? (Because there are so many versions, you need to give us the full version number from the "Nastran Support > About" command, such as version 2018.2.1.428.)

[djparsonsK7ZYY]

Thanks for the quick response. 
I'm using Autodesk Nastran In-CAD Version 2019.0.0.103
I have managed to get a full mesh to generate using the legs as shell and the rest as solid using continuous meshing, so it may have something to do with the contacts as well. Before, I was using normal bonded contacts on the midsurface shells without any penetration offset, which could be a problem except for the fact that it would work on most of them. Only issue with the mixed instance is that I get roughly 6000 skew angle notifications (none of which show up in mesh quality check) and then I imagine inventor runs out of memory and promptly crashes. Haven't attempted sketching/extruding/revolving the 60 brackets and 15 legs for obvious reasons.

[John_Holtz · Accepted solution]

Hi @djparsonsK7ZYY

Before I forget, you can edit the Parameter ElemGeomChecks and change the value from On to Off. This will avoid the crash that can occur during the analysis when there are so many G301x warnings. (The "Parameters" is the second to last branch in the model tree. Right-click on it and choose "Edit". Then search for ElemGeomChecks.)

About the midsurface model. I am not sure what is occurring here since the loads/constraints/contacts are no longer in the model. When I applied some (just "random" values since I am not totally familiar with the setup), my items did not disappear when I re-opened the model. The only suggestion that I have is that all of these items (loads/constraints/contact) need to be defined on the midsurface model, not on the solid model. So create the midsurfaces first, then add the loads, constraints, etc. It looks like you created the solid model first, then tried the midsurface model. So I can imagine that the loads/constraints/contacts were based on the original surface model. All of those items become "disconnected" when the midsurfaces are added to the model and replace all of the surfaces of the solid.

About the solid mesh. I can see that the legs do not mesh as solid. There is some problem at the top of the leg such that the surfaces are not matching up properly. See the image below. My guess is this is a problem with precision or something (the legs are very thin for the diameter), but I will submit your model to the developers so that they can have the meshing people look at it.

Figure 1. Looking at the mesh on the top of one leg. The face highlighted in blue is the face that contacts the equatorial ring. The white edges that are visible between the 11 o'clock and 1 o'clock positions are where the flat face on top does not match up with the outside surface. This mismatch prevents the leg from being meshed as a solid.

Shell versus solid. This is the type of model that benefits from using shell elements: very large overall dimensions, comparatively thin material . The pros and cons then become:

• Do you use the midsurface command to create the shell surfaces from the solid? Or create a surface model from scratch in Inventor? The midsurface approach is certainly possible, but personally I do not like the transparent surfaces that the midsurface command creates. Also, using offset bonded contact to weld the pieces together is not as good as a matched mesh. Creating a surface model in Inventor provides more control over both of these issues.
• Create a multi-body, single part surface model? or a multi-surface-part assembly? A single part model has the benefit that the mesh will match between pieces without needing to use contact or the "Continuous Meshing" option. (The faces do need to be split where they are supposed to match.) A multi-part model gives you the ability to hide parts more easily in In-CAD but requires the use of offset bonded contact. (Do not use "Continuous Meshing" on a shell model until the fix is released. In current software, constraints and loads applied to an edge can be "secretly" applied to other edges of the model. It is difficult to detect such errors.)

I would be interested in reading how other users handle shell models: create a surface model in Inventor? Use the offset/midsurface command in In-CAD? What are other problems or benefits?

[djparsonsK7ZYY]

Thank you for the amazing response @John_Holtz .
I finally found a control vs settings arrangement that allowed for the leg mesh to still self refine near the border, preventing meshing errors; previously on the solid simulations I was forgetting the two "edge" like surfaces contacting the sphere, and treating them to the same refinement as the legs themselves. I can currently get a working solid mesh, but not without it reaching ~2 million nodes. If I were to persue the solid mesh I would definitely end up subdividing some faces for better control. 

Apologies about the model I uploaded in regards to the nastran analysis that was active; it was a save that (hopefully) had the warnings show on load up like I spoke of in the first post. About midsurfaces in general, I was applying the loads and contacts etc to the midsurface idealizations. The missing ones in the general model category there were most likely copies that were used in analysis 1. The ones that popped up on load in were from the mesh failing on analysis 2.

Given what you've said, I believe my best course of action is to re-sketch the model as pure, stitched surfaces. This should avoid the high node/element counts while still being an accurate model. Thank you for the tip on the G301X warnings.