Pressure vessel analysis

[Anonymous]

I am somewhat new to Nastran In-CAD (using 2018 version). I'm trying to be proficient in using it to analyze custom pressure vessels and calculate maximum allowable working pressures. For the most part, I can do this using solid body analysis (although the mesh convergence confuses me). Recently, I found out that using shell analysis is a more accurate way to do this. Rather than come here to ask the many questions I have, I would really appreciate input on books and training courses which focus on this type of analysis, and to help guide me when shell or solid body is more appropriate, how to account for gaps in a shell, whether FEA can be performed on both shell and solid body components simultaneously, suggestions for constraints (especially when shell removes the supports), how to use the solver contacts correctly, guidance on mesh, the use of connectors to simulate bolted flanges in a shell model, etc. Really appreciate any and all suggestions here. Thank you.

[John_Holtz]

Hi @Anonymous 

I am sure that books, videos, or websites exist that specialize in pressure vessel analysis, but I am not familiar with any. Hopefully some other readers will be able to provide some specific recommendations. Lacking that, I suggest that you Google something like "FEA pressure vessel". 

The book "Building Better Products with Finite Element Analysis" by Vince Adams and Abraham Askenazi is a good book that covers the practical aspect of analysis. It is not written for any particular software, so although they show lots of examples/figures, there are no exercises in the book. "Up and Running with Autodesk Nastran In-CAD 2019" by Wasim Younis (and the "with Autodesk Inventor Nastran 2020") are specific to our software and include many exercises.

For your In-CAD specific questions, I think this forum would be the place to post those. For example:

1. How to account for gaps in a shell? I assume that you are creating solid models and using the "midsurface" command to create the surfaces and shells. If the shells are welded, used "offset bonded" type of contact. If you have two faces that are in surface contact (such as two flanges bolted together), use separation contact and a "Penetration Surface Offset" equal to 0.5*(sum of shell thicknesses). To avoid the gaps, the best solution is to create a surface model that has no gaps between the parts.
2. Can FEA be performed on both shell and solid body components simultaneously? Yes. You assign the parts to solid Idealizations and surfaces to shell idealizations. The contacts you define are basically the same as when working with 100% solid or 100% shell - bonded and/or separation.
3. Suggestions for constraints (especially when shell removes the supports)? Why are the constrained parts being removed? (I am guessing that you have something like legs, brackets, or saddles on the vessel that are somehow missing when you "shell" the model.) If the supports are structurally important, then they need to be modeled as shells or solids and the constraints applied at the mounting location. If the supports are not structurally important, then you might be able to use a rigid body connector to simulate the support, and apply a constraint to the end point of the connector. The third option is to apply the constraints directly to the parts that are remaining in the model.
4. How to use the solver contacts correctly? Use "solver contact" to create contact that involves the majority of the contact. For example, use a bonded solver contact instead of creating (and managing) 100 contact pairs between all of the parts. Define the manual contacts for areas that use a different type of contact (such as separation).
5. Guidance on mesh? Start with a coarse mesh so that the analysis is faster. (If you are like me, it always takes a couple of tries to get the setup properly. 🤔) After the analysis is running as intended, use a finer mesh and/or "Mesh Controls" to make smaller elements in the areas of high stresses. Ignoring the stress singularities (where the stress goes from "max" to some fraction of the max value over 1 or 2 elements), refine the mesh in areas of high stress until the mesh no longer changes. In other words, the stress results are more accurate with finer meshes. You may not have the real stress value until you make the mesh small enough to capture the real stress.
6. The use of connectors to simulate bolted flanges in a shell model? That may be doable. I assume you are using separation contact between the flanges, so you need to use the "Penetration Surface Offset" to account for the gap between the shells. The only question in my mind is whether the bolt preload can be calculated in this situation. (Because the bolted members have some stiffness, the analysis requires a higher load in the bolts to squeeze the members and generate a force in the bolts equal to the preload. The analysis actually does a "pre-analysis" with all parts bonded to calculate the required force to generate the specified preload. Will this approach work with shells and a penetration surface offset? You should do a simple test.)

What other questions do you have?