Seemingly inaccurate hydrostatic load and general FEA approach

[orkraggurn]

Hi all,

I’m new to PrePoMax and FEA in general. I’m struggling to produce a good analysis for my model, a balloon that is subject to an atmospheric pressure gradient. To model this, I’m using PrePoMax’s hydrostatic load, and setting it such that the magnitude is highest at the top of the balloon. However, when running analysis I’m noticing that the balloon seems to just tip to one side, rather than stretch in the z direction and expand circumferentially like I expected. I’m not sure if the problem is with my load, my model, or my boundary conditions, but I have tried quite a few different methods for analyzing this model and all have come up short.

I’ve tested hydrostatic loads on simple pressure vessels and PrePoMax seemed to show proper deformations, even when running non-linear analysis. But as soon as I add “seams” (the longitudinal components that run around the balloon, which are stiffer than the balloon itself), I run into issues.

The image below shows the finished analysis. When the analysis finishes, a message appears saying, “Some node coordinates in the result .frd file are different from the coordinates in the model mesh. Apply model mesh properties (part names, geometry…) to the result mesh?”

This is the base of the balloon–for some reason the seams are detached, even though I applied a tie constraint.

Hydrostatic loading parameters

Boundary conditions–I’m wondering if this is a possible culprit. I want the BC at the base of the balloon because that is where a payload would be attached.

Finally, here’s a previous analysis I did with similar hydrostatic loading parameters, but without the seam geometry. The BC was also the entire top dome of the vessel, not a few small surfaces like the model above.

I’ve been working on this for a while and I’m at a loss, so if anyone could help that would be great! Please let me know if there’s anything else I can provide to help you diagnose the issue, such as the .step file of my model or anything from PrePoMax. Thanks!

[FEAnalyst]

@orkraggurn

Please let me know if there’s anything else I can provide to help you diagnose the issue, such as the .step file of my model or anything from PrePoMax.

.pmx file with this analysis would be best. Maybe it’s just a matter of tie constraint settings. You should check if it works properly in a frequency analysis.

[orkraggurn]

Thank you for your reply! I tried to compress the file but it’s still around 15MB, so unfortunately I can’t post it here.

I tried a frequency analysis with mixed results:

Is there a way I could compress the file further so that I could post it here? Thank you again for your help.

[FEAnalyst]

You can upload the file to some hosting website and share the link here.

[orkraggurn]

Great, I uploaded the file to dropbox

https://www.dropbox.com/scl/fi/hmfqpr6pod9u8ue42svmb/orkraggurn_hydrostatic.zip?rlkey=gyf4spdis514l0qw4kucbu5yc&st=bs7s4h8w&dl=0

I also decided to combine the geometry and see if the analysis was successful, and it was! So it probably does have something to do with the tie constraints, since almost nothing else about the geometry was changed (I made the walls thinner but I don’t think it would have an effect). Here’s a link to the working model:
https://www.dropbox.com/scl/fi/azqc7y2eg1x6493hlf1pv/orkraggurn_combined_geometry.zip?rlkey=w6ypgz3j9xxyp5hwoznzxcheh&st=5d289w98&dl=0

[FEAnalyst]

There’s a large difference in mesh densities of both parts. You can increase the position tolerance for tie constraint (to something above 1 mm) to compensate for it but the vessel part shouldn’t be that coarse. Also, such thin-walled parts usually need to be modeled with shell elements (and you can tie solid parts like welds to them if you want).

[orkraggurn]

I changed the pressure vessel from a solid part to a shell part and increased its mesh density. However, it appears that the longitudinal “seams” are completely disconnected from the body. I created the tie constraints by first creating contact surfaces in my model, then going to Constraints → Search Contact Pairs. PrePoMax seemed to correctly identify the contacts. I ran a few different frequency analyses, progressively increasing the tie constraint from 0.1mm, to 1mm, to 2mm, all with the same results.

Below you can see that the vessel is now a shell, and the contact surface is visible from the inside. The slight yellow color shows that the tie constraint was applied to that section.

Here is the link to the new analysis:
https://www.dropbox.com/scl/fi/2ey2lmlcre7jqma0sud84/orkraggurn_shell.zip?rlkey=fs10pemlx2heiemaf1ckxdxxd&st=adr3wi3y&dl=0

[FEAnalyst]

You should swap master and slave (master should be coarser) and account for the shell thickness (using either position tolerance above 2.5 mm or shell section offset of 0.5).

[orkraggurn]

It works! So some things I’ve learned in case folks come across similar issues:

1. Thin-walled pressure vessels should generally be modeled as shells
2. Large differences in mesh densities can cause problems, and for a model of this size a finer mesh that more accurately follows the geometry will be better
3. When making constraints, the master should be coarser
4. When using shells, constraints should have a position tolerance that is above half the thickness (or a shell section offset, though I’ll admit I couldn’t find a way to edit this in the constraint, please let me know where that is for the future)

Is what I’ve written above generally correct? Also, based on your suggestion of using 2.5mm, that to me implies that PrePoMax (and maybe FEA software in general) adds shell thickness symmetricly, is that correct?

Lastly, thank you for your help! I’ve seen a lot of your videos and read through much of your advice in the PrePoMax forums, I couldn’t have gotten to this point without that–you rock!

Verification of proper constraints

[FEAnalyst]

I’m glad I could help you with this.

@orkraggurn

or a shell section offset, though I’ll admit I couldn’t find a way to edit this in the constraint, please let me know where that is for the future

This is set in the shell section dialog, it’s not just a setting for tie constraint.

@orkraggurn

Also, based on your suggestion of using 2.5mm, that to me implies that PrePoMax (and maybe FEA software in general) adds shell thickness symmetricly, is that correct?

Yes, unless offset is used. It’s meant to offset the thickness so that the surface (geometry and mesh) in your model is not in the middle but on the top/bottom or in other location with respect to the expanded shell (with thickness).