Abaqus surface-based fluid cavity. 2

[UMEngineer]

I've been tasked with creating a 3D model of a demo inflatable structure here in our lab. The goal is to inflate it in ABAQUS, and I have been making some progress in using the *FLUID CAVITY keyword. However I'm noticing odd things in my results. I have the pressure of the gas increase to 4psi in a tabular form, however as I watch the frame by frame, the stress concentrations on the structure vary oddly, and the model deforms oddly. Almost as if it was a ball being pressed back and forth against the floor, expand contract, that kind of deal. I'm not really sure what is causing it.

Another problem I seem to have, is a few jobs I run, the input file gets submitted and cleared, but ABAQUS never attempts to start ABAQUS/Explicit, it just sits there int he running state. When I monitor it, no signs of incrementation is occuring, however the process is running in the background, it happens on any new jobs I run since yesterday. Older saved .cae files work fine.

Last problem I'm having at the moment, is more of a how-to question. We want this model to inflate from 0psi to operating pressure, but I can't seem to figure it out in ABAQUS. I've read over the example file on the side impact airbag, but I can't seem to figure out how to get a reference mesh, and then the mesh of the folded structure.


If anyone can help, I greatly appreciate. I hate asking for help, but I've been stuck on this for a few long days. I can submit my input files if anyone thinks th at may help.

 

[UMEngineer]

Any help at all?

 

[akabarten]

Hello,

Unfortunatly Abaqus/CAE dose not support making of reference mesh and folding. To generate reference mesh in Abagus format you need to write a script which take mesh from model and write to file in correct format. I know Ansa can show abaqus reference mesh but I not sure does Ansa can generate reference mesh.
Usually folding is done in third part software. You can try use free pre-postprocessor for Ls-Dyna FE solver. Please take a look here:

http://www.lstc.com/lspp/content/tutorials/7/t7p1.shtml

>>> I can submit my input files
Please do it.

Reagrds
akaBarten

 

[UMEngineer]

Thank you akabarten, you have no idea how helpful that has been already. I have uploaded my input file. Explicit is running now, the big problem I've been having now is the reference mesh, I have to inflate it, then do contact analysis with high speed projectiles.

Again, thank you so much.

 

[akabarten]

Hi,

I took a look at your model. I have same suggestions.

Please try change mesh of fluid cavity. Triangular elements at top and bottom have low quality (very small angles).
This is a reason why you get unrealistic stresses in this region.

You mentioned about reference mesh. Reference mesh works only with three node memebrane elements (M3D3). In your model fluid cavity is model also with M3D4 elements.
Why do you need reference mesh, elements in your model are not distorted? Maybe I don't know all details about your model.

Reference node of fluid cavity has only one degree of freedom (8 - pressure). In this case boundary condition type pinned will not work. Reference node is always in the same position during analysis. Fluid cavity can move in a space but node will stay in the same place. If you want to block movement of fluid cavity you can not use reference node.

I made simple example with similar model as yours. Please teak a look for the inputdeck.
Regards
akaBarten

 

[UMEngineer]

That answers some questions I had, thanks.

I had the mesh the way I did because meshing as you had it creates stress concentrations so I was hoping to avoid those. Normally I have the top and bottom partitioned in such a way that they are mesh with M3D3 and the mesh algorithm used around it is Swept M3D4.

I mentioned the reference mesh because the goal is to inflate the model. I start with a zero volume, folded model and inflate it, very similar to an airbag analysis in Ansys only much slower.

I took a look at LS-Dyna pre-processor. I don't think I can get it to work, but I have not given up yet, I have imported the model, I just need to find a way to mesh it.

The reference mesh is the mesh at zero volume, the model I have made is after the structure is inflated.

Thanks!