Using CBUSH Elements in GAP Element Connections

[nl12345]

Hello,

I have a mass element attached to an RBE3 connected to surface #1, and surface #1 is connected to surface #2 via gap elements. Because I’m not concerned about the stress results from surface #1 and just care about the stiffness it imparts onto surface #2, I tried to replace surface #1 with a series of CBUSH elements that all have the same stiffness. However, whenever I try to run this analysis, I get an excessive pivot ratios error. I activated BAILOUT to see the deformation, and the deformation looks almost identical to the results when surface #1 was represented using plate elements, so I'm not sure why it's throwing the error. Is there a way I can resolve the excessive pivot ratios error using this approach or is there another approach recommended to achieve the same result?

See images of the compared results below:

SOL 101 Analysis with Surface 1 (top plate) represented as plate elements:


SOL 101 BAILOUT Analysis with Surface 1 (top plate) represented as CBUSH elements:

 

[BlasMolero]

Hello!,
Please post a copy of both FEMAP (*.modfem) models and we will take a look to investigate the problem, the devil is in the details!, thanks!.
Best regards,
Blas.

 

[nl12345]

Hi Blas!

Thank you for the response!

I cleaned up the modfem to highlight the results in question. Please find the modfem attached.

Note that Result 14 relates to Group 5, and Result 29 relates to Group 7.

Thank you!

 

[SWComposites]

why are you bothering to replace surface 1?

 

[nl12345]

It's definitely just a matter of preference. Personally, I'd rather not have a "dummy" plate included in my model if the only property we really care about is the stiffness it imposes for contact.

 

[dcascap]

Checking your model I noticed 2 things, that will make your pivot ratio error to go away:
1. Your CBUSH and gap stiffness are way too high. Use 1E6-1E9 but not 1E20, that will give you an ill-conditioned matrix, it's very difficult for nastran to manage and invert a matrix without numerical error if you have very high stiffness differences.
2. You didn't constraint the rotations on your CBUSH connections so that nodes (Independent RBE3 rot. DOFS, and the gap rotation DOFS)

I changed that 2 things and problem solved

I don't really understand why are you using Gaps on that model, seems like an overkill, you could do it with the plate or with the CBUSH only (you already know you have a downward load)...

Hope it helps!
Diego

 

[nl12345]

Hi Diego!

Thank your support on this!

1. I originally had a stiffness value of around 1E10, but I noticed after iterating when running the analysis in BAILOUT, a stiffness value closer to 5.0E20 caused the VM stress to converge on values similar to the plate-on-plate contact analysis. My last thought on this was that a very specific high stiffness around this range would cause the error to go away. Was this just a coincidence?

2. Thank you for pointing this out! I'm always hesitant to constrain rotational DOF's on the independent RBE3 nodes...

This model is just a proof of concept of a more complex model that contains discontinuous conical contacts. I just wanted to verify this to method of contact before moving forward.

Thanks again!

 

[BlasMolero]

Dear NL12345,
In fact, CGAP are redundant, but if you insist to have CGAP + CBUSH + RBE3 in the same model instead to have to apply external rotational constraints in nodes shared by CGAP & CBUSH the trick is to convert the RBE3 in a rigid RBE2 activating the 6 DOF in the DEPENDENT NODES. Of course, the model behaviour will be stiffer.
And always stiffness in both CGAP & CBUSH elements set to k=1e6 Lb/in



Best regards,
Blas.