Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

OptiStruct creating Beam Elements

Hey,

I want to make a static analysis of a composite part. I'm simulating a monocoque. I want to represent the axes by beam elements. As you can see in my attached file this works very well. The following is repeatedly observed when the analysis is running:

*** WARNING # 5628
The compliance is negative or large 9.02038e+11.
The rotational displacement has large magnitude, 159742 degrees (larger than 180).
The rotational degree of freedom may not be constrained properly in the model.
subcase id = 1
grid id = 1
component = 4

Can you please help me to solve the problem? Unfortunately i am under a lot of time pressure.

Thank you in advance!

Unable to find an attachment - read this blog

Find more posts tagged with

English

OptiStruct

Accepted answers

All comments

Adriano_Koga

Hi @Annika

Large compliance is usually associated to rigid body motion, and usually missing proper boundary conditions.

Looking into your model, there are a few temp nodes that you might have used for building your model.

The problem here is that you probably didn't use this node to create your beams, so that the temp node and the beam nodes are different.

Then when you constrained your model (with SPCs), you've used the temp node instead of the beam node.

There are a few ways of correcting, but i would say, delete the SPCs, clear temp nodes and create the SPCs again with the proper nodes.

image.png.91736c7227d4d42e4c713552e8d1b6cd.png

Annika

Thanks for your quick answer!

I cleared the SPC and tried it with the proper nodes. But there is still a problem. Is it possible that I have to change the RBE3 Element type to a RBE2 rigid one?

Adriano_Koga

rbe2 and rbe3 are 'opposite' in terms of dependecy. So if you're having some issue with DOFs from RBE it might be necessary.

Or create a CBUSH to avoid constraining RBE nodes.

Can you share the .out with error message?

Annika

I would like to use the beam elements to direct forces into my shell model. However, the forces do not act directly on the beam elements. I wanted to give restrictions on the bar elements. Do I need RBE 3 to transfer forces? And RBE 2 when I'm having some issue with DOFs?

Unable to find an attachment - read this blog

Adriano_Koga

did you check for your temp nodes? did you fix the constraints iin these nodes?

your model is running, with no error, except by the large compliance which still indicates some issues with contraints.

you could apply forces directly on your beam elements, or use RBE2 or RBE3. In case you use RBE2 or RBE3 you just need to take care of not creating SPCs at their dependet nodes (central node in RBE2 and the opposite in RBE3).

Also take care to not make the RBE using colinear nodes, avoiding some rotational instability.

Annika

Yes I Checked the temp nodes and removed them. Would it be possible that there are problems with the connection from the beam elements to the RBE3 element to the shell model?

<?xml version="1.0" encoding="UTF-8"?>

Adriano_Koga

do you know how to setup a modal analysis in OptiStruct? It would help you figure out what is not properly fixed.

Or even opening the H3D result file from your model, and change the deformation scale factor and try to identify what is going on in your model.

Probably something is free to rotate.

Other than that:

- check for loose elements/edges

- check free nodes (F10)

- check material properties and units consistency

- check thicknesses

Annika

I found the problem a knot was free. Now everything works. The compliance is no longer too great.

Thank you so much for your help! You helped me a lot /emoticons/default_smile.png' srcset='/emoticons/smile@2x.png 2x' title=':)' width='20' />

Annika

Sorry, I have one more question. Can you explain me the following:

*** INFORMATION # 3454
MPC, RBE# (and other rigids) and JOINTG constraints for
subcase 1 will be enforced with lagrange multipliers.

What does it mean?