Thermal Expansion with RBE2 element

[Anonymous]

Hello,

I am trying to build a thermal expansion model for a large assembly.  I have a number of components attached via RBE2 elements.  When I try to find displacments of nodes, I get unexpected results.  I built a simple model with a series of parallel plates that are attached with RBE2 elements.  The temperature of everything should be 70, but the plates move when a CTE is introduced for the RBE2's.  I'm OK with setting the CTE of the rigid elements to zero, but I set it to the same as the component it was attaching to in order to not create thermal stresses.  Is this a known issue?  Is there some simple fix that I'm missing?

[Anonymous]

I did a little more research this morning on the model.  It appears that one node of the RBE2 is at zero degrees, regardless of what temperature is specified in the load case.  This temperature differential is creating thermal expansion of the RBE2 elements.

Has anyone else seen this?

[shigeaki.k]

Sorry @Anonymous.

do you have the file you could share with us, so we can have a closer look at the system being analysed?

Regards,

Shigeaki K.

[Anonymous]

Hello,

In this case, I set all the temperatures in the model (material reference temperature, default temperatures, and temperature on nodes) to 70°.  I also set the thermal expansion coefficient to the RBE2 elements holding the plates together to non-zero values.  When I run the model, I would expect zero thermal expansion of the model; however, the plates move according to a 70° temperature difference across the RBE2.

See the pictures below for a bit more information.

I tried to attach a .nas and a .out file, but they were rejected, saying they didn't have valid extensions.  So, I changed the file extensions.  The file named "RBE2 CTE Issue_nas.txt" is a .nas file.  The file named "rbe2 cte issue_OUT.txt" is a .out file.  You can change the file extensions back.  I can send along any other files, if needed.  I appreciate the feedback.

[jdalidd · Accepted solution]

Hi @Anonymous,

Thank you for attaching the sample Nastran file. I took a look at it and I think I see the problem. You have specified a LOAD temperature, but it looks like you haven't specified an initial temperature (TEMP(INITIAL) = 1). Without specifying an initial temperature, the solver will use the reference temperature on the material cards, however, a rigid element does not have a material card associated with it, so the initial temperature would be zero if not specified.

Please try adding the initial temperature card (i.e., initial conditions) and let me know if it fixes the problem. I recommend always explicitly specifying the initial temperatures in all analyses.

Cheers,

Jonas

[Anonymous]

Hi Jonas,

Yes, that does clear up the issue.  Very helpful advice.  Thank you!