rigid element for 3D analysis NASTRAN

[jmarcoj]

I am working with 3D elements (CHEXA) using NASTRAN. I need to use rigid elements and I am using RBE2s but they are not rigid at all for 3D analysis. I have alread used those elements before (2D models) and they work great but when I try and connect brick elements the rigid elements RBE2 are not rigid anymore.
The displacement of the slave node is not equal to the displacement of the master (I thought of a rigid rotation but even the lenght of the rigid is different).

Does anyone know why this happens and how to solve this problem?

cheers

 

[Aerodesign]

Simplistically. CHEXA has limited rotational stiffness,if you are expecting to use DOFs 1-6 (ie MPC all translations and rotations) you will have to coat the CHEXA's with thin CQUADs. If you want to MPC drilling DOF's you need to consider carefully the configuration of the RBE.
Hope this helps.

 

[jmarcoj]

Thank very much for your help.

I thought about coating CHEXAs with CQUADs but the problem is...what property and thickness should I give the CQUADs in order not to affect the analysis?

 

[Aerodesign]

jmarcoj,
It should not make too much difference, use 1/100th stiffness of HEXA elements. We typically scale stiffness by this factor and use a 0.1mm thick (our structures are typically 0.5-10m long and 2-3mm thickness) You could try different values and see how it affects the results.

 

[jmarcoj]

Thank very much indeed.
This infomation was really useful.

Cheers

 

[ykantor]

jmarcoj

a rigid element stay rigid in linear analysis, dosn't matter if its 2D or 3D.


you wrote:
"The displacement of the slave node is not equal to the displacement of the master".

The displacements are not necessarily equal.

check your model by replacing the rigid element with a pyramid made of bars, ans see what happens

cheers