INTERFACE ELEMENT IN NASTRAN

[JIJINAV]

I am using nastran student version for fe analysis. My model consists of CHEXA elements and CQUARD4 elements. I want to incorporate interface elements between shell and solid elements. but i don't know how to do this in nastran. Can any one suggest how to make interface elements in nastran.
Thanks in advance.

 

[stressebookllc]

The important aspect here is you need to make sure you transfer the moments accurately between the shell and solid elements.

You may find this thread useful:
thread1234-335821

Aerospace Stress Analysis and FEA Courses

http://www.stressebook.com

Stressing Stresslessly!

 

[JIJINAV]

Thanks for the answer.
is this the effective way to incorporate soil-structure interaction through interface elements in Nastran?
please help me.

 

[aerostress82]

Wherever your solid elements are to interface the shell elements, cover your hex elements with quad4 elements at the interface region. (I will call these quad elements as "FACE ELEMENTS" from here on)
For these face elements, assign a very small thickness like 0.001mm. Additionally, for these face elements, assign 12I/T**3 value in that pshell card with a value like 1e9 smt (it is 1.0 by default). This will make sure the bending is perfectly translated from your hex nodes to the (covering) shell nodes.

At the last step, make sure you are connecting the face element nodes to your quad elements (your original representation of a midsurface of your model I guess) with RBE3 connections. The dependent node of the RBE3 will be on your QUAD elements, whereas the independent nodes of your RBE3 will be on your FACE ELEMENTS.

Additional information on RBE3 connection on a single part that is modeled with QUAD & HEX together:
Not sure if you are using Patran/Hypermesh/ANSA, but ANSA has a weighted scale factoring for an RBE3 connection to different distance nodes that it is connecting to. Meaning, if your RBE3 is connecting to 1 dependent and 2 independent nodes and if these 2 independent nodes are 5.0mm and 10.0mm away from your dependent node, the scale factors defined in the RBE3 card will be 0.666 and 0.333 subsequently. Patran also had an additional utility function for this scale factor issue. Not sure if they have it as default in newer versions as I have only used 2005 and 2008 versions only.

If your mesh is perfect, you can just connect 1 dependent node to 2-3-4-5 independent nodes at each horizontal/vertical plane location of your interface region. The trick is to have the RBE3s connected exactly where the material should have been continuous. You don't need to connect the RBE3s to any nodes that are not in the continuum region of the material.
(Stiffener cross-section cut-1 side of the stiffener is quad, the other side is HEX - your RBE3s will only be at the cross-section cut plane of your flanges/web of the stiffener and will be connected at the quad elements via dependent node of your RBE3)

Spaceship!!


(Aircraft Stress Engineer of 7 years experience - United States)