FEMAP/Nxnastran Linear gap modelling

[kanraj]

Hi,
I have an isodamp sandwiched between 2 plates. I have ignored isodamp (0.1" thick) in the model. Under the given linear loading condition, I see the plates bending and touching each other which in reality is prevented by the presence of isodamp. I then tried to use a linear gap as shown in the picture. I'm not happy with this as its acting like a rigid element. Could someone please share their thoughts on this way of modeling?

Thanks

 

[Tuw]

Hello,

I dont think we can understand your problem without the pictures. What given linear loading condition, we dont see it...

My guess is, if you are using linear solution (for example Sol101), then cgap elements will behave linearly as well, and it is possible that the cgap element is pretty stiff (based on your input) and is thus behaving like rigid element.

Tuw

 

[BlasMolero]

Dear Kanraj
In linear static analysis with NX NASTRAN (SOL101) the 2-node explicit contact CGAP elements to behave as a contact element (not like spring) you need to activate the option GAPS AS CONTACT in the NASTRAN BULK DATA OPTIONS:

This is a requirement for NX Nastran only, checking this option will allow gap elements to be treated as linear contact elements during a Linear Static analysis (SOL 101). This option creates a BCSET in the case control section of the NX Nastran file, which is what tells NX Nastran to use the gaps as linear contact elements.

Note:
If you have linear contact defined elsewhere in your model using the entities created on the Connect menu, there is no need to turn this option on for gaps to work as linear contact elements, as a BCSET is already being created in the case control.

Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/