Stiffness Matrix Element problem

[alenglaro]

Hello,
I need to represent a complex 3d model by its stiffness matrix calculated "manually" at a desired point by applying on the full 3d model unitary loads in each DOF direction and measuring displacements. I used these values in a Stiffness Matrix Element but solver returns "Element Type not supported by Translator". I'm using Nx Nastran Static solver.
Can anyone explain me how to properly use this element (which solver supports it and in which coordinate system the matrix is expressed)? Is there another method to get the same behaviour? I think I can't use CELAS or CBUSH elements because a load applied, let's say, in X direction affects displacements of all DOFs so it can't be represented by a single spring element.
Any suggestions?
Thank you and sorry for my english.
A

 

[rb1957]

maybe "superelement" is what you need ?

Quando Omni Flunkus Moritati

 

[jbrackin]

You have a couple of options. One is to use a GENEL, see the Nastran documentation for explanation and example. The other possibility would be an external superelement, see the EXTSEOUT Case Control command in the Nastran documentation.

 

[alenglaro]

Thank you rb1957 and jbrackin!
I will try both superelement and GENEL methods. I have few more questions. It is possible to insert in a model multiple superelements representing the same complex part but translated and rotated to a specified position? Can I do the same with GENEL?
In Femap i can't find how to create a GENEL element. Maybe you can only create it by inserting code lines in the nastran bdf files?

 

[rb1957]

it makes sense to me that you can position a superelement in space, and that you can reuse the same element ... "all" the superelement is doing is replacing a bunch of detail elements with a stiffness matrix.

haven't used "GENEL", maybe it is not incorporated into FeMap ... ask them ?

Quando Omni Flunkus Moritati

 

[alenglaro]

I generated an external superelement with two boundary nodes. One will be constrainted to ground, the other will be connected to another structure. Now i have to include two of these superelements in the main model at specified positions but i can't find a detailed tutorial on how to do it. Can you help me? Thank you very much!

 

[jbrackin]

Femap does not support the GENEL, if that method suits your application, then you would need to refer to Nastran documents, create the bulk data and then could "include" it via Femap start text.

A couple of notes on Superelements. First creation of the external Superelement does not require a superelement license, however attaching and using that external superelement will require a superelement license. Nastran does offer the ability to take a "primary" superelement and then define a transformation to relocate it as a "secondary" superelement. Femap does not support that special input, so you would need to create the bulk data entries via text editor and include them via start text. This would be suggested for advanced/experienced Nastran users only.

If you want to use Femap to set things up, it would easier to actually make a copy of your model, transform the model, then create another superelement of the transformed model.
In an assembly run you can attach these multiple external supplements using the Femap interface.