superelements assembly

[david1982]

Hi all,

I'm studying the substructure modelling and i would like to know how to assembly superelements in patran. I don't know how to do the analysis for each superelement.

I found MSC.Nastran 2001 Superelement User’s Guide, but doesn't explain the modelling proces in patran.

Do you know any tutorial/example/exercise... where this theme is clearly explained?

Regards,

David

 

[franc11HD]

The easiest way I found was to create a group you want to condensate into a super element. It needs to contain all the internal and boundary nodes and elements.

Then you go to Elements - Create - DOF List

Give a name select define terms, choose all the nodes of your super element and the DOF of those nodes. APPLY

Then go to Analysis - Solution Type - Select ASET and you should be able to choose the DOF list you previously created. This will create in the bdf file a ASET Card.

Then go to Analysis - TRanslation PArameters - Ext. Superlement Spec - Method DMIGPCH and select what you need, generally stiffness and load and give a EXTID number (anything).

This will create the EXTSEOUT card.

Run this analysis. Once this is done, Nastran will create a *.pch file that contains the Stiffness matrix (KAAX) and the load matrix (PAX).

When you want to run the external elements of the model and "plug" the super element, you only need to add (by hand) in the bdf file and include line that will include the .pch file and add
K2GG=KAAX
P2G=PAX

just before the subcase or in the subcase.

There is a lot of things to be carefull about that could make this not work, but this process, well understood and apply correctly works. At least it worked for me.

Good luck!

 

[david1982]

Thanks franc, your post has been very useful!

I have another question referent to a internal superelements. If

you want to do an iterative analysis of internal superelment,

changing mesh or/and thickness, what I have to do?

First of all, I create the superelements with constraints and loads.

Then, in analyse/select superlements, I've selected one

superelement and check Write PART superelement, but after run, it

doesn't work corectly.

Any idea?

Thank you

Regards

David

 

[franc11HD]

I never used that option and don't really know what it actually does. But I don't really understand what your are trying to do. If you want to iterate on your superelement, you shouldn't create a superelement in first place.

My understanding is to use superelement for geometry that does not change in order to speed up the solving process or to share with other people. It is basically a stiffness matrix that you solve once and reuse afterwards.

Therefore, if you want to iterate on the "internal part", then create a superelement of the external and use the "internal" as is and iterate on the mesh or the thickness directly.

Using superelement in submodeling (again as I understand the process) is actually using superlement for the structure that do not change. For example, you have a big cylinder on which is attached a lug. You want to iterate on the whole diameter of the lug. Then you create a superlement of the cylinder until the boundary of the lug. Then, keeping the boundary nodes, you can modify the geometry of the lug and mesh in order to find the optimal design and you do this wihtout always solving the cylinder part since it is already condensed into a stiffness matrix.

Or maybe I just don't understand what you are trying to do.

 

[david1982]

Ok, I have a superelement created for the structure that do not change and I reached the results exactly than without superlements, decreasing the time of calculus. Thanks for your posts!

regards

david