XANSYS Message: 5869 [Go back to message list]
[bookmark on del.icio.us]
Average Rating: 10 (1 votes)
Rate item:

Subject: Re: Reading in an external Superelement (Nastran)
Author: Mike Andruszkiewicz Mike_Andruszkiewicz@
Date: 1999-10-29 18:09:00

Thomas, I'm not sure this is what you are asking for, but there is a 1997
International Modal Analysis Conference (IMAC) paper using ANSYS showing how to
tie an attached structure (defined only by modal information) to a FEA model.
It is "Experimentally Characterized Dynamic Structures in an Analytical Finite
Element Solution", p1399, vol II. Included is a 2-D example with 6 modes
connected to 2 FEA nodes with 2DOF each, showing how the modal info is input as
SDOF, [designated p( j )], of 6 Modal Masses (=1 typically) and 6 SDOF Modal
Stiffnesses (=w^2 ( j )) connected to ground and then tied to the full FEA model
by constraint equations (CE's). The coefficients of the constraint equations
are the displacements of the [4x6] mode shape matrix rows. That is, using the
definition of modal superposition, physical interface node DOF u(i)= Sum of
(disp i, mode 1*p(1) + disp i, mode 2 *p(2) +...disp i mode 6*p(6)]. This is 4
constraint equations with 6 coef's = constant. ANSYS format wants the
constant=0 so a 7th coef becomes -1. The time consuming part will be to get the
constraint equations, so a code would seem useful. In your case, there would be
18 nodes times 6DOF =48 constraint equations with 25 +1 coefficients from each
row of the NASTRAN modeshape matrix . You would manually have to create 25 SDOF
Masses (Mass21) and 25 springs (Matrix 27) with coincident nodes, one of which
is tied to ground and the other node is the modal SDOF's p( j ).

I think this is how you would do Component Mode Synthesis (CMS) in ANSYS.
However, I have not used it yet in ANSYS, so caveat emptor. If there is another
way to do it, or do it now with ANSYS super elements, I would be very interested
in knowing. Good Luck!

Mike Andruszkiewicz
Project Engineer, Design Analysis, Mercury Marine

John Swanson on 10/29/99 12:57:22 PM

To: "'xansys@o...'"
cc: (bcc: Mike Andruszkiewicz/FDL/Mercury)

Look on the ansys distribution media for a file called wrtsub.F It
is a
routine for writing ANSYS substructure files.
John Swanson
Swanson Analysis Services, Inc.

> -----Original Message-----
> From: Thomas Ernst [SMTP:thomas.ernst@t...]
> Sent: Friday, October 29, 1999 5:41 AM
> To: xansys@o...
> Subject: [xansys] Reading in an external Superelement (Nastran)

> From: "Thomas Ernst"

> Hi,
> I have a problem in that I have a external superelement, the
> result
> of a component mode syn.(CMS) model which contains 18 grids (nodes)
> on
> the interface (BSET) and 25 modes (frequencies). How can I read these
> matrices into Ansys?
> Would it be possible to write a *.sub file which contains the
> stiffness
> and mass matrices produced by Nastran? Could this be performed by
> the use of a small external program?

Posts possibly associated with message #5869AuthorDateScore
5857Reading in an external Superelement (Nastran)Thomas Ernst1999/10/29 
5862Re: Reading in an external Superelement (Nastran)John Swanson1999/10/29 
5869Re: Reading in an external Superelement (Nastran)Mike Andruszkiewicz Mike_Andruszkiewicz@1999/10/2910