XANSYS Message: 93180 [Go back to message list]
[bookmark on del.icio.us]
No rating yet
Rate item:

Subject: Re: INISTATE and user material
Author: Guoyu Lin
Date: 2008-05-06 14:35:44

To access initial stress from usermat, you can use following API:


c *** get initial stress
call vzero(sigi(1),ncomp)
i = ncomp
call get_ElmData ('ISIG', elemId, kDomIntPt, i, sigi(1))

thanks,

Guoyu

Guoyu Lin, Ph.D.
Technical Fellow
ANSYS Inc.
275 Technology Dr.
Canonsburg, PA15317
Tel: 724-514-3635
Fax: 724-514-3118
Email: guoyu.lin_at_ansys.com
------------------------------------------------------------------------
--------------
The information transmitted is intended only for the person or entity to
which it is addressed and may contain confidential and/or privileged
material. Any review, retransmission, dissemination or other use of, or
taking of any action in reliance upon, this information by persons or
entities other than the intended recipient is prohibited. If you
received this in error, please contact the sender and delete the
material from any computer.


-----Original Message-----
From: xansys-bounces_at_xansys.org [mailto:xansys-bounces_at_xansys.org] On
Behalf Of Dave Lindeman
Sent: Tuesday, May 06, 2008 10:23 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] INISTATE and user material

If the material is nonlinear (with the possible exception of
hyperelastic), then there are no doubt state variables (e.g., strain
components) that would need to be initialized also. It may be possible
to pass all of the necessary values (including the initial stresses)
into USERMAT via the state variable array, but unless the initial state
is trivial (e.g, still in the linear elastic regime), you'll end up
having to calculate the proper evolution of the strain components and
state variables to ensure everything is consistent (i.e., you'll need to

simulate the loading that produces this initial state). It all depends
on the nature of your constitutive model I suppose.

Regards,

Dave

-------------------------
Dave Lindeman
Lead Research Specialist
3M Company
3M Center 235-3F-08
St. Paul, MN 55144
651-733-6383


Daniel Aubram wrote:
> Dear all,
>
> Ansys manual says that an initial stress state for PLANE182 elements
can
> be established in the first load step when issuing INISTATE command or
> upf subroutine USTRESS.
>
> INISTATE works fine for standard linear elastic material. However, I
> want to perform an analysis with a user defined material by using upf
> subroutine USERMAT, but now INISTATE does not put an initial
> stress. The stress array in USERMAT is left blank.
>
> I only changed the material characteristics input considering the user
> material but not the keyoption keyopt,1,10,0 (No user subroutine to
> provide initial stresses (default)) or anything else. Are there
additional
> commands or options that have to be considered?
>
> I found nothing in the ANSYS manual referring to this topic. Looks
> like INISTATE together with TB,USER is intended to work...
>
> Thank You!
>
> Regards,
> Daniel
>
^--------------------------------------------------------
| XANSYS - www.xansys.org |
| The Discussion List for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
^--------------------------------------------------------
^--------------------------------------------------------
| XANSYS - www.xansys.org |
| The Discussion List for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
^--------------------------------------------------------

Posts possibly associated with message #93180AuthorDateScore
93165INISTATE and user materialDaniel Aubram 2008/05/06 
93166INISTATE and user materialDaniel Aubram 2008/05/06 
93178Re: INISTATE and user materialDave Lindeman2008/05/06 
93179Re: INISTATE and user materialGuoyu Lin2008/05/06 
93180Re: INISTATE and user materialGuoyu Lin2008/05/06 
93200Re: INISTATE and user materialDaniel Aubram 2008/05/07 
93201Re: INISTATE and user materialDaniel Aubram 2008/05/07