Paynee:

It appears that you are using the ISTRESS command to apply the initial
stress.  The ISTRESS command can only be issued once.  If you issue it a
second time, it will overwrite the previous entry.  You need to use the
ISFILE command approach.  The following steps should work.

1.  Apply the first set of initial stresses using the ISTRESS command
and write that information to a file using the ISWRITE command.
2. Remove the applied initial stresses.
3. Apply the next set of initial stresses and write them to a different
file.
4. Remove the applied initial stresses.
5. Combine the two initial stress files into one file using a text
editor.
6. Apply the initial stresses stored in the combined file using ISFILE.

One note: in the next ANSYS Release (11.0), we are replacing the ISTRESS
commands with a group of initial state commands.  With those commands
you will be able to directly apply different initial stress values to
different groups of elements.  So the above process will only be
applicable to Release 10.0 and before.

Regards.

Daniel Shaw
ANSYS

-----Original Message-----
From: mems-talk-bounces@memsnet.org
[mailto:mems-talk-bounces@memsnet.org] On Behalf Of li ling
Sent: Tuesday, January 09, 2007 8:07 PM
To: mems-talk@memsnet.org
Subject: [mems-talk] About initial stress in ANSYS

Dear Alls
   Do anyone knows how to apply the initial stress in ANSYS simulation.
   I have two different materials (silicon nitride and silicon dioxide)
to apply initial stress.But It seems that the initial force in nitrideit
always overwrite the  one in silicon dioxide I applied first.. Would
anyone tell me how to fix this problem.