Variable pressure in Workbench

[Baldy112]

Does anyone know how to put a variable pressure in Workbench. There's a drop down menu to select other options but there's only one option and that's constant.

 

[Stringmaker]

Baldy,
You're going to have to use the insert commands function under the Solution tab. Basic procedure goes like such:

-Define local coordinate system
-Get/define all necessary parameters/arrays
-Define pressure function (SFFUN command)

Have you done this before in Ansys? If not I could try to provide you with a macro which may help you.

-Brian

 

[Baldy112]

I have never used Commands in ANSYS Classic.

But while reading the Help Documentation, it states that you need a License Level of ANSYS Professional and above to be able to use the Commands. Which I don't have, so thanks anyways.

 

[ansysfreak]

Hi

I think Ansys 11 will have an function(or table) to give to your pressure, so have patience.
Ansys 11 will come out at the end of feb.

Grtz
Garry

 

[cbrn]

Hi,
it may be simpler than this, without waiting for future versions (do the best you can with what you have, no? ;-) )
let's say you have a pressure varying with the coordinate Z of the system CSYS,21 (whatever this coord sys can be).
If you don't want to cope with SFFUN, simply discretize your P-variation law in, say, 10 P values at 10 Z coords.
Then, add a Commands snippet in the Solution and add these commands:
/PREP7
*DIM,P_TABLE,table,10,,,Z,,,21
P_TABLE(1)=p1,p2,...,p10 !pressure values
P_TABLE(1,0)=z1,z2,...,z10 !coord values
cmsel,s,COMPONENT_OF_PRESSURIZED_SURFS
SF,all,pres,%P_TABLE%
allsel
/SOLU

et voilà! The SFFUN method is, by far, more sophisticated, but also more difficult to catch up...

Hope this can help.

Regards