Nodal Forces in Ansys !

[Pavan Bathla]

hi
how can i put the nodal force at a node into a variable in ANSYS ?? I tried this command but it didn't work !
*GET,Var,NODE,#Node,RF,FX

I can list all the nodal forces thru' GUI mode, but i need to put it in a variable. Any help in this regrad will be appreciated, I have to do this by Wed night, so it's kinda URGENT !

--
Pavan

[Dave Lindeman]

Pavan:

Well, if you're talking about applied nodal forces (F,NODE,...), then try:

*GET,Par,NODE,n,F,[FX,FY,FZ,MX,MY,MZ]

If your're talking about reaction forces (PRRFOR), then try:

*GET,Par,NODE,n,RF,[FX,FY,FZ,MX,MY,MZ]

If you're talking about nodal forces (the forces required to maintain
equlibrium at an unconstrained node), then select the node and the
appropriate elements, then use:

FSUM
*GET,Par,FSUM,,ITEM,[FX,FY,FZ,MX,MY,MZ]

Note that if you select all the elements attached to a node the nodal forces
should sum to zero. Therefore, you only want to select the elements on one
'side' of the node.

Regards,

Dave

Pavan Bathla <bat...@email.com> wrote in message
news:39064A15...@email.com...

Opinions expressed herein are my own and may not represent those of my employer.

[Jeffrey Tischler]

Don't really know, but suggest you try mapping nodal force onto a path and use that as a variable. I don't have Ansys anymore and can't play with it.

[Jeffrey Tischler]