Hello, Is it possible to use parallel processing for the ANSYS and/or CFX parts of a fluid-structure interaction simulation? I have access to an 8 processor Linux server. Thanks!

If you have a parallel license, I think you can do this. Why do you ask? Doesn't it work?

Gert-Jan

I'm new to FSI... do have parallel license. I think I read somewhere that at least the Ansys part cannot run parallel, but I'm not sure. How do I start the parallel FSI? From the ANSYS launcher (MFX option) or from the CFX solver manager? Thanks for your help, Jorn

I am new to FSI as well, sorry. The flow calculation can be done in parallel, the Mechanical simulation not. But you won't need that as in general this requires less computational time, provided you do not perform explicit Mechanical calculations.

There are tutorials on FSI which should lead you through the process. I would suggest to try these first.

Gert-Jan

Thanks for the info... I did the tutorial as well as some first transient FSI simulations of a flexible dynamic analysis in ANSYS coupled to a transient fluid flow analysis in CFX. I got the hang of it now I guess. Too bad the ANSYS part can't be run parallel...

You can run the ANSYS part in parallel, but only local parallel. When starting from the CFX Solver Manager, in the box where it asks for additional ANSYS arguments, just enter:

-np 2

to make use of 2 processors. However, caution is needed, which is best explained with an example. Lets say you have a machine with 6 processors available. You run CFX on all 6 processors using HP MPI and ANSYS on 4 processors (ANSYS uses MPI for it's parallel communication). Sounds good right - the CFX run isn't going to use those processors while ANSYS is solving ? Unfortunatley any MPI slave process tries to uses 100% CPU when it is idling. So when CFX isn't doing anything and ANSYS is trying to solve, 5 of the CFX CPU's will still be trying to pull 100% CPU. The results is ANSYS will solve dead slow. When ANSYS isn't doing anything and CFX is trying to solve, ANSYS will still try to pull 300% CPU, which will result in CFX solving dead slow. Note that this appears to just be the way MPI works, it's got nothing to do with CFX or ANSYS specifically. You don't run into this problem if either CFX or ANSYS is running in serial. You can run CFX using PVM to avoid it pulling CPU when it isn't doing anything, but you don't have that option for ANSYS. So in general, if both codes are running in parallel, run them on different machines or make sure you have enough CPU's (or cores) to serve both solvers simultaneously.