CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   FSI simulation is DEAD SLOW (

Lance March 19, 2009 04:25

FSI simulation is DEAD SLOW
I'm doing a 2-way FSI simulation using Workbench. It's basically a pipe with a precribed time dependent inlet velocity and outlet pressure. The problem is that my simulation is really really slow, and I wonder if there are some settings I've missed. One single timestep can take up to several hours even though my mesh sizes are reasonable small.

I'm using a linux cluster with 16 GB RAM and 8 cores with HP MPI Distributed Parallel.

My start command is:
cfx5solve -def $deffile -double -name $name -ansys-license aa_r -ansys-input $inpfile -par-dist $(hostlist -e -s, -a'*8' $SLURM_NODELIST) -start-method "HP MPI Distributed Parallel"

I've tried to add /nproc,2 to the ANSYS .inp file to get two cores, but couldn't see any difference.

I also get a warning that:
The current start method, HP MPI Distributed Parallel, is not a standard
PVM parallel start method, and so the parallel option cannot be changed
independently to Distributed Parallel. Request ignored.

If you are using both -start-method and -par-local or -par-dist on the
command line, you can move the -start-method switch to after the -par-*switch.

What does this mean? I have -start-method after -par-dist in the start command.

Any suggestions that could solve my problem(s) are highly appreciated!

vivekcfd April 29, 2009 15:25

Did you try your problem with a serial run? There should not be any problem in convergence if the settings (e.g. BC and solver options) in your case are appropriate.
Your time-steps (fluid and solid side) should be reasonable, check number of outer iterations and stagger iterations. Are you initializing your transient solution (in the fsi run) from steady solutions (on fluid and the structure side)? If not then try this as well with a steady-state FSI initial run.

What is the ratio of your structure to fluid density? If it is close to 1, in that you will have a lot of problems.

Lance April 30, 2009 07:57

Yeah, I've tried serial runs and different timesteps. The number of staggers are high, around 70... The initial values comes from a steady-state FSI run.

And yes, the ratio between solid and fluid density is very close to 1 (bio-fluid material...). Any suggestion on what to do?

vivekcfd May 1, 2009 02:18

if your fsi coupling effect is linear for certain mass flow and/or viscosity range. You can scale the fluid density via fluid velocity or viscosity such that the Reynolds number remains constant. Scaling via velocity or viscosity will depend on the nature of your problem. If viscous forces on structure are important, I would scale the problem via velocity. On the other hand, if kinetic energy of the fluid or the inertia is more dominating factor, I would scale it via viscosity.

Finally, if possible you should bring your scaling factor at least between 5 to 10.

Similarly, you may also scale density of the solid but have you to know what exactly you are doing while scaling the problem. Try to write down the FSI equations and you will see what happens if you scale things on one side (e.g fluid or structue side).

stumpy May 1, 2009 22:49

I'm assuming that both solvers are iterating at normal speeds, but they are just taking a lot of iterations each timestep. First, create some monitor points for force at the interface and displacements at the interface, turn on coefficient loop monitoring, then watch what happens to the forces and displacements WITHIN each timestep. If things are jumping around use more relaxation of the interface quantities - and visa versa. Biomed case and some of the most difficult since the fluid/solid density ratio is close to 1, but even so you should be able to get convergence in say 10 stagger loops. There's a method for making the interface coupling more implicit by using source terms - cfx support should have those details - that will help a lot.
Lastly, restarts from steady state FSI cases are not straight forward (you need to make a .mf, then edit it and turn on TIMINT). Make sure you aren't getting any jumps in forces or displacements when restarting.

taedeneo September 10, 2009 08:50

it is the nature of FSI simulation since you have to run both solid and fluid equations and also have to run them for many times to get the solution to converged in the coupling sense. Moreover, if your problem have light structure(Huge density ratio, Ms/Mf), you will end up with what so-called "Added mass instability" which will force the use of very small relaxation factors--> huge computational time.

mortazavi September 12, 2009 09:00

i am solving the same fsi case and i have encountered the same problems...first of all you should ramp your boundary condition if it is constant...this will deform the structure slowly in the first itterations and prevent high distortion...tell me more about your inlet and outlet boundary conditions.

All times are GMT -4. The time now is 06:54.