
[Sponsors] 
March 19, 2009, 04:25 
FSI simulation is DEAD SLOW

#1 
Senior Member
Lance
Join Date: Mar 2009
Posts: 606
Rep Power: 14 
Hi,
I'm doing a 2way 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 ansyslicense aa_r ansysinput $inpfile pardist $(hostlist e s, a'*8' $SLURM_NODELIST) startmethod "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 startmethod and parlocal or pardist on the command line, you can move the startmethod switch to after the par*switch. What does this mean? I have startmethod after pardist in the start command. Any suggestions that could solve my problem(s) are highly appreciated! 

April 29, 2009, 15:25 

#2 
Member

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 timesteps (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 steadystate 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. 

April 30, 2009, 07:57 

#3 
Senior Member
Lance
Join Date: Mar 2009
Posts: 606
Rep Power: 14 
Hi,
Yeah, I've tried serial runs and different timesteps. The number of staggers are high, around 70... The initial values comes from a steadystate FSI run. And yes, the ratio between solid and fluid density is very close to 1 (biofluid material...). Any suggestion on what to do? 

May 1, 2009, 02:18 

#4 
Member

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). 

May 1, 2009, 22:49 

#5 
Senior Member
Join Date: Apr 2009
Posts: 532
Rep Power: 14 
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. 

September 10, 2009, 08:50 

#6 
New Member
Join Date: Apr 2009
Posts: 13
Rep Power: 10 
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 socalled "Added mass instability" which will force the use of very small relaxation factors> huge computational time.


September 12, 2009, 09:00 

#7 
Member
Join Date: Jun 2009
Posts: 53
Rep Power: 10 
hi:
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. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
slow simulation  Shuo  Main CFD Forum  2  February 28, 2008 20:07 
Ultra slow convergence velocity in the simulation  demigod  FLUENT  1  October 5, 2005 08:03 
EXA dead ?  CFD_user  Main CFD Forum  2  February 1, 2005 23:56 
Dead Leg  zahid  FLUENT  0  September 15, 2003 07:03 
Is CFD a dead end?  Sebastien Perron  Main CFD Forum  17  March 25, 2001 21:00 