CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

FSI simulation is DEAD SLOW

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 19, 2009, 04:25
Default FSI simulation is DEAD SLOW
  #1
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 466
Rep Power: 10
Lance is on a distinguished road
Hi,
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!
Lance is offline   Reply With Quote

Old   April 29, 2009, 15:25
Default
  #2
New Member
 
Vivek Kumar
Join Date: Mar 2009
Posts: 27
Blog Entries: 1
Rep Power: 7
vivekcfd is on a distinguished road
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.
vivekcfd is offline   Reply With Quote

Old   April 30, 2009, 07:57
Default
  #3
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 466
Rep Power: 10
Lance is on a distinguished road
Hi,
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?
Lance is offline   Reply With Quote

Old   May 1, 2009, 02:18
Default
  #4
New Member
 
Vivek Kumar
Join Date: Mar 2009
Posts: 27
Blog Entries: 1
Rep Power: 7
vivekcfd is on a distinguished road
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).
vivekcfd is offline   Reply With Quote

Old   May 1, 2009, 22:49
Default
  #5
Senior Member
 
Join Date: Apr 2009
Posts: 464
Rep Power: 11
stumpy is on a distinguished road
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.
stumpy is offline   Reply With Quote

Old   September 10, 2009, 08:50
Default
  #6
New Member
 
Join Date: Apr 2009
Posts: 13
Rep Power: 6
taedeneo is on a distinguished road
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.
taedeneo is offline   Reply With Quote

Old   September 12, 2009, 09:00
Default
  #7
New Member
 
Join Date: Jun 2009
Posts: 18
Rep Power: 6
mortazavi is on a distinguished road
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.
mortazavi is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
slow simulation Shuo Main CFD Forum 2 February 28, 2008 19:07
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 22:56
Dead Leg zahid FLUENT 0 September 15, 2003 07:03
Is CFD a dead end? Sebastien Perron Main CFD Forum 17 March 25, 2001 20:00


All times are GMT -4. The time now is 09:40.