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

FSI problems

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 30, 2011, 12:33
Default FSI problems
  #1
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 6
lingdeer is on a distinguished road
Hi, I am simulating blood flow through blood vessel and have been facing some problems that I can't reference to in the CFX manual documents.

1) The first time I used coupling convergence of 1e-2, source term of 300 (This is from trial and error until my simulation won't crash). However when I monitor two supposed-to-be symmetric points, it gives me unequal mesh displacement. Also, the solution fail to converge after running for 30 cycles (for each cycle I imposed sinusoidal velocity inflow profile. Outlet I imposed static pressure = 0Pa). Fluid convergence = RMS 1e-5
Therefore, I realize I need to tighten my coupling convergence to lower value to improve convergence.

Now, I changed to coupling convergence to 1e-3, the two monitor points now have equal values. And the mesh displacement waveform of those two points make more sense. Also, since they are at a junction, it will have the biggest displacement in the entire domain. These points are downstream of the flow, so biggest mesh displacement happen later in the cycle. However, when I run with this new coupling convergence, it crashed at the 60th timestep (each cycle time = 1s, time step = 0.01s), which is the point it reaches the biggest mesh displacement and start to retract to its original position.

Since it crash at the middle of the simulation, it's hard to check if it the source term/parameters are good at the beginning of the simulation.

I wonder for anyone who simulate blood flow in blood vessel with CFX can give me some hints on the parameters that I should use to ensure it run smoothly. e.g. what source term do you use? coefficient loop?

2) FSI simulation occupies diskspace. Until it reaches transient convergence (low cycle-to-cycle variation), I don't need results of earlier timestep, but only the last few cycles. So for fluid I know I can delete the previous .trn files to save diskspace. For solid, (.ansys folder), anyone knows how to save space? What files are necessary to keep are what are not (fluid and ansys)?

Thanks Thanks Thanks!
lingdeer is offline   Reply With Quote

Old   November 30, 2011, 12:45
Default
  #2
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 6
lingdeer is on a distinguished road
P.S. the reason of the crash is because of thickness change too big, extreme distortion in the solid solver, which shows at fatal overflow error in the CFX fluid part.
lingdeer is offline   Reply With Quote

Old   November 30, 2011, 16:42
Default
  #3
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
For 1) posting the monitor plots showing force/displacement within each timestep close to the crash would be useful.
For 2) you need to keep all the files while it's running. After the run finishes you can delete the .rst file if you don't want to view the results. You can use MFOU and OUTRES to reduce the frequency and amount of data that is written to the rst file, but you'd need to stop and restart to increase the frequency or data output once you reached the point of interest. Make sure you write at least:
OUTRES,NSOL,LAST
otherwise you won't be able to restart at all.
stumpy is offline   Reply With Quote

Old   December 4, 2011, 18:29
Default
  #4
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 6
lingdeer is on a distinguished road
Thanks Stumpy

1) After it crashed I don't know why I cannot view the monitor points anymore.. Maybe because the .res is not created? (I am running in background so I don't have it opened till it crashed)

2) I have serious trouble with restarting FSI cases.
The ideal case for me is to backup fluid and solid at every timestep instead of coupling step, so I can start at the timestep before something crashed.

I know:
MFOU,10
MFRC,50,1

means writing ANSYS results every 10 time steps
and MFRC will clear the results every 50 time steps and save the new ones again.

The thing is I don't write fluid results every coupling step but every time step instead to save space.

Would the command you suggested write at every time step or every coupling step?

I read from the command reference that 'LAST' means every last substep of each load step. Here is each load step means coupling step or time step?

What if I want to save ANSYS results every time step instead of every coupling step? MFOU and MFRC maybe useful, but what if I am not certain who many coupling steps it would actually run in each time step?

Thanks!
lingdeer is offline   Reply With Quote

Old   December 5, 2011, 12:16
Default
  #5
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
A time step and a coupling step are the same thing. Perhaps you're mixing up coupling iteration with coupling step?
MFOU write data to the rst file, as you said.
MFRC creates backup points and does not remove or add any data from the rst file. A backup point in Mechanical writes data to r001, r002, etc files. If you only keep 1 backup point then you'll only get the r001 file. When restarting data from the rst file is also needed, so when MFRC writes data you have to make sure MFOU is also writing data at the same timestep. So if you want to backup points every timestep you would need:
MFOU,1
MFRC,1,1
then in CFX ask for backup files every timestep. I never use the coupling step frequency options in CFX for reasons I won't get into now. Every timestep is probably a bit excessive, and you might already to too close to failing to have "good' results. Backups every 10 timesteps would be:
MFOU,10 (or 5 or 2 or 1 if you want more frequent data for post-processing)
MFRC,10,1
Then in CFX ask for every 10th timestep.
For FSI a load step = coupling step = time step. So LAST means once per time step, but this gets over-ridden by MFOU.
stumpy is offline   Reply With Quote

Old   December 5, 2011, 14:30
Default
  #6
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 6
lingdeer is on a distinguished road
Worked! Thank you so much!
lingdeer 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
[ICEM] Problems with coedge curves and surfaces tommymoose ANSYS Meshing & Geometry 0 August 5, 2011 16:02
Needed Benchmark Problems for FSI Mechstud Main CFD Forum 4 July 26, 2011 12:13
Problems with circular shapes in FSI simulations kezman ANSYS Meshing & Geometry 1 September 16, 2009 11:24
FSI Two-Way Problems Abduri CFX 6 February 4, 2009 00:41
how to extend FSI 2D codes to 3D, need advises abouziar Main CFD Forum 1 May 30, 2008 04:08


All times are GMT -4. The time now is 21:10.