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

Prescribe mesh motion from 2-way FSI

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 28, 2010, 10:01
Default Prescribe mesh motion from 2-way FSI
  #1
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 533
Rep Power: 11
Lance is on a distinguished road
Hi,
I've successfully run a 2-way FSI simulation with a RANS model and now I want to run the same simulation with LES instead. I imagine that LES-FSI would take forever to simulate, so to save some time I was thinking of taking the mesh deformation from the RANS model and prescribe it in the LES model, i.e. doing LES with 1-way FSI (with the assumption that the mesh deformation does not change significantly with turbulence model).
The thing is that I dont really know how to implement it. I guess some user CEL or Fortran is needed...?

So, is is possible to extract each node location at every time step from the RANS and then set it using "Specified Location" for the LES model? If so, does the time step size need to be the same for both simulations, or is it possible to interpolate the mesh location between time steps?

Lance
Lance is offline   Reply With Quote

Old   June 28, 2010, 13:36
Default
  #2
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
LES-FSI does indeed take a while, but it may still be a good option depending on the nature of your case. Firstly, it you are looking at vortex induced vibrations, then you can't use the 1-way assumption in any case. If you run LES-FSI your timestep is likely going to be small already. This means you typically don't need very many stagger/coupling iterations to converge the interface quantities - perhaps 3 at the most, assuming the under-relaxtion factor is 1, as it should be. If your structural mesh is small, then you might be only be looking at a 2x "slow down" compared to the fluids-only LES run. You might also consider explicit coupling (i.e. 1 stagger/coupling iteration per timestep), then you hardly have any slow-down, but it may or may not be stable.
If you do decide to use the approach you describe, then you can export Total Mesh Displacement X|Y|Z from Post for each timestep on the boundary of interest (script this step). You can import those files into CFX-Pre as a Profile Boundary then set your Total Mesh Displacement X|Y|Z equal to the profile boundary functions. That works well for a single profile, but in your case you have one profile per timestep. So I think reading in the profiles via Fortran is the best option, but you can still use the general Profile Boundary mechanism to set the displacements. The other problem is your LES timestep will be less than your RANS timestep, so you won't have enough profiles for the LES run.
stumpy is offline   Reply With Quote

Old   June 29, 2010, 09:56
Default
  #3
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 533
Rep Power: 11
Lance is on a distinguished road
Thanks Stumpy for your input. I will consider the 2-way approach if I cant get the Fortran to work. For the timestep issue, I'll guess I can interpolate between two RANS timesteps to get the coordinates for the LES timestep.

Seems like it's gonna be a couple of weeks of Fortran then...
Lance is offline   Reply With Quote

Old   June 29, 2010, 18:45
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,929
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I remember in CFX V11 the ball valve example used fortran to read in some meshes. That might be a good starting point for you. I think the example was replaced with a purely CEL example in V12 so you will need to get hold of the V11 examples to see it.
ghorrocks is offline   Reply With Quote

Old   July 1, 2010, 03:06
Default
  #5
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 533
Rep Power: 11
Lance is on a distinguished road
Hi Glenn,
yeah, I also remembered that, and it seems to be a good example to start from. Thanks.
Lance 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
Moving mesh part 2 lr103476 OpenFOAM Running, Solving & CFD 49 December 14, 2010 07:20
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
FSI mesh stiffness help realanony87 Main CFD Forum 2 June 21, 2009 15:29
how to extend FSI 2D codes to 3D, need advises abouziar Main CFD Forum 1 May 30, 2008 04:08
large scale mesh motion sb FLUENT 1 April 27, 2007 22:23


All times are GMT -4. The time now is 09:53.