
[Sponsors] 
May 13, 2011, 11:49 
Folded mesh in two way FSI

#1 
New Member
James
Join Date: Apr 2011
Posts: 13
Rep Power: 5 
Hi all,
I am trying to solve a two way FSI Problem in CFX (Ansys 13). First I will explain the CFX problem: Blood simulator flows in an elastic pipe (latex). The elastic pipe is deformed by an external pressure acting on the surface (limitted area). The pressure is a time dependent function  P0*sin(F0*t). Now, to my problem: The CFX is working great on 0.002s timestep, but when I am trying to use a smaller time step (0.001, 0.0004 or 0.0001) , I get a folded mesh error. I tried to use the mesh stiffness function (wall distance and small volume) but nothing really helps. Thanks in advance, James Uploaded with ImageShack.us Uploaded with ImageShack.us Uploaded with ImageShack.us 

May 14, 2011, 06:15 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,442
Rep Power: 76 
Consider remeshing. CFX support has some examples of remeshing inside a run to avoid folding mesh problems.


May 16, 2011, 09:02 

#3 
Senior Member
Join Date: Apr 2009
Posts: 503
Rep Power: 11 
You can't do remeshing with 2way FSI.
Stop the run just before the mesh folds and examine the results. Where and why is it folding? Are the forces sent to ANSYS reasonable? Are the displacements received from ANSYS reasonable given the forces sent? The fact that it works with a larger timestep may suggest your initial conditions are not consistent. Assuming this is a transient run, then are the initial forces sent close to zero? If not, then you should use a steadystate 2way FSI run to establish a good starting point for the transient run. 

May 16, 2011, 09:18 

#4 
Senior Member
Lance
Join Date: Mar 2009
Posts: 480
Rep Power: 10 
I remember from an Ansys FSI Training course that decreasing the time step could give start up problems.
"Half the time step, acceleration increases by a factor of 4" 

May 16, 2011, 16:40 
Thanks for the response

#5  
New Member
James
Join Date: Apr 2011
Posts: 13
Rep Power: 5 
Quote:
Thanks for the response. Are you sure I can't remesh in 2way FSI? I I can't find any reference to this limitation. I will check the rest. 

May 16, 2011, 16:44 

#6  
New Member
James
Join Date: Apr 2011
Posts: 13
Rep Power: 5 
Quote:
Do you refer to the fluid acceleration alone? If so, do you have any advice on this matter? Thanks James 

May 17, 2011, 01:39 

#7 
Senior Member
Lance
Join Date: Mar 2009
Posts: 480
Rep Power: 10 
Say that your wall moves 0.1 mm in 1e4 s => velocity = 1e4 m/1e4 s = 1 m/s => acceleration 1 m/s /1e4 s = 10000 m/s^2
Need an enormous pressure difference to get your fluid to accelerate at that rate. Have you tried a steady twoway as initial condition? 

May 17, 2011, 08:49 

#8 
Senior Member
Join Date: Apr 2009
Posts: 503
Rep Power: 11 
Yes, I'm sure remeshing with 2way FSI is not supported. There's some older threads discussing this on the forum.


May 17, 2011, 13:40 

#9 
New Member
James
Join Date: Apr 2011
Posts: 13
Rep Power: 5 
[QUOTE=Lance;307887]Say that your wall moves 0.1 mm in 1e4 s => velocity = 1e4 m/1e4 s = 1 m/s => acceleration 1 m/s /1e4 s = 10000 m/s^2
Need an enormous pressure difference to get your fluid to accelerate at that rate. Thanks for the quick reponse. How can a steady simulation help me? I have a time dependent force starting from zero (sin function). The fluid's velocity and the structure deformation are zero as well. What is the steadystate problem to be solved? Thanks in advance, James 

May 17, 2011, 13:41 

#10 
New Member
James
Join Date: Apr 2011
Posts: 13
Rep Power: 5 

May 18, 2011, 03:32 

#11  
Senior Member
Lance
Join Date: Mar 2009
Posts: 480
Rep Power: 10 
Quote:
"Mesh adaptation is unavailable for [...], cases with external solver coupling, [...], transient, [...], mesh motion, [...]". Quote:
If a larger time step works, why not start with that and then lower it as the solution progresses? 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
SnappyHexMesh for internal Flow  vishwa  OpenFOAM Native Meshers: snappyHexMesh and Others  23  August 6, 2014 03:50 
3D Hybrid Mesh Errors  DarrenC  ANSYS Meshing & Geometry  11  August 5, 2013 06:42 
[ICEM] Unstructure Meshing Around Imported Plot3D Structured Mesh ICEM  kawamatt2  ANSYS Meshing & Geometry  17  December 20, 2011 11:45 
snappyHexMesh won't work  zeros everywhere!  sc298  OpenFOAM Native Meshers: snappyHexMesh and Others  2  March 27, 2011 21:11 
FSI mesh stiffness help  realanony87  Main CFD Forum  2  June 21, 2009 15:29 