# Folded mesh in two way FSI

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

 May 13, 2011, 11:49 Folded mesh in two way FSI #1 New Member   James Join Date: Apr 2011 Posts: 13 Rep Power: 8 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 time-step, 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 http://imageshack.us/photo/my-images/824/cfxmesh.png/ http://imageshack.us/photo/my-images/851/geom.jpg/ http://imageshack.us/photo/my-images/543/pipei.png/ Last edited by wyldckat; September 3, 2015 at 17:27. Reason: disabled embedded images

 May 14, 2011, 06:15 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,997 Rep Power: 107 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: 532 Rep Power: 14 You can't do remeshing with 2-way 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 steady-state 2-way 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: 615 Rep Power: 15 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: 8
Quote:
 Originally Posted by stumpy You can't do remeshing with 2-way 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 steady-state 2-way FSI run to establish a good starting point for the transient run.
Hi stumpy,
Thanks for the response.
Are you sure I can't remesh in 2-way 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: 8
Quote:
 Originally Posted by Lance 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"
Hi Lance,
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: 615 Rep Power: 15 Say that your wall moves 0.1 mm in 1e-4 s => velocity = 1e-4 m/1e-4 s = 1 m/s => acceleration 1 m/s /1e-4 s = 10000 m/s^2 Need an enormous pressure difference to get your fluid to accelerate at that rate. Have you tried a steady two-way as initial condition?

May 17, 2011, 08:49
#8
Senior Member

Join Date: Apr 2009
Posts: 532
Rep Power: 14
Quote:
 Originally Posted by James113 Hi stumpy, Thanks for the response. Are you sure I can't remesh in 2-way FSI? I I can't find any reference to this limitation. I will check the rest.
Yes, I'm sure re-meshing with 2-way 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: 8 [QUOTE=Lance;307887]Say that your wall moves 0.1 mm in 1e-4 s => velocity = 1e-4 m/1e-4 s = 1 m/s => acceleration 1 m/s /1e-4 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 steady-state 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: 8
Quote:
 Originally Posted by stumpy Yes, I'm sure re-meshing with 2-way FSI is not supported. There's some older threads discussing this on the forum.
I will look it up.
Thank you

May 18, 2011, 03:32
#11
Senior Member

Lance
Join Date: Mar 2009
Posts: 615
Rep Power: 15
Quote:
 Originally Posted by stumpy Yes, I'm sure re-meshing with 2-way FSI is not supported. There's some older threads discussing this on the forum.
Also, if you click the Mesh Refinement button in PRE, there's a text saying:
"Mesh adaptation is unavailable for [...], cases with external solver coupling, [...], transient, [...], mesh motion, [...]".

Quote:
 Originally Posted by James113 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 steady-state problem to be solved? Thanks in advance, James
OK, I've seen people trying to start FSI-simulations with a pressure step (initial conditions = 0, Boundary conditions = 10000 Pa) which might give the solver hard time in the first time step. Thats why I suggested a steady-state solution as a better inital guess. But as your forces already start from zero you should be fine.

If a larger time step works, why not start with that and then lower it as the solution progresses?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post vishwa OpenFOAM Native Meshers: snappyHexMesh and Others 24 June 27, 2016 08:54 DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42 kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 12:45 sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11 realanony87 Main CFD Forum 2 June 21, 2009 15:29

All times are GMT -4. The time now is 14:47.