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

Folded mesh in two way FSI

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 13, 2011, 11:49
Post Folded mesh in two way FSI
  #1
New Member
 
James
Join Date: Apr 2011
Posts: 13
Rep Power: 5
James113 is on a distinguished road
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


Uploaded with ImageShack.us


Uploaded with ImageShack.us


Uploaded with ImageShack.us
James113 is offline   Reply With Quote

Old   May 14, 2011, 06:15
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,442
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Consider remeshing. CFX support has some examples of remeshing inside a run to avoid folding mesh problems.
ghorrocks is offline   Reply With Quote

Old   May 16, 2011, 09:02
Default
  #3
Senior Member
 
Join Date: Apr 2009
Posts: 503
Rep Power: 11
stumpy is on a distinguished road
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.
stumpy is offline   Reply With Quote

Old   May 16, 2011, 09:18
Default
  #4
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 480
Rep Power: 10
Lance is on a distinguished road
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"
Lance is offline   Reply With Quote

Old   May 16, 2011, 16:40
Default Thanks for the response
  #5
New Member
 
James
Join Date: Apr 2011
Posts: 13
Rep Power: 5
James113 is on a distinguished road
Quote:
Originally Posted by stumpy View Post
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.
James113 is offline   Reply With Quote

Old   May 16, 2011, 16:44
Default
  #6
New Member
 
James
Join Date: Apr 2011
Posts: 13
Rep Power: 5
James113 is on a distinguished road
Quote:
Originally Posted by Lance View Post
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
James113 is offline   Reply With Quote

Old   May 17, 2011, 01:39
Default
  #7
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 480
Rep Power: 10
Lance is on a distinguished road
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?
Lance is offline   Reply With Quote

Old   May 17, 2011, 08:49
Default
  #8
Senior Member
 
Join Date: Apr 2009
Posts: 503
Rep Power: 11
stumpy is on a distinguished road
Quote:
Originally Posted by James113 View Post
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.
stumpy is offline   Reply With Quote

Old   May 17, 2011, 13:40
Default
  #9
New Member
 
James
Join Date: Apr 2011
Posts: 13
Rep Power: 5
James113 is on a distinguished road
[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
James113 is offline   Reply With Quote

Old   May 17, 2011, 13:41
Default
  #10
New Member
 
James
Join Date: Apr 2011
Posts: 13
Rep Power: 5
James113 is on a distinguished road
Quote:
Originally Posted by stumpy View Post
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
James113 is offline   Reply With Quote

Old   May 18, 2011, 03:32
Default
  #11
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 480
Rep Power: 10
Lance is on a distinguished road
Quote:
Originally Posted by stumpy View Post
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 View Post

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?
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
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


All times are GMT -4. The time now is 01:57.