[James113]

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/

[ghorrocks]

Consider remeshing. CFX support has some examples of remeshing inside a run to avoid folding mesh problems.

[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.

[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"

[James113]

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.

[James113]

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

[Lance]

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?

[stumpy]

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.

[James113]

[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]

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

[Lance]

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, [...]".

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?