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

FSI Two-Way Problems

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 29, 2009, 00:49
Default FSI Two-Way Problems
  #1
Abduri
Guest
 
Posts: n/a
How come that my steady-state simulation converges and gives good results but the same mesh does not seem to be sufficient when I turn it into a steady-state FSI Two-Way simulation? The fluid part of the solver does not even reach the 10th accumulated time step altough I use same physical timestep as before.
  Reply With Quote

Old   January 29, 2009, 18:42
Default Re: FSI Two-Way Problems
  #2
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Are you sure the motion is correctly modelled? If the motion is rapid then the mesh motion will cause convergence difficulties.

Glenn Horrocks
  Reply With Quote

Old   January 30, 2009, 01:06
Default Re: FSI Two-Way Problems
  #3
Abduri
Guest
 
Posts: n/a
Hi,

I have run simple but similar problems. I deal with Mach Numbers at about 7 and it all worked fine when the mesh of fluid and solid domain was coarse and simple.

Now I have made it quite complex and maybe solid and fluid domain mesh are slightly overlapping. Can this be a problem?

I also have problems with negative volumes now although the mesh of the fluid domain had no problems when I just did a CFD run.
  Reply With Quote

Old   January 30, 2009, 01:15
Default Re: FSI Two-Way Problems
  #4
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Well that will be your problem. If your mesh is getting negative volume elements then even before then the element quality will be terrible and high mach number flows and poor mesh quality will often lead to convergence problems. You will need to be a bit smarter about your mesh motion. Have a look at the mesh motion weighting functions.

Also have a look at V12 beta as that has lots of remeshing stuff so (I believe, I have not done it) you can monitor mesh quality and trigger a remesh when the quality exceeds a certain value. This type of approach may be useful for you.

Glenn Horrocks
  Reply With Quote

Old   January 30, 2009, 01:40
Default Re: FSI Two-Way Problems
  #5
Abduri
Guest
 
Posts: n/a
Yes. The negative volume appears at elements with very poor quality. I have just checked. When I did a run without FSI with the same mesh it worked. Anyhow: Are there any certain restrictions concerning the mesh of the fluid and solid domain?

Like the nodes have to match between solid and fluid? Or is that independant? Any other things to keep in mind?

By the way: How can I open a mesh file in ANSYS Workbench (Simulation) I created with ANSYS ICEM?
  Reply With Quote

Old   February 1, 2009, 03:23
Default Re: FSI Two-Way Problems
  #6
bornspur
Guest
 
Posts: n/a
Hi Abduri, try reducing Model Exponent for the mesh stiffness model. You can choose either "increase near small volumes" or "increase near boundary" , it doesn't affect much. Try 1 ro the model Exponent. If you look in the CFX manual, you will see the equation showing that if the gradient of the mesh stiffness will be higher when you use high value of model exponent(1 to 10). Imagine you have two adjacent elements, high gradient of mesh stiffness makes one element very stiff compare to the other. This might cause folded mesh in your domain. I normally use 1 but I think in some cases other values may allow larger deformation.

Pat
  Reply With Quote

Old   February 4, 2009, 00:41
Default Re: FSI Two-Way Problems
  #7
Abduri
Guest
 
Posts: n/a
Thank you!! It helped a lot!

Cheers
  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
Problems with circular shapes in FSI simulations kezman CFX 3 October 3, 2012 17:07
[ICEM] Problems with coedge curves and surfaces tommymoose ANSYS Meshing & Geometry 0 August 5, 2011 17:02
Needed Benchmark Problems for FSI Mechstud Main CFD Forum 4 July 26, 2011 13:13
help! FSI problems woweitukuang CFX 0 April 4, 2009 04:21
how to extend FSI 2D codes to 3D, need advises abouziar Main CFD Forum 1 May 30, 2008 05:08


All times are GMT -4. The time now is 17:37.