# FSI Two-Way Problems

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

 January 29, 2009, 00:49 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.

 January 29, 2009, 18:42 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

 January 30, 2009, 01:06 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.

 January 30, 2009, 01:15 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

 January 30, 2009, 01:40 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?

 February 1, 2009, 03:23 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

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

 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 kezman CFX 3 October 3, 2012 16:07 tommymoose ANSYS Meshing & Geometry 0 August 5, 2011 16:02 Mechstud Main CFD Forum 4 July 26, 2011 12:13 woweitukuang CFX 0 April 4, 2009 03:21 abouziar Main CFD Forum 1 May 30, 2008 04:08

All times are GMT -4. The time now is 18:04.