CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > CFX

FSI and additional variable

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

LinkBack Thread Tools Display Modes
Old   September 10, 2007, 17:16
Default FSI and additional variable
Posts: n/a
Hello, In ANSYS/CFX 11 I'm simulating flow as a result of solid deformation. The deformation repeats itself every second. I then want to simulate the behavior of an additional variable (say a dye in the fluid) for e.g. 30 sec. I now do this by recalculating the same mechanical deformation and fluid velocity every 'cycle' of 1 sec over and over again, the only difference is the additional variable. Is there a way to do this more efficient?

Thanks, Jorn
  Reply With Quote

Old   September 10, 2007, 18:34
Default Re: FSI and additional variable
Glenn Horrocks
Posts: n/a

I can't think of a way of doing it more efficiently than just running it. If the flow is steady state you can turn the flow solver off and just run the additional variable solver but that won't work with a periodic flow like this.

Glenn Horrocks
  Reply With Quote

Old   September 27, 2007, 12:20
Default Re: FSI and additional variable
Stinky Pete
Posts: n/a
Hi Jorn and Glenn,

While you won't be able to get around solving the flow field at each time step, you can get around the FSI and mechanical deformation repetition.

The Ball Valve tutorial (21, I think) is essentially an FSI simulation that is setup entirely within CFX. It is the second part of this tutorial that is relevant. In particular, you can tell CFX to replace the mesh coordinates for all domain nodes using values from data files. This is done using junction box routines, as described in the tutorial.

In your case, I'd recommend the following: * run one cycle with FSI and no dye AV * during that run, use your own junction box routine (i.e. not provided with the noted tutorial) to write a sequence of mesh files. - If you are running in serial, then the JB routine will

be pretty simple. - Model your output based upon the format of the mesh

files provided with the tutorial; you'll be

able to re-use the JB routines provided with the

tutorial when reading the meshes if you do this - Look at the JB routines provided with the tutorial to

find out where the mesh coordinates are stored within

CFX; once you have these data, you just write them to

your mesh files * Now setup your run with the AV, and use the JB routines that are provided with the tutorial to read the meshes in

If, by chance, you're running this in Linux, you'll need to use the Portland Group compiler. There is a note in the CFX installation documentation that highlights how the gnu compiler can not be used with JB routines that involve file I/O.

Hope it helps.
  Reply With Quote


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
Structural force in FSI mapping Fluent 12.0 benjamon FLUENT 1 October 24, 2011 10:32
FSI - Specified Mesh Displacement Vinzent CFX 2 September 17, 2010 07:09
CFX Additional Variable Transport Equation Scott Nordsen CFX 3 January 30, 2010 06:36
Fluid Structure Interaction (FSI) Harendra Siemens 17 February 20, 2005 14:38
How to do FSI using FLUENT? Harendra FLUENT 0 February 5, 2005 02:56

All times are GMT -4. The time now is 08:34.