CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Examples of implicitly coupled domains

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 15, 2008, 16:44
Default Hello, I am looking for infor
  #1
nadine
Guest
 
Posts: n/a
Hello,
I am looking for information how to solve a model with implicitly coupled domains.

For example, a solid heat transfer model in one half, and an incompressible fluid flow model with heat transport in the other half.

I know that the coupling can be done iteratively, but need want to combine the solutions of both domains into a single equation system to improve the solution quality at the contact interface (the heat transfer is only a simplified example).

Does any such example exist, how to combine the equation systems of different domains? The more trivial the better.

NB
  Reply With Quote

Old   August 15, 2008, 18:09
Default I wrote one of those and it i
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
I wrote one of those and it i currently in the SVN for 1.4.1-dev. Have a look at the code in:

http://openfoam-extend.svn.sourceforge.net/viewvc/openfoam-extend/trunk/Core/Ope nFOAM-1.4.1-dev/applications/solvers/conjugate/conjugateHeatFoam/

The "killer bit" is a build and solution of a block matrix:


coupledFvScalarMatrix TEqns(2);

// Add fluid equation
TEqns.set
(
0,
new fvScalarMatrix
(
fvm::ddt(T)
+ fvm::div(phi, T)
- fvm::laplacian(DT, T)
)
);

// Add solid equation
TEqns.set
(
1,
new fvScalarMatrix
(
fvm::ddt(Tsolid) - fvm::laplacian(DTsolid, Tsolid)
)
);

TEqns.solve();

There is a tutorial in:

http://openfoam-extend.svn.sourceforge.net/viewvc/openfoam-extend/trunk/Core/Ope nFOAM-1.4.1-dev/tutorials/conjugateHeatFoam/

This will all be moved to 1.5-dev soon...

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 15, 2008, 18:40
Default That's the perfect example for
  #3
nadine
Guest
 
Posts: n/a
That's the perfect example for our problem :-)

Just to make sure, does the "TEqns.solve()" really solve the coupled system and not some relaxed iteration of the two equations? The latter was shown to creep to convergence in our scenario, so that I don't want to give it a try.

Thank you!
NB
  Reply With Quote

Old   August 15, 2008, 18:53
Default Yes, it REALLY solves the coup
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
Yes, it REALLY solves the coupled system: eacy solver sweep, each vector-matrix multiply are coupled.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak 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
Sub Domains prakash CFX 4 May 22, 2008 10:43
Sub domains? Chris Wetton CFX 1 February 24, 2008 17:47
Two Domains kdarc OpenFOAM Running, Solving & CFD 1 March 13, 2007 12:08
Did openoam implicitly implement Gamma differencing shceme harry OpenFOAM Running, Solving & CFD 2 February 5, 2007 03:11
The terms that should be treated implicitly in LES ben Main CFD Forum 3 January 28, 2005 04:32


All times are GMT -4. The time now is 17:23.