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

[hjasak]

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

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

[hjasak]

Yes, it REALLY solves the coupled system: eacy solver sweep, each vector-matrix multiply are coupled.

Hrv