[hjasak]

Hi All,

I have recently released a top-level solver and tutorial for conjugate heat transfer simulations in OpenFOAM using a new coupled matrix approach. The new classes allow you to create a multi-mesh domain and couple equations on various meshes on a per-variable basis.

For example, in conjugate heat transfer, flow equations are solver only on a fluid mesh, while the energy equation is solved in a coupled manner for the fluid and solid domain at the matrix level.

A code snippet showing how the coupling is achieved is given below:


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();


As a good object-oriented citizen I have implemented the machinery to allow arbitrary multi-mesh and multi-variable coupling: this allows you to tackle any coupled problems involving multiple meshes.

Code:

OpenFOAM-1.4.1-dev/applications/solvers/conjugate/conjugateHeatFoam

Tutorial case:

OpenFOAM-1.4.1-dev/tutorials/conjugateHeatFoam/conjugateCavity + heatedBlock

Enjoy,

Hrv