Loads and executes an OpenFOAM solver modules for each region of a multiregion simulation e.g. for conjugate heat transfer. More...

Detailed Description

Loads and executes an OpenFOAM solver modules for each region of a multiregion simulation e.g. for conjugate heat transfer.

Original source file foamMultiRun.C

The region solvers are specified in the regionSolvers dictionary entry in controlDict, containing a list of pairs of region and solver names, e.g. for a two region case with one fluid region named liquid and one solid region named tubeWall:

    regionSolvers
    {
        liquid          fluid;
        tubeWall        solid;
    }

The regionSolvers entry is a dictionary to support name substitutions to simplify the specification of a single solver type for a set of regions, e.g.

    fluidSolver     fluid;
    solidSolver     solid;

    regionSolvers
    {
        tube1             $fluidSolver;
        tubeWall1         solid;
        tube2             $fluidSolver;
        tubeWall2         solid;
        tube3             $fluidSolver;
        tubeWall3         solid;
    }

Uses the flexible PIMPLE (PISO-SIMPLE) solution for time-resolved and pseudo-transient and steady simulations.

Usage: foamMultiRun [OPTION]

-libs '("lib1.so" ... "libN.so")'
Specify the additional libraries loaded
Example usage:

To update and run a chtMultiRegion case add the following entry to the controlDict:

        regionSolvers
        {
            fluid           fluid;
            solid           solid;
        }

then execute foamMultiRun

Definition in file foamMultiRun.C.