chtMultiRegionFoam: SIMPLE operation and transonic switch

Multi-region PIMPLE controls have been applied to the chtMultiRegionFoam
solver, and a transonic option has been implemented.

The new PIMPLE controls let the solver operate SIMPLE mode. The
utilisation of library solution and convergence control functionality
has significantly reduced the amount of code in the solver. The
chtMultiRegionSimpleFoam solver has also been made obsolete, and has
therefore been removed.

A few changes will be necessary to convert an existing
chtMultiRegionSimpleFoam case to chtMultiRegionFoam. All the SIMPLE
sub-dictionaries in the system/<regions>/fvSolution will need to be
renamed PIMPLE. The system/fvSolution file will also need an empty
PIMPLE sub-dictionary. In addition, additional "<variable>Final" solver
and relaxation entries will be needed. For a steady case, adding a
wildcard ending, ".*", to the variable names should be sufficient.

Solution parameters appropriate for a steady case are shown below:

    solvers
    {
        "p_rgh.*"
        {
            solver           GAMG;
            tolerance        1e-7;
            relTol           0.01;
            smoother         DIC;
            maxIter          10;
        }

        "(U|h|e|k|epsilon).*"
        {
            solver           PBiCGStab;
            preconditioner   DILU;
            tolerance        1e-7;
            relTol           0.1;
        }
    }

    PIMPLE
    {
        // ...
    }

    relaxationFactors
    {
        fields
        {
            "p_rgh.*"       0.7;
        }
        equations
        {
            "U.*"           0.5;
            "(h|e).*"       0.3;
            "(k|epsilon).*" 0.2;
        }
    }

This work was supported by Fabian Buelow, at Evonik
Tobias Holzmann provided cases for testing the convergence controls

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/air/T

@@ -0,0 +1,46 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 0 0 1 0 0 0];
+
+internalField   uniform 300;
+
+boundaryField
+{
+    walls
+    {
+        type            zeroGradient;
+    }
+    inlet
+    {
+        type            fixedValue;
+        value           uniform 300;
+    }
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform 300;
+        value           uniform 300;
+    }
+    blades
+    {
+        type            zeroGradient;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/air/U

@@ -0,0 +1,50 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volVectorField;
+    location    "0";
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0 0 0);
+
+boundaryField
+{
+    walls
+    {
+        type            noSlip;
+    }
+
+    inlet
+    {
+        type            fixedValue;
+        value           uniform (0 0 5);
+    }
+
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform (0 0 0);
+        value           uniform (0 0 0);
+    }
+
+    blades
+    {
+        type            fixedValue;
+        value           uniform (0 0 0);
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/air/alphat

@@ -0,0 +1,47 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0/air";
+    object      alphat;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -1 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    walls
+    {
+        type            compressible::alphatWallFunction;
+        value           uniform 0;
+    }
+    inlet
+    {
+        type            calculated;
+        value           uniform 0;
+    }
+    outlet
+    {
+        type            calculated;
+        value           uniform 0;
+    }
+    blades
+    {
+        type            compressible::alphatWallFunction;
+        value           uniform 0;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/air/epsilon

@@ -0,0 +1,46 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      epsilon;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -3 0 0 0 0];
+
+internalField   uniform 0.54;
+
+boundaryField
+{
+    walls
+    {
+        type            epsilonWallFunction;
+        value           $internalField;
+    }
+    inlet
+    {
+        type            fixedValue;
+        value           $internalField;
+    }
+    outlet
+    {
+        type            zeroGradient;
+    }
+    blades
+    {
+        type            epsilonWallFunction;
+        value           $internalField;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/air/k

@@ -0,0 +1,46 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -2 0 0 0 0];
+
+internalField   uniform 0.375;
+
+boundaryField
+{
+    walls
+    {
+        type            kqRWallFunction;
+        value           $internalField;
+    }
+    inlet
+    {
+        type            fixedValue;
+        value           $internalField;
+    }
+    outlet
+    {
+        type            zeroGradient;
+    }
+    blades
+    {
+        type            kqRWallFunction;
+        value           $internalField;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/air/nut

@@ -0,0 +1,47 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0/air";
+    object      nut;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -1 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    walls
+    {
+        type            nutkWallFunction;
+        value           uniform 0;
+    }
+    inlet
+    {
+        type            calculated;
+        value           uniform 0;
+    }
+    outlet
+    {
+        type            calculated;
+        value           uniform 0;
+    }
+    blades
+    {
+        type            nutkWallFunction;
+        value           uniform 0;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/air/p

@@ -0,0 +1,47 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 100000;
+
+boundaryField
+{
+    walls
+    {
+        type            calculated;
+        value           uniform 100000;
+    }
+    inlet
+    {
+        type            calculated;
+        value           uniform 100000;
+    }
+    outlet
+    {
+        type            calculated;
+        value           uniform 100000;
+    }
+    blades
+    {
+        type            calculated;
+        value           uniform 100000;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/air/p_rgh

@@ -0,0 +1,44 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 100000;
+
+boundaryField
+{
+    walls
+    {
+        type            fixedFluxPressure;
+    }
+    inlet
+    {
+        type            fixedFluxPressure;
+    }
+    outlet
+    {
+        type            fixedValue;
+        value           $internalField;
+    }
+    blades
+    {
+        type            fixedFluxPressure;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/porous/AoV

@@ -0,0 +1,31 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      AoV;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 -1 0 0 0 0 0];
+
+internalField   uniform 200;
+
+boundaryField
+{
+    ".*"
+    {
+        type            zeroGradient;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/porous/T

@@ -0,0 +1,42 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 0 0 1 0 0 0];
+
+internalField   uniform 350;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform 400;
+    }
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform 350;
+        value           uniform 350;
+    }
+    fixedWalls
+    {
+        type            zeroGradient;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/porous/U

@@ -0,0 +1,42 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volVectorField;
+    location    "0";
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0.01 0 0);
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform (0.01 0 0);
+    }
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform (0 0 0);
+        value           uniform (0 0 0);
+    }
+    fixedWalls
+    {
+        type            noSlip;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/porous/htcConst

@@ -0,0 +1,31 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      htcConst;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 0 -3 -1 0 0 0];
+
+internalField   uniform 10;
+
+boundaryField
+{
+    ".*"
+    {
+        type            zeroGradient;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/porous/p

@@ -0,0 +1,42 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 100000;
+
+boundaryField
+{
+    inlet
+    {
+        type            calculated;
+        value           uniform 100000;
+    }
+    outlet
+    {
+        type            calculated;
+        value           uniform 100000;
+    }
+    fixedWalls
+    {
+        type            calculated;
+        value           uniform 100000;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/0.orig/porous/p_rgh

@@ -0,0 +1,40 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 100000;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedFluxPressure;
+    }
+    outlet
+    {
+        type            fixedValue;
+        value           uniform 100000;
+    }
+    fixedWalls
+    {
+        type            fixedFluxPressure;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/Allclean

@@ -0,0 +1,15 @@
+#!/bin/sh
+
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+cleanCase
+
+foamCleanPolyMesh -region air
+foamCleanPolyMesh -region porous
+
+rm -f *.OpenFOAM
+
+rm -rf 0

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/Allrun

@@ -0,0 +1,10 @@
+#!/bin/sh
+
+cd ${0%/*} || exit 1    # Run from this directory
+
+./Allrun.pre
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+runApplication $(getApplication)

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/Allrun-parallel

@@ -0,0 +1,16 @@
+#!/bin/sh
+
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+./Allrun.pre
+
+runApplication -s air    decomposePar -region air
+runApplication -s porous decomposePar -region porous
+
+runParallel $(getApplication)
+
+runApplication -s air    reconstructPar -latestTime -region air
+runApplication -s porous reconstructPar -latestTime -region porous

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/Allrun.pre

@@ -0,0 +1,29 @@
+#!/bin/sh
+
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+#create meshes
+runApplication -s air    blockMesh -region air
+runApplication -s porous blockMesh -region porous
+
+# create rotor blades in air region
+runApplication -s air.1 \
+    topoSet -region air -dict system/topoSetDict.1
+
+runApplication createBaffles -region air -overwrite
+
+# create rotor zone in air region for MRF
+runApplication -s air.2 \
+    topoSet -region air -dict system/topoSetDict.2
+
+rm -rf constant/air/polyMesh/sets
+
+# create dummy files for post-processing
+paraFoam -touch -region porous
+paraFoam -touch -region air
+
+
+cp -rf 0.orig 0

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/air/MRFProperties

@@ -0,0 +1,32 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      MRFProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+MRF1
+{
+    cellZone    rotor;
+    active      yes;
+
+    // Fixed patches (by default they 'move' with the MRF zone)
+    nonRotatingPatches ();
+
+    origin    (0.25 0.25 0.25);
+    axis      (0 0 1);
+    omega     47.7; // 50 rpm
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/air/fvOptions

@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      fvOptions;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+airToporous
+{
+    type            constantHeatTransfer;
+
+    interpolationMethod cellVolumeWeight;
+    nbrRegionName   porous;
+    master          false;
+
+    nbrModel        porousToair;
+    fields          (h);
+    semiImplicit    no;
+}
+
+porosityBlockage
+{
+    type            interRegionExplicitPorositySource;
+
+    interRegionExplicitPorositySourceCoeffs
+    {
+        interpolationMethod cellVolumeWeight;
+        nbrRegionName   porous;
+
+        type            DarcyForchheimer;
+
+        d   (-1000 -1000 1e4);
+        f   (0 0 0);
+
+        coordinateSystem
+        {
+            type    cartesian;
+            origin  (0 0 0);
+            coordinateRotation
+            {
+                type    axesRotation;
+                e1      (0 1 0);
+                e2      (0 0 1);
+            }
+        }
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/air/g

@@ -0,0 +1,23 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       uniformDimensionedVectorField;
+    location    "constant";
+    object      g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -2 0 0 0 0];
+//value           ( 0 0 9.81);
+value           ( 0 0 0);
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/air/radiationProperties

@@ -0,0 +1,25 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      radiationProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+radiation       off;
+
+radiationModel  none;
+
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/air/thermophysicalProperties

@@ -0,0 +1,54 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      thermophysicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            heRhoThermo;
+    mixture         pureMixture;
+    transport       polynomial;
+    thermo          hPolynomial;
+    equationOfState icoPolynomial;
+    specie          specie;
+    energy          sensibleEnthalpy;
+}
+
+mixture
+{
+    // coefficients for air
+
+    specie
+    {
+        molWeight       28.85;
+    }
+    equationOfState
+    {
+        rhoCoeffs<8>    ( 4.0097 -0.016954 3.3057e-05 -3.0042e-08 1.0286e-11 0 0 0 );
+    }
+    thermodynamics
+    {
+        Hf              0;
+        Sf              0;
+        CpCoeffs<8>     ( 948.76 0.39171 -0.00095999 1.393e-06 -6.2029e-10 0 0 0 );
+    }
+    transport
+    {
+        muCoeffs<8>     ( 1.5061e-06 6.16e-08 -1.819e-11 0 0 0 0 0 );
+        kappaCoeffs<8>  ( 0.0025219 8.506e-05 -1.312e-08 0 0 0 0 0 );
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/air/turbulenceProperties

@@ -0,0 +1,30 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType  RAS;
+
+RAS
+{
+    RASModel        kEpsilon;
+
+    turbulence      on;
+
+    printCoeffs     on;
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/porous/fvOptions

@@ -0,0 +1,32 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      fvOptions;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+porousToair
+{
+    type            constantHeatTransfer;
+
+    interpolationMethod cellVolumeWeight;
+    nbrRegionName   air;
+    master          true;
+
+    nbrModel        airToporous;
+    fields          (h);
+    semiImplicit    no;
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/porous/g

@@ -0,0 +1,23 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       uniformDimensionedVectorField;
+    location    "constant";
+    object      g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -2 0 0 0 0];
+//value           ( 0 0 9.81);
+value           ( 0 0 0);
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/porous/thermophysicalProperties

@@ -0,0 +1,54 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      thermophysicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            heRhoThermo;
+    mixture         pureMixture;
+    transport       polynomial;
+    thermo          hPolynomial;
+    equationOfState icoPolynomial;
+    specie          specie;
+    energy          sensibleEnthalpy;
+}
+
+
+mixture
+{
+    // coefficients for water
+
+    specie
+    {
+        molWeight       18;
+    }
+    equationOfState
+    {
+        rhoCoeffs<8>    ( 1000 0 0 0 0 0 0 0 );
+    }
+    thermodynamics
+    {
+        Hf              0;
+        Sf              0;
+        CpCoeffs<8>     ( 4183 0 0 0 0 0 0 0 );
+    }
+    transport
+    {
+        muCoeffs<8>     ( 0.001 0 0 0 0 0 0 0 );
+        kappaCoeffs<8>  ( 0.58  0 0 0 0 0 0 0 );
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/porous/turbulenceProperties

@@ -0,0 +1,19 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType  laminar;
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/constant/regionProperties

@@ -0,0 +1,24 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      regionProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+regions
+(
+    fluid   (air porous)
+    solid   ()
+);
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/air/blockMeshDict

@@ -0,0 +1,149 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 0.05;
+
+vertices
+(
+    (0 0 0)             // 0
+    (10 0 0)            // 1
+    (10 10 0)           // 2
+    (0 10 0)            // 3
+
+    (2.879 2.879 0)     // 4
+    (7.121 2.879 0)     // 5
+    (7.121 7.121 0)     // 6
+    (2.879 7.121 0)     // 7
+
+    (4.293 4.293 0)     // 8
+    (5.707 4.293 0)     // 9
+    (5.707 5.707 0)     // 10
+    (4.293 5.707 0)     // 11
+
+
+    (0 0 10)            // 12
+    (10 0 10)           // 13
+    (10 10 10)          // 14
+    (0 10 10)           // 15
+
+    (2.879 2.879 10)    // 16
+    (7.121 2.879 10)    // 17
+    (7.121 7.121 10)    // 18
+    (2.879 7.121 10)    // 19
+
+    (4.293 4.293 10)    // 20
+    (5.707 4.293 10)    // 20
+    (5.707 5.707 10)    // 22
+    (4.293 5.707 10)    // 23
+);
+
+blocks
+(
+    hex (0 1  5  4 12 13 17 16) (30 30 30) simpleGrading (1 1 1)
+    hex (1 2  6  5 13 14 18 17) (30 30 30) simpleGrading (1 1 1)
+    hex (2 3  7  6 14 15 19 18) (30 30 30) simpleGrading (1 1 1)
+    hex (3 0  4  7 15 12 16 19) (30 30 30) simpleGrading (1 1 1)
+    hex (4 5  9  8 16 17 21 20) cylinder (30 30 30) simpleGrading (1 1 1)
+    hex (5 6 10  9 17 18 22 21) cylinder (30 30 30) simpleGrading (1 1 1)
+    hex (6 7 11 10 18 19 23 22) cylinder (30 30 30) simpleGrading (1 1 1)
+    hex (7 4  8 11 19 16 20 23) cylinder (30 30 30) simpleGrading (1 1 1)
+    hex (8 9 10 11 20 21 22 23) innerCylinder (30 30 30) simpleGrading (1 1 1)
+);
+
+edges
+(
+    arc 4 5 (5 2 0)
+    arc 5 6 (8 5 0)
+    arc 6 7 (5 8 0)
+    arc 7 4 (2 5 0)
+
+    arc 8 9 (5 4 0)
+    arc 9 10 (6 5 0)
+    arc 10 11 (5 6 0)
+    arc 11 8 (4 5 0)
+
+    arc 16 17 (5 2 10)
+    arc 17 18 (8 5 10)
+    arc 18 19 (5 8 10)
+    arc 19 16 (2 5 10)
+
+    arc 20 21 (5 4 10)
+    arc 21 22 (6 5 10)
+    arc 22 23 (5 6 10)
+    arc 23 20 (4 5 10)
+);
+
+boundary
+(
+    walls
+    {
+        type wall;
+        faces
+        (
+            (0 4 5 1)
+            (1 5 6 2)
+            (2 6 7 3)
+            (3 7 4 0)
+
+            (12 13 17 16)
+            (13 14 18 17)
+            (14 15 19 18)
+            (15 12 16 19)
+
+            (0 12 13 1)
+            (1 13 14 2)
+            (2 14 15 3)
+            (3 15 12 0)
+        );
+    }
+    inlet
+    {
+        type patch;
+        faces
+        (
+            (4 8 9 5)
+            (5 9 10 6)
+            (6 10 11 7)
+            (7 11 8 4)
+            (8 11 10 9)
+        );
+    }
+    outlet
+    {
+        type patch;
+        faces
+        (
+            (16 17 21 20)
+            (17 18 22 21)
+            (18 19 23 22)
+            (19 16 20 23)
+            (20 21 22 23)
+        );
+    }
+
+    blades
+    {
+        type wall;
+        faces
+        ();
+    }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/air/createBafflesDict

@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      createBafflesDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+// Whether to convert internal faces only (so leave boundary faces intact).
+// This is only relevant if your face selection type can pick up boundary
+// faces.
+internalFacesOnly true;
+
+
+// Baffles to create.
+baffles
+{
+    baffleFaces
+    {
+        //- Use predefined faceZone to select faces and orientation.
+        type        faceZone;
+        zoneName    rotorBlades;
+
+
+        patches
+        {
+            master
+            {
+                //- Master side patch
+                name            blades;
+                type            patch;
+            }
+            slave
+            {
+                //- Slave side patch
+                name            blades;
+                type            patch;
+            }
+        }
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/air/decomposeParDict

@@ -0,0 +1,45 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 4;
+
+method          scotch;
+
+simpleCoeffs
+{
+    n               (2 2 1);
+    delta           0.001;
+}
+
+hierarchicalCoeffs
+{
+    n               (1 1 1);
+    delta           0.001;
+    order           xyz;
+}
+
+manualCoeffs
+{
+    dataFile        "";
+}
+
+distributed     no;
+
+roots           ( );
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/air/fvSchemes

@@ -0,0 +1,57 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default         steadyState;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+    grad(U)         cellLimited Gauss linear 1;
+}
+
+divSchemes
+{
+    default         none;
+    div(phi,U)      bounded Gauss upwind;
+    div(phi,h)      bounded Gauss upwind;
+    div(phi,e)      bounded Gauss upwind;
+    div(phi,K)      bounded Gauss upwind;
+    div(phi,k)      bounded Gauss upwind;
+    div(phi,epsilon) bounded Gauss upwind;
+    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear limited corrected 0.33;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         limited corrected 0.33;
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/air/fvSolution

@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system/air";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "p_rgh.*"
+    {
+        solver           GAMG;
+        tolerance        1e-7;
+        relTol           0.01;
+        smoother         DIC;
+        maxIter          100;
+    }
+
+    "(U|h|e|k|epsilon).*"
+    {
+        solver           PBiCGStab;
+        preconditioner   DILU;
+        tolerance        1e-6;
+        relTol           0.1;
+    }
+}
+
+PIMPLE
+{
+    nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+    fields
+    {
+        "rho.*"         1;
+        "p_rgh.*"       0.7;
+    }
+    equations
+    {
+        "U.*"           0.3;
+        "(h|e).*"       0.3;
+        "k.*"           0.3;
+        "epsilon.*"     0.3;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/air/topoSetDict.1

@@ -0,0 +1,120 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      topoSetDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+actions
+(
+    // rotor faces
+    {
+        name    rotorCells;
+        type    cellSet;
+        action  new;
+        source  zoneToCell;
+        sourceInfo
+        {
+            name    cylinder;
+        }
+    }
+    {
+        name    rotorFaces;
+        type    faceSet;
+        action  new;
+        source  cellToFace;
+        sourceInfo
+        {
+            set     rotorCells;
+            option  all;
+        }
+    }
+    {
+        name    rotorFaces;
+        type    faceSet;
+        action  subset;
+        source  boxToFace;
+        sourceInfo
+        {
+            box (-100 -100 0.1) (100 100 0.15);
+        }
+    }
+
+    {
+        name    rotorBladesFaceSet;
+        type    faceSet;
+        action  new;
+        source  faceToFace;
+        sourceInfo
+        {
+            set     rotorFaces;
+        }
+    }
+
+    {
+        name    rotorBladesFaceSet;
+        type    faceSet;
+        action  subset;
+        source  boxToFace;
+        sourceInfo
+        {
+            box (-100 0.249 -100) (100 0.251 100);
+        }
+    }
+
+    {
+        name    rotorBlades2;
+        type    faceSet;
+        action  new;
+        source  faceToFace;
+        sourceInfo
+        {
+            set     rotorFaces;
+        }
+    }
+
+    {
+        name    rotorBlades2;
+        type    faceSet;
+        action  subset;
+        source  boxToFace;
+        sourceInfo
+        {
+            box (0.249 -100 -100) (0.251 100 100);
+        }
+    }
+
+    {
+        name    rotorBladesFaceSet;
+        type    faceSet;
+        action  add;
+        source  faceToFace;
+        sourceInfo
+        {
+            set     rotorBlades2;
+        }
+    }
+    {
+        name    rotorBlades;
+        type    faceZoneSet;
+        action  new;
+        source  setToFaceZone;
+        sourceInfo
+        {
+            faceSet rotorBladesFaceSet;
+        }
+    }
+);
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/air/topoSetDict.2

@@ -0,0 +1,64 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      topoSetDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+actions
+(
+    // rotor cell zone
+    {
+        name    rotorCells;
+        type    cellSet;
+        action  new;
+        source  zoneToCell;
+        sourceInfo
+        {
+            name    cylinder;
+        }
+    }
+    {
+        name    rotorCells;
+        type    cellSet;
+        action  add;
+        source  zoneToCell;
+        sourceInfo
+        {
+            name    innerCylinder;
+        }
+    }
+    {
+        name    rotorCells;
+        type    cellSet;
+        action  subset;
+        source  boxToCell;
+        sourceInfo
+        {
+            box (-100 -100 0.1) (100 100 0.15);
+        }
+    }
+    {
+        name    rotor;
+        type    cellZoneSet;
+        action  new;
+        source  setToCellZone;
+        sourceInfo
+        {
+            set rotorCells;
+        }
+    }
+);
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/controlDict

@@ -0,0 +1,49 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application     chtMultiRegionFoam;
+
+startFrom       latestTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         2000;
+
+deltaT          1;
+
+writeControl    timeStep;
+
+writeInterval   50;
+
+purgeWrite      0;
+
+writeFormat     ascii;
+
+writePrecision  6;
+
+writeCompression off;
+
+timeFormat      general;
+
+timePrecision   6;
+
+runTimeModifiable true;
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/decomposeParDict

@@ -0,0 +1,45 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 4;
+
+method          scotch;
+
+simpleCoeffs
+{
+    n               (2 2 1);
+    delta           0.001;
+}
+
+hierarchicalCoeffs
+{
+    n               (1 1 1);
+    delta           0.001;
+    order           xyz;
+}
+
+manualCoeffs
+{
+    dataFile        "";
+}
+
+distributed     no;
+
+roots           ( );
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/fvSchemes

@@ -0,0 +1,42 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+}
+
+gradSchemes
+{
+}
+
+divSchemes
+{
+}
+
+laplacianSchemes
+{
+}
+
+interpolationSchemes
+{
+}
+
+snGradSchemes
+{
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/fvSolution

@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+PIMPLE
+{
+    nOuterCorrectors 1;
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/porous/blockMeshDict

@@ -0,0 +1,76 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 0.05;
+
+vertices
+(
+    (-2 2 6)     // 0
+    (12 2 6)     // 1
+    (12 8 6)     // 2
+    (-2 8 6)     // 3
+
+    (-2 2 7)     // 4
+    (12 2 7)     // 5
+    (12 8 7)     // 6
+    (-2 8 7)     // 7
+);
+
+blocks
+(
+    hex (0 1 2 3 4 5 6 7) (40 30 30) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+    inlet
+    {
+        type patch;
+        faces
+        (
+            (0 4 7 3)
+        );
+    }
+    outlet
+    {
+        type patch;
+        faces
+        (
+            (1 2 6 5)
+        );
+    }
+    fixedWalls
+    {
+        type wall;
+        faces
+        (
+            (0 1 2 3)
+            (4 5 6 7)
+            (3 2 6 7)
+            (0 1 5 4)
+        );
+    }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/porous/decomposeParDict

@@ -0,0 +1,45 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 4;
+
+method          simple;
+
+simpleCoeffs
+{
+    n               (2 2 1);
+    delta           0.001;
+}
+
+hierarchicalCoeffs
+{
+    n               (1 1 1);
+    delta           0.001;
+    order           xyz;
+}
+
+manualCoeffs
+{
+    dataFile        "";
+}
+
+distributed     no;
+
+roots           ( );
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/porous/fvSchemes

@@ -0,0 +1,55 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default         steadyState;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+    div(phi,U)      bounded Gauss upwind;
+    div(phi,h)      bounded Gauss upwind;
+    div(phi,e)      bounded Gauss upwind;
+    div(phi,Ekp)    bounded Gauss upwind;
+    div(phi,K)      bounded Gauss upwind;
+    div(phi,k)      bounded Gauss upwind;
+    div(phi,epsilon) bounded Gauss upwind;
+    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear uncorrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         uncorrected;
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/heatExchanger/system/porous/fvSolution

@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system/porous";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "p_rgh.*"
+    {
+        solver           GAMG;
+        tolerance        1e-7;
+        relTol           0.01;
+        smoother         DIC;
+        maxIter          10;
+    }
+
+    "(U|h|e|k|epsilon).*"
+    {
+        solver           PBiCGStab;
+        preconditioner   DILU;
+        tolerance        1e-7;
+        relTol           0.1;
+    }
+}
+
+PIMPLE
+{
+    nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+    fields
+    {
+        "rho.*"         1;
+        "p_rgh.*"       0.7;
+    }
+    equations
+    {
+        "U.*"           0.3;
+        "(h|e).*"       0.3;
+        "k.*"           0.3;
+        "epsilon.*"     0.3;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/0/G

@@ -0,0 +1,30 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      G;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 0 -3 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    ".*"
+    {
+        type            calculated;
+        value           $internalField;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/0/IDefault

@@ -0,0 +1,30 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      IDefault;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 0 -3 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    ".*"
+    {
+        type            calculated;
+        value           $internalField;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/0/T

@@ -0,0 +1,30 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 0 0 1 0 0 0];
+
+internalField   uniform 300;
+
+boundaryField
+{
+    ".*"
+    {
+        type            calculated;
+        value           $internalField;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/0/U

@@ -0,0 +1,30 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volVectorField;
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0.1 0 0);
+
+boundaryField
+{
+    ".*"
+    {
+        type            calculated;
+        value           $internalField;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/0/epsilon

@@ -0,0 +1,31 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      epsilon;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -3 0 0 0 0];
+
+internalField   uniform 0.01;
+
+boundaryField
+{
+    ".*"
+    {
+        type            calculated;
+        value           $internalField;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/0/k

@@ -0,0 +1,31 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -2 0 0 0 0];
+
+internalField   uniform 0.1;
+
+boundaryField
+{
+    ".*"
+    {
+        type            calculated;
+        value           $internalField;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/0/p

@@ -0,0 +1,30 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 1e5;
+
+boundaryField
+{
+    ".*"
+    {
+        type            calculated;
+        value           $internalField;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/0/p_rgh

@@ -0,0 +1,30 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 1e5;
+
+boundaryField
+{
+    ".*"
+    {
+        type            calculated;
+        value           $internalField;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/0/qr

@@ -0,0 +1,30 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      qr;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 0 -3 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    ".*"
+    {
+        type            calculated;
+        value           $internalField;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/Allclean

@@ -0,0 +1,35 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial clean functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+cleanCase
+rm -rf VTK
+rm -rf constant/cellToRegion constant/polyMesh/sets
+rm -rf 0/bottomAir
+rm -rf 0/topAir
+rm -rf 0/heater
+rm -rf 0/leftSolid
+rm -rf 0/rightSolid
+rm -f 0/cellToRegion
+
+rm -rf constant/bottomAir/polyMesh
+rm -rf constant/topAir/polyMesh
+rm -rf constant/heater/polyMesh
+rm -rf constant/leftSolid/polyMesh
+rm -rf constant/rightSolid/polyMesh
+
+rm -f constant/bottomAir/F
+rm -f constant/bottomAir/constructMap*
+rm -f constant/bottomAir/finalAgglom
+rm -f constant/bottomAir/globalFaceFaces
+rm -f constant/bottomAir/subMap
+
+rm -f constant/topAir/F
+rm -f constant/topAir/constructMap*
+rm -f constant/topAir/finalAgglom
+rm -f constant/topAir/globalFaceFaces
+rm -f constant/topAir/subMap
+
+#------------------------------------------------------------------------------

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/Allrun

@@ -0,0 +1,38 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+
+# Setup case
+./Allrun.pre
+
+
+#-- Run on single processor
+
+# Agglomerate patch faces
+for i in bottomAir topAir
+do
+    runApplication -s $i \
+        faceAgglomerate -region $i -dict constant/viewFactorsDict
+done
+
+# Generate view factors
+for i in bottomAir topAir
+do
+    runApplication -s $i \
+        viewFactorsGen -region $i
+done
+
+runApplication `getApplication`
+
+
+
+echo
+echo "creating files for paraview post-processing"
+echo
+paraFoam -touchAll
+
+#------------------------------------------------------------------------------

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/Allrun-parallel

@@ -0,0 +1,45 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+
+# Setup case
+./Allrun.pre
+
+
+#-- Run in parallel
+
+# Decompose
+runApplication decomposePar -allRegions
+
+# Agglomerate patch faces
+for i in bottomAir topAir
+do
+    runParallel -s $i -np 4 \
+        faceAgglomerate -region $i -dict constant/viewFactorsDict
+done
+
+# Generate view factors
+for i in bottomAir topAir
+do
+    runParallel -s $i -np 4 \
+        viewFactorsGen -region $i
+done
+
+# Run
+runParallel `getApplication`
+
+# Reconstruct
+runApplication reconstructPar -allRegions
+
+
+
+echo
+echo "creating files for paraview post-processing"
+echo
+paraFoam -touchAll
+
+#------------------------------------------------------------------------------

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/Allrun.pre

@@ -0,0 +1,24 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+runApplication blockMesh
+runApplication topoSet
+runApplication splitMeshRegions -cellZones -overwrite
+
+# remove fluid fields from solid regions (important for post-processing)
+for i in heater leftSolid rightSolid
+do
+   rm -f 0*/$i/{rho,nut,alphat,epsilon,k,U,p_rgh,qr,G,IDefault}
+done
+
+for i in bottomAir topAir heater leftSolid rightSolid
+do
+    runApplication -s $i  changeDictionary -region $i
+done
+
+
+#------------------------------------------------------------------------------

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/bottomAir/g

@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       uniformDimensionedVectorField;
+    object      g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -2 0 0 0 0];
+value           (0 -9.81 0);
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/bottomAir/radiationProperties

@@ -0,0 +1,45 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      radiationProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+radiation       on;
+
+radiationModel  viewFactor;
+
+viewFactorCoeffs
+{
+    smoothing true; //Smooth view factor matrix (use when in a close surface
+                    //to force Sum(Fij = 1)
+    constantEmissivity true; //constant emissivity on surfaces.
+}
+
+// Number of flow iterations per radiation iteration
+solverFreq 3;
+
+absorptionEmissionModel constantAbsorptionEmission;
+
+constantAbsorptionEmissionCoeffs
+{
+    absorptivity    absorptivity    [0 -1 0 0 0 0 0] 0.01;
+    emissivity      emissivity      [0 -1 0 0 0 0 0] 0.01;
+    E               E               [1 -1 -3 0 0 0 0] 0;
+}
+
+scatterModel    none;
+
+sootModel       none;
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/bottomAir/thermophysicalProperties

@@ -0,0 +1,48 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant/bottomAir";
+    object      thermophysicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            heRhoThermo;
+    mixture         pureMixture;
+    transport       const;
+    thermo          hConst;
+    equationOfState perfectGas;
+    specie          specie;
+    energy          sensibleEnthalpy;
+}
+
+mixture
+{
+    specie
+    {
+        molWeight       28.9;
+    }
+    thermodynamics
+    {
+        Cp              1000;
+        Hf              0;
+    }
+    transport
+    {
+        mu              1.8e-05;
+        Pr              0.7;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/bottomAir/turbulenceProperties

@@ -0,0 +1,19 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType  laminar;
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/bottomAir/viewFactorsDict

@@ -0,0 +1,70 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      viewFactorsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+writeViewFactorMatrix     true;
+writeFacesAgglomeration   true;
+writePatchViewFactors     false;
+
+bottomAir_to_heater
+{
+    nFacesInCoarsestLevel     30;
+    featureAngle              10;
+}
+
+bottomAir_to_leftSolid
+{
+    nFacesInCoarsestLevel     20;
+    featureAngle              10;
+}
+
+bottomAir_to_rightSolid
+{
+    nFacesInCoarsestLevel     20;
+    featureAngle              10;
+}
+
+minX
+{
+    nFacesInCoarsestLevel     10;
+    featureAngle              10;
+}
+
+minY
+{
+    nFacesInCoarsestLevel     30;
+    featureAngle              10;
+}
+
+minZ
+{
+    nFacesInCoarsestLevel     20;
+    featureAngle              10;
+}
+
+maxX
+{
+    nFacesInCoarsestLevel     10;
+    featureAngle              10;
+}
+
+maxZ
+{
+    nFacesInCoarsestLevel     20;
+    featureAngle              10;
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/heater/radiationProperties

@@ -0,0 +1,36 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      radiationProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+radiation       on;
+
+radiationModel  opaqueSolid;
+
+absorptionEmissionModel constantAbsorptionEmission;
+
+constantAbsorptionEmissionCoeffs
+{
+    absorptivity    absorptivity [0 -1 0 0 0 0 0] 0.0;  //opaque
+    emissivity      emissivity [0 -1 0 0 0 0 0] 0.1;
+    E               E [1 -1 -3 0 0 0 0] 0;
+}
+
+scatterModel    none;
+
+sootModel none;
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/heater/thermophysicalProperties

@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------* \
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      thermophysicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            heSolidThermo;
+    mixture         pureMixture;
+    transport       constIso;
+    thermo          hConst;
+    equationOfState rhoConst;
+    specie          specie;
+    energy          sensibleEnthalpy;
+}
+
+mixture
+{
+    specie
+    {
+        molWeight   12;
+    }
+
+    transport
+    {
+        kappa   80;
+    }
+
+    thermodynamics
+    {
+        Hf      0;
+        Cp      450;
+    }
+
+    equationOfState
+    {
+        rho     8000;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/leftSolid/radiationProperties

@@ -0,0 +1 @@
+../heater/radiationProperties

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/leftSolid/thermophysicalProperties

@@ -0,0 +1 @@
+../heater/thermophysicalProperties

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/regionProperties

@@ -0,0 +1,24 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      regionProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+regions
+(
+    fluid       (bottomAir topAir)
+    solid       (heater leftSolid rightSolid)
+);
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/rightSolid/radiationProperties

@@ -0,0 +1 @@
+../heater/radiationProperties

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/rightSolid/thermophysicalProperties

@@ -0,0 +1 @@
+../heater/thermophysicalProperties

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/topAir/g

@@ -0,0 +1 @@
+../bottomAir/g

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/topAir/radiationProperties

@@ -0,0 +1 @@
+../bottomAir/radiationProperties

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/topAir/thermophysicalProperties

@@ -0,0 +1 @@
+../bottomAir/thermophysicalProperties

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/topAir/turbulenceProperties

@@ -0,0 +1 @@
+../bottomAir/turbulenceProperties

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/constant/topAir/viewFactorsDict

@@ -0,0 +1,71 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      viewFactorsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+
+writeViewFactorMatrix     true;
+writeFacesAgglomeration   true;
+writePatchViewFactors     false;
+
+topAir_to_heater
+{
+    nFacesInCoarsestLevel     24;
+    featureAngle              10;
+}
+
+topAir_to_leftSolid
+{
+    nFacesInCoarsestLevel     20;
+    featureAngle              10;
+}
+
+topAir_to_rightSolid
+{
+    nFacesInCoarsestLevel     20;
+    featureAngle              10;
+}
+
+minX
+{
+    nFacesInCoarsestLevel     10;
+    featureAngle              10;
+}
+
+maxY
+{
+    nFacesInCoarsestLevel     40;
+    featureAngle              10;
+}
+
+minZ
+{
+    nFacesInCoarsestLevel     20;
+    featureAngle              10;
+}
+
+maxX
+{
+    nFacesInCoarsestLevel     10;
+    featureAngle              10;
+}
+
+maxZ
+{
+    nFacesInCoarsestLevel     20;
+    featureAngle              10;
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/blockMeshDict

@@ -0,0 +1,96 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+    (-0.1 -0.04  -0.05)
+    ( 0.1 -0.04  -0.05)
+    ( 0.1  0.04  -0.05)
+    (-0.1  0.04  -0.05)
+    (-0.1 -0.04   0.05)
+    ( 0.1 -0.04   0.05)
+    ( 0.1  0.04   0.05)
+    (-0.1  0.04   0.05)
+);
+
+blocks
+(
+    hex (0 1 2 3 4 5 6 7) (30 10 10) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+    maxY
+    {
+        type wall;
+        faces
+        (
+            (3 7 6 2)
+        );
+    }
+    minX
+    {
+        type patch;
+        faces
+        (
+            (0 4 7 3)
+        );
+    }
+    maxX
+    {
+        type patch;
+        faces
+        (
+            (2 6 5 1)
+        );
+    }
+    minY
+    {
+        type wall;
+        faces
+        (
+            (1 5 4 0)
+        );
+    }
+    minZ
+    {
+        type wall;
+        faces
+        (
+            (0 3 2 1)
+        );
+    }
+    maxZ
+    {
+        type wall;
+        faces
+        (
+            (4 5 6 7)
+        );
+    }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/bottomAir/changeDictionaryDict

@@ -0,0 +1,184 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      changeDictionaryDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+boundary
+{
+    minX
+    {
+        type            wall;
+    }
+    maxX
+    {
+        type            wall;
+    }
+}
+
+U
+{
+    internalField   uniform (0.01 0 0);
+    boundaryField
+    {
+        ".*"
+        {
+            type            fixedValue;
+            value           uniform (0 0 0);
+        }
+    }
+}
+
+T
+{
+    internalField   uniform 300;
+    boundaryField
+    {
+        ".*"
+        {
+            type            zeroGradient;
+        }
+
+        "bottomAir_to_.*"
+        {
+            type            compressible::turbulentTemperatureRadCoupledMixed;
+            Tnbr            T;
+            kappaMethod     fluidThermo;
+            qrNbr           none;
+            qr              qr;
+            value           uniform 300;
+        }
+    }
+}
+
+epsilon
+{
+    internalField   uniform 0.01;
+    boundaryField
+    {
+        ".*"
+        {
+            type            epsilonWallFunction;
+            value           uniform 0.01;
+        }
+    }
+}
+
+k
+{
+    internalField   uniform 0.1;
+    boundaryField
+    {
+        ".*"
+        {
+            type            kqRWallFunction;
+            value           uniform 0.1;
+        }
+    }
+}
+
+p_rgh
+{
+    internalField   uniform 1e5;
+    boundaryField
+    {
+        ".*"
+        {
+            type            fixedFluxPressure;
+            value           uniform 1e5;
+        }
+    }
+}
+
+p
+{
+    internalField   uniform 1e5;
+    boundaryField
+    {
+        ".*"
+        {
+            type            calculated;
+            value           uniform 1e5;
+        }
+    }
+}
+
+qr
+{
+    internalField   uniform 0;
+    boundaryField
+    {
+        ".*"
+        {
+            type            greyDiffusiveRadiationViewFactor;
+            emissivityMode  lookup;
+            qro             uniform 0;
+            emissivity      uniform 1.0;
+            value           uniform 0;
+        }
+
+        "bottomAir_to_.*"
+        {
+            type            greyDiffusiveRadiationViewFactor;
+            emissivityMode  solidRadiation;
+            qro             uniform 0;
+            value           uniform 0;
+        }
+    }
+}
+
+G
+{
+    internalField   uniform 0;
+    boundaryField
+    {
+        ".*"
+        {
+            type            MarshakRadiation;
+            emissivityMode  lookup;
+            emissivity      uniform 1.0;
+            value           uniform 0;
+        }
+
+        "bottomAir_to_.*"
+        {
+            type            MarshakRadiation;
+            emissivityMode  solidRadiation;
+            value           uniform 0;
+        }
+    }
+}
+
+IDefault
+{
+    internalField   uniform 0;
+    boundaryField
+    {
+        ".*"
+        {
+            type            greyDiffusiveRadiation;
+            emissivityMode  lookup;
+            emissivity      uniform 1.0;
+            value           uniform 0;
+        }
+
+        "bottomAir_to_.*"
+        {
+            type            greyDiffusiveRadiation;
+            emissivityMode  solidRadiation;
+            value           uniform 0;
+        }
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/bottomAir/decomposeParDict

@@ -0,0 +1,44 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    note        "mesh decomposition control dictionary";
+    location    "system";
+    object      decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains  4;
+
+method          scotch;
+
+simpleCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+}
+
+hierarchicalCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+    order       xyz;
+}
+
+
+manualCoeffs
+{
+    dataFile    "decompositionData";
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/bottomAir/fvSchemes

@@ -0,0 +1,58 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default     steadyState;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+
+    div(phi,U)      bounded Gauss upwind;
+    div(phi,K)      bounded Gauss upwind;
+    div(phi,h)      bounded Gauss upwind;
+    div(phi,k)      bounded Gauss upwind;
+    div(phi,K)      bounded Gauss upwind;
+    div(phi,epsilon) bounded Gauss upwind;
+    div(phi,R)      bounded Gauss upwind;
+    div(R)          Gauss linear;
+    div(Ji,Ii_h)    Gauss linearUpwind grad(U);
+    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear uncorrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         uncorrected;
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/bottomAir/fvSolution

@@ -0,0 +1,62 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "p_rgh.*"
+    {
+        solver           GAMG;
+        tolerance        1e-7;
+        relTol           0.01;
+
+        smoother         GaussSeidel;
+
+    }
+
+    "(U|h|k|epsilon).*"
+    {
+        solver           PBiCGStab;
+        preconditioner   DILU;
+        tolerance        1e-7;
+        relTol           0.1;
+    }
+}
+
+PIMPLE
+{
+    momentumPredictor yes;
+    nNonOrthogonalCorrectors 0;
+    pRefCell        0;
+    pRefValue       100000;
+}
+
+relaxationFactors
+{
+    fields
+    {
+        "rho.*"         1.0;
+        "p_rgh.*"       0.7;
+    }
+    equations
+    {
+        "U.*"            0.3;
+        "h.*"            0.7;
+        "(k|epsilon|omega).*" 0.7;
+        "qr.*"          0.7;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/controlDict

@@ -0,0 +1,49 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application     chtMultiRegionFoam;
+
+startFrom       startTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         2000;
+
+deltaT          1;
+
+writeControl    timeStep;
+
+writeInterval   300;
+
+purgeWrite      10;
+
+writeFormat     ascii;
+
+writePrecision  7;
+
+writeCompression uncompressed;
+
+timeFormat      general;
+
+timePrecision   6;
+
+runTimeModifiable true;
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/decomposeParDict

@@ -0,0 +1,72 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    note        "mesh decomposition control dictionary";
+    location    "system";
+    object      decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains  4;
+
+//- Keep owner and neighbour on same processor for faces in zones:
+// preserveFaceZones (heater solid1 solid3);
+
+method          scotch;
+// method          hierarchical;
+// method          simple;
+// method          manual;
+
+simpleCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+}
+
+hierarchicalCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+    order       xyz;
+}
+
+scotchCoeffs
+{
+    //processorWeights
+    //(
+    //    1
+    //    1
+    //    1
+    //    1
+    //);
+    //writeGraph  true;
+    //strategy "b";
+}
+
+manualCoeffs
+{
+    dataFile    "decompositionData";
+}
+
+
+//// Is the case distributed
+//distributed     yes;
+//// Per slave (so nProcs-1 entries) the directory above the case.
+//roots
+//(
+//    "/tmp"
+//    "/tmp"
+//);
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/fvSchemes

@@ -0,0 +1,42 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+}
+
+gradSchemes
+{
+}
+
+divSchemes
+{
+}
+
+laplacianSchemes
+{
+}
+
+interpolationSchemes
+{
+}
+
+snGradSchemes
+{
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/fvSolution

@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+PIMPLE
+{
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/heater/changeDictionaryDict

@@ -0,0 +1,80 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      changeDictionaryDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+boundary
+{
+    minY
+    {
+        type            patch;
+    }
+    minZ
+    {
+        type            patch;
+    }
+    maxZ
+    {
+        type            patch;
+    }
+}
+
+T
+{
+    internalField   uniform 300;
+
+    boundaryField
+    {
+        ".*"
+        {
+            type            zeroGradient;
+            value           uniform 300;
+        }
+
+        heater_to_topAir
+        {
+            type            compressible::turbulentTemperatureRadCoupledMixed;
+            Tnbr            T;
+            kappaMethod     solidThermo;
+            qrNbr           qr;
+            qr              none;
+            value           uniform 300;
+        }
+
+        heater_to_bottomAir
+        {
+            type            compressible::turbulentTemperatureRadCoupledMixed;
+            Tnbr            T;
+            kappaMethod     solidThermo;
+            qrNbr           qr;
+            qr              none;
+            value           uniform 300;
+        }
+
+        "heater_to_.*"
+        {
+            type            compressible::turbulentTemperatureCoupledBaffleMixed;
+            Tnbr            T;
+            kappaMethod     solidThermo;
+            value           uniform 300;
+        }
+        minY
+        {
+            type            fixedValue;
+            value           uniform 500;
+        }
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/heater/decomposeParDict

@@ -0,0 +1,46 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    note        "mesh decomposition control dictionary";
+    location    "system";
+    object      decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains  4;
+
+
+method          scotch;
+
+simpleCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+}
+
+hierarchicalCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+    order       xyz;
+}
+
+
+manualCoeffs
+{
+    dataFile    "decompositionData";
+}
+
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/heater/fvSchemes

@@ -0,0 +1,49 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default     steadyState;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+}
+
+laplacianSchemes
+{
+    default             none;
+    laplacian(alpha,h)  Gauss linear uncorrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         uncorrected;
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/heater/fvSolution

@@ -0,0 +1,41 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "h.*"
+    {
+        solver           PCG;
+        preconditioner   DIC;
+        tolerance        1e-06;
+        relTol           0.1;
+    }
+}
+
+PIMPLE
+{
+    nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+    equations
+    {
+        "h.*"           0.7;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/leftSolid/changeDictionaryDict

@@ -0,0 +1,71 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      changeDictionaryDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+boundary
+{
+    minZ
+    {
+        type            patch;
+    }
+    maxZ
+    {
+        type            patch;
+    }
+}
+
+T
+{
+    internalField   uniform 300;
+
+    boundaryField
+    {
+        ".*"
+        {
+            type            zeroGradient;
+            value           uniform 300;
+        }
+
+        leftSolid_to_topAir
+        {
+            type            compressible::turbulentTemperatureRadCoupledMixed;
+            Tnbr            T;
+            kappaMethod     solidThermo;
+            qrNbr           qr;
+            qr              none;
+            value           uniform 300;
+        }
+
+        leftSolid_to_bottomAir
+        {
+            type            compressible::turbulentTemperatureRadCoupledMixed;
+            Tnbr            T;
+            kappaMethod     solidThermo;
+            qrNbr           qr;
+            qr              none;
+            value           uniform 300;
+        }
+
+        "leftSolid_to_.*"
+        {
+            type            compressible::turbulentTemperatureCoupledBaffleMixed;
+            Tnbr            T;
+            kappaMethod     solidThermo;
+            value           uniform 300;
+        }
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/leftSolid/decomposeParDict

@@ -0,0 +1,46 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    note        "mesh decomposition control dictionary";
+    location    "system";
+    object      decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains  4;
+
+
+method          scotch;
+
+simpleCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+}
+
+hierarchicalCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+    order       xyz;
+}
+
+
+manualCoeffs
+{
+    dataFile    "decompositionData";
+}
+
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/leftSolid/fvSchemes

@@ -0,0 +1 @@
+../heater/fvSchemes

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/leftSolid/fvSolution

@@ -0,0 +1,41 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "h.*"
+    {
+        solver           PCG;
+        preconditioner   DIC;
+        tolerance        1e-06;
+        relTol           0.1;
+    }
+}
+
+PIMPLE
+{
+    nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+    equations
+    {
+        "h.*"           0.7;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/rightSolid/changeDictionaryDict

@@ -0,0 +1,71 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      changeDictionaryDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+boundary
+{
+    minZ
+    {
+        type            patch;
+    }
+    maxZ
+    {
+        type            patch;
+    }
+}
+
+T
+{
+    internalField   uniform 300;
+
+    boundaryField
+    {
+        ".*"
+        {
+            type            zeroGradient;
+            value           uniform 300;
+        }
+
+        rightSolid_to_topAir
+        {
+            type            compressible::turbulentTemperatureRadCoupledMixed;
+            Tnbr            T;
+            kappaMethod     solidThermo;
+            qrNbr           qr;
+            qr              none;
+            value           uniform 300;
+        }
+
+        rightSolid_to_bottomAir
+        {
+            type            compressible::turbulentTemperatureRadCoupledMixed;
+            Tnbr            T;
+            kappaMethod     solidThermo;
+            qrNbr           qr;
+            qr              none;
+            value           uniform 300;
+        }
+
+        "rightSolid_to_.*"
+        {
+            type            compressible::turbulentTemperatureCoupledBaffleMixed;
+            Tnbr            T;
+            kappaMethod     solidThermo;
+            value           uniform 300;
+        }
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/rightSolid/decomposeParDict

@@ -0,0 +1,46 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    note        "mesh decomposition control dictionary";
+    location    "system";
+    object      decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains  4;
+
+
+method          scotch;
+
+simpleCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+}
+
+hierarchicalCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+    order       xyz;
+}
+
+
+manualCoeffs
+{
+    dataFile    "decompositionData";
+}
+
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/rightSolid/fvSchemes

@@ -0,0 +1 @@
+../heater/fvSchemes

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/rightSolid/fvSolution

@@ -0,0 +1,41 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "h.*"
+    {
+        solver           PCG;
+        preconditioner   DIC;
+        tolerance        1e-06;
+        relTol           0.1;
+    }
+}
+
+PIMPLE
+{
+    nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+    equations
+    {
+        "h.*"           0.7;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/topAir/changeDictionaryDict

@@ -0,0 +1,231 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      changeDictionaryDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+U
+{
+    internalField   uniform (0.1 0 0);
+    boundaryField
+    {
+        ".*"
+        {
+            type            fixedValue;
+            value           uniform (0 0 0);
+        }
+        minX
+        {
+            type            fixedValue;
+            value           uniform (0.1 0 0);
+        }
+        maxX
+        {
+            type            inletOutlet;
+            inletValue      uniform (0 0 0);
+            value           uniform (0.1 0 0);
+        }
+    }
+}
+
+T
+{
+    internalField   uniform 300;
+    boundaryField
+    {
+        ".*"
+        {
+            type            zeroGradient;
+        }
+
+        minX
+        {
+            type            fixedValue;
+            value           uniform 300;
+        }
+        maxX
+        {
+            type            inletOutlet;
+            inletValue      uniform 300;
+            value           uniform 300;
+        }
+
+        "topAir_to_.*"
+        {
+            type            compressible::turbulentTemperatureRadCoupledMixed;
+            Tnbr            T;
+            kappaMethod     fluidThermo;
+            qrNbr           none;
+            qr              qr;
+            value           uniform 300;
+        }
+    }
+}
+
+epsilon
+{
+    internalField   uniform 0.01;
+    boundaryField
+    {
+        ".*"
+        {
+            type            epsilonWallFunction;
+            value           uniform 0.01;
+        }
+
+        minX
+        {
+            type            fixedValue;
+            value           uniform 0.01;
+        }
+        maxX
+        {
+            type            inletOutlet;
+            inletValue      uniform 0.01;
+            value           uniform 0.01;
+        }
+    }
+}
+
+k
+{
+    internalField   uniform 0.1;
+    boundaryField
+    {
+        ".*"
+        {
+            type            kqRWallFunction;
+            value           uniform 0.1;
+        }
+
+        minX
+        {
+            type            fixedValue;
+            value           uniform 0.1;
+        }
+        maxX
+        {
+            type            inletOutlet;
+            inletValue      uniform 0.1;
+            value           uniform 0.1;
+        }
+    }
+}
+
+p_rgh
+{
+    internalField   uniform 1e5;
+    boundaryField
+    {
+        ".*"
+        {
+            type            fixedFluxPressure;
+            value           uniform 1e5;
+        }
+
+        maxX
+        {
+            type            fixedValue;
+            value           uniform 1e5;
+        }
+    }
+}
+
+p
+{
+    internalField   uniform 1e5;
+    boundaryField
+    {
+        ".*"
+        {
+            type            calculated;
+            value           uniform 1e5;
+        }
+
+        maxX
+        {
+            type            calculated;
+            value           uniform 1e5;
+        }
+    }
+}
+
+qr
+{
+    internalField   uniform 0;
+    boundaryField
+    {
+        ".*"
+        {
+            type            greyDiffusiveRadiationViewFactor;
+            emissivityMode  lookup;
+            qro             uniform 0;
+            emissivity      uniform 1.0;
+            value           uniform 0;
+        }
+
+        "topAir_to_.*"
+        {
+            type            greyDiffusiveRadiationViewFactor;
+            emissivityMode  solidRadiation;
+            qro             uniform 0;
+            value           uniform 0;
+        }
+    }
+}
+
+G
+{
+    internalField   uniform 0;
+    boundaryField
+    {
+        ".*"
+        {
+            type            MarshakRadiation;
+            emissivityMode  lookup;
+            emissivity      uniform 1.0;
+            value           uniform 0;
+        }
+
+        "topAir_to_.*"
+        {
+            type            MarshakRadiation;
+            emissivityMode  solidRadiation;
+            value           uniform 0;
+        }
+    }
+}
+
+IDefault
+{
+    internalField   uniform 0;
+    boundaryField
+    {
+        ".*"
+        {
+            type            greyDiffusiveRadiation;
+            emissivityMode  lookup;
+            emissivity      uniform 1.0;
+            value           uniform 0;
+        }
+
+        "topAir_to_.*"
+        {
+            type            greyDiffusiveRadiation;
+            emissivityMode  solidRadiation;
+            value           uniform 0;
+        }
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/topAir/decomposeParDict

@@ -0,0 +1,44 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    note        "mesh decomposition control dictionary";
+    location    "system";
+    object      decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains  4;
+
+method          scotch;
+
+simpleCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+}
+
+hierarchicalCoeffs
+{
+    n           (2 2 1);
+    delta       0.001;
+    order       xyz;
+}
+
+
+manualCoeffs
+{
+    dataFile    "decompositionData";
+}
+
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/topAir/fvSchemes

@@ -0,0 +1 @@
+../bottomAir/fvSchemes

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/topAir/fvSolution

@@ -0,0 +1,62 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "p_rgh.*"
+    {
+        solver           GAMG;
+        tolerance        1e-7;
+        relTol           0.01;
+
+        smoother         GaussSeidel;
+
+    }
+
+    "(U|h|k|epsilon).*"
+    {
+        solver           PBiCGStab;
+        preconditioner   DILU;
+        tolerance        1e-7;
+        relTol           0.1;
+    }
+}
+
+PIMPLE
+{
+    momentumPredictor yes;
+    nNonOrthogonalCorrectors 0;
+    pRefCell        0;
+    pRefValue       100000;
+}
+
+relaxationFactors
+{
+    fields
+    {
+        "rho.*"         1.0;
+        "p_rgh.*"       0.7;
+    }
+    equations
+    {
+        "U.*"           0.3;
+        "h.*"           0.7;
+        "(k|epsilon|omega).*" 0.7;
+        "qr.*"          0.7;
+    }
+}
+
+// ************************************************************************* //

tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeaterRadiation/system/topoSetDict

@@ -0,0 +1,178 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      topoSetDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+actions
+(
+    // Heater
+    {
+        name    heaterCellSet;
+        type    cellSet;
+        action  new;
+        source  boxToCell;
+        sourceInfo
+        {
+            box (-0.01001    0 -100 )(0.01001 0.00999 100);
+        }
+    }
+    {
+        name    heaterCellSet;
+        type    cellSet;
+        action  add;
+        source  boxToCell;
+        sourceInfo
+        {
+            box (-0.01001 -100 -0.01001)(0.01001 0.00999 0.01001);
+        }
+    }
+    {
+        name    heater;
+        type    cellZoneSet;
+        action  new;
+        source  setToCellZone;
+        sourceInfo
+        {
+            set heaterCellSet;
+        }
+    }
+
+    // leftSolid
+    {
+        name    leftSolidCellSet;
+        type    cellSet;
+        action  new;
+        source  boxToCell;
+        sourceInfo
+        {
+            box (-100 0 -100 )(-0.01001 0.00999 100);
+        }
+    }
+    {
+        name    leftSolid;
+        type    cellZoneSet;
+        action  new;
+        source  setToCellZone;
+        sourceInfo
+        {
+            set leftSolidCellSet;
+        }
+    }
+
+    // rightSolid
+    {
+        name    rightSolidCellSet;
+        type    cellSet;
+        action  new;
+        source  boxToCell;
+        sourceInfo
+        {
+            box (0.01001 0 -100 )(100 0.00999 100);
+        }
+    }
+    {
+        name    rightSolid;
+        type    cellZoneSet;
+        action  new;
+        source  setToCellZone;
+        sourceInfo
+        {
+            set rightSolidCellSet;
+        }
+    }
+
+    // topAir
+    {
+        name    topAirCellSet;
+        type    cellSet;
+        action  new;
+        source  boxToCell;
+        sourceInfo
+        {
+            box (-100 0.00999 -100 )(100 100 100);
+        }
+    }
+    {
+        name    topAir;
+        type    cellZoneSet;
+        action  new;
+        source  setToCellZone;
+        sourceInfo
+        {
+            set topAirCellSet;
+        }
+    }
+
+
+    // bottomAir is all the other cells
+    {
+        name    bottomAirCellSet;
+        type    cellSet;
+        action  new;
+        source  cellToCell;
+        sourceInfo
+        {
+            set heaterCellSet;
+        }
+    }
+    {
+        name    bottomAirCellSet;
+        type    cellSet;
+        action  add;
+        source  cellToCell;
+        sourceInfo
+        {
+            set leftSolidCellSet;
+        }
+    }
+    {
+        name    bottomAirCellSet;
+        type    cellSet;
+        action  add;
+        source  cellToCell;
+        sourceInfo
+        {
+            set rightSolidCellSet;
+        }
+    }
+    {
+        name    bottomAirCellSet;
+        type    cellSet;
+        action  add;
+        source  cellToCell;
+        sourceInfo
+        {
+            set topAirCellSet;
+        }
+    }
+    {
+        name    bottomAirCellSet;
+        type    cellSet;
+        action  invert;
+    }
+    {
+        name    bottomAir;
+        type    cellZoneSet;
+        action  new;
+        source  setToCellZone;
+        sourceInfo
+        {
+            set bottomAirCellSet;
+        }
+    }
+);
+
+
+// ************************************************************************* //