tutorials/modules/CHT/rivuletBox: New CHT/film/fluid tutorial case

Demonstration case for three region coupling with film consisting of an
aluminium panel with surface film running down forming rivulets in a box of air
which moved due to buoyancy with 6-way thermal and velocity coupling between the
panel<->film<->air<->panel.  The case runs serial and parallel with arbitrary
decomposition.

Currently extrudeToRegionMesh does not directly support three region coupling so
foamDictionary is used to edit the of the boundary files of box and film regions
to add box<->film coupling.

tutorials/modules/CHT/rivuletBox/0/box/T

@@ -0,0 +1,53 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 0 0 1 0 0 0];
+
+internalField   uniform 300;
+
+boundaryField
+{
+    inlet
+    {
+        type            inletOutlet;
+        inletValue      $internalField;
+        value           $internalField;
+    }
+
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      $internalField;
+        value           $internalField;
+    }
+
+    sides
+    {
+        type            zeroGradient;
+    }
+
+    film
+    {
+        type            coupledTemperature;
+        value           $internalField;
+    }
+
+    window
+    {
+        type            zeroGradient;
+    }
+}
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/0/box/U

@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volVectorField;
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0 0 0);
+
+boundaryField
+{
+    inlet
+    {
+        type            pressureInletOutletVelocity;
+        value           $internalField;
+    }
+
+    outlet
+    {
+        type            pressureInletOutletVelocity;
+        value           $internalField;
+    }
+
+    sides
+    {
+        type            noSlip;
+    }
+
+    film
+    {
+        type            mappedValue;
+        value           $internalField;
+    }
+
+    window
+    {
+        type            noSlip;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/0/box/p

@@ -0,0 +1,53 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 100000;
+
+boundaryField
+{
+    inlet
+    {
+        type            calculated;
+        value           $internalField;
+    }
+
+    outlet
+    {
+        type            calculated;
+        value           $internalField;
+    }
+
+    sides
+    {
+        type            calculated;
+        value           $internalField;
+    }
+
+    film
+    {
+        type            calculated;
+        value           $internalField;
+    }
+
+    window
+    {
+        type            calculated;
+        value           $internalField;
+    }
+}
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/0/box/p_rgh

@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    object      p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    inlet
+    {
+        type            prghTotalHydrostaticPressure;
+        p0              $internalField;
+        value           $internalField;
+    }
+
+    outlet
+    {
+        type            prghTotalHydrostaticPressure;
+        p0              $internalField;
+        value           $internalField;
+    }
+
+    sides
+    {
+        type            fixedFluxPressure;
+    }
+
+    film
+    {
+        type            fixedFluxPressure;
+    }
+
+    window
+    {
+        type            fixedFluxPressure;
+    }
+}
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/0/box/ph_rgh.orig

@@ -0,0 +1,51 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    object      ph_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedFluxPressure;
+        value           $internalField;
+    }
+
+    outlet
+    {
+        type            fixedValue;
+        value           $internalField;
+    }
+
+    sides
+    {
+        type            fixedFluxPressure;
+    }
+
+    film
+    {
+        type            fixedFluxPressure;
+    }
+
+    window
+    {
+        type            fixedFluxPressure;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/0/film/T

@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 0 0 1 0 0 0];
+
+internalField   uniform  300;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform 300;
+    }
+
+    outlet
+    {
+        type            zeroGradient;
+    }
+
+    sides
+    {
+        type            zeroGradient;
+    }
+
+    wall
+    {
+        type            coupledTemperature;
+        value           $internalField;
+    }
+
+    surface
+    {
+        type            coupledTemperature;
+        value           $internalField;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/0/film/U

@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volVectorField;
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0 0 0);
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform (0 -0.075 0);
+    }
+
+    outlet
+    {
+        type            zeroGradient;
+    }
+
+    sides
+    {
+        type            noSlip;
+    }
+
+    wall
+    {
+        type            noSlip;
+    }
+
+    surface
+    {
+        type            filmSurfaceVelocity;
+        Cs              0.005;
+        value           $internalField;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/0/film/delta

@@ -0,0 +1,64 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    object      delta;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 0 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    inlet
+    {
+        type            turbulentInlet;
+        fluctuationScale 0.05;
+        referenceField  uniform 1e-3;
+        alpha           0.1;
+        value           uniform 1e-3;
+    }
+
+    outlet
+    {
+        type            zeroGradient;
+    }
+
+    sides
+    {
+        type            zeroGradient;
+    }
+
+    wall
+    {
+        type            filmContactAngle;
+
+        contactAngle
+        {
+            type            gravitational;
+            theta0          70;
+            thetaAdv        90;
+            thetaRec        50;
+            gTheta          0.1;
+        }
+
+        value           $internalField;
+    }
+
+    surface
+    {
+        type            zeroGradient;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/0/film/p

@@ -0,0 +1,51 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform  1e5;
+
+boundaryField
+{
+    inlet
+    {
+        type            zeroGradient;
+    }
+
+    outlet
+    {
+        type            zeroGradient;
+    }
+
+    sides
+    {
+        type            zeroGradient;
+    }
+
+    wall
+    {
+        type            zeroGradient;
+    }
+
+    surface
+    {
+        type            mappedFilmPressure;
+
+        value           $internalField;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/0/panel/T

@@ -0,0 +1,40 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [ 0 0 0 1 0 0 0 ];
+
+internalField   uniform 330;
+
+boundaryField
+{
+    "(inlet|outlet|sides)"
+    {
+        type            zeroGradient;
+    }
+
+    wall
+    {
+        type            coupledTemperature;
+        value           $internalField;
+    }
+
+    insulatedWall
+    {
+        type            zeroGradient;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/Allclean

@@ -0,0 +1,12 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial clean functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+cleanCase
+
+rm -rf constant/panel/polyMesh
+rm -rf constant/film/polyMesh
+
+#------------------------------------------------------------------------------

tutorials/modules/CHT/rivuletBox/Allrun

@@ -0,0 +1,47 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+runApplication blockMesh -region box
+
+runApplication -s panel extrudeToRegionMesh \
+    -dict system/extrudeToRegionMeshDict.panel \
+    -region box -overwrite
+
+runApplication -s film extrudeToRegionMesh \
+    -dict system/extrudeToRegionMeshDict.film \
+    -region panel -overwrite
+
+# Add the coupling between box and film
+# Third-region coupling is not currently supported by extrudeToRegionMesh
+
+runApplication -s box foamDictionary -set \
+    "entry0/film/type=mappedExtrudedWall, \
+     entry0/film/neighbourRegion=film, \
+     entry0/film/neighbourPatch=surface, \
+     entry0/film/transformType=none" \
+     constant/box/polyMesh/boundary
+
+runApplication -s film foamDictionary -set \
+    "entry0/surface/type=mappedFilmSurface, \
+     entry0/surface/neighbourRegion=box, \
+     entry0/surface/neighbourPatch=film, \
+     entry0/surface/oppositePatch=wall, \
+     entry0/surface/transformType=none" \
+     constant/film/polyMesh/boundary
+
+printf "\n%s\n" "Creating files for paraview post-processing"
+paraFoam -touchAll
+echo
+
+# Serial run
+#runApplication $(getApplication)
+
+# Parallel run
+runApplication decomposePar -allRegions
+runParallel $(getApplication)
+runApplication reconstructPar -allRegions
+
+#------------------------------------------------------------------------------

tutorials/modules/CHT/rivuletBox/constant/box/g

@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       uniformDimensionedVectorField;
+    location    "constant";
+    object      g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -2 0 0 0 0];
+value           (0 -9.81 0);
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/constant/box/hRef

@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       uniformDimensionedScalarField;
+    location    "constant";
+    object      hRef;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 0 0 0 0 0];
+value           0;
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/constant/box/momentumTransport

@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      momentumTransport;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType  laminar;
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/constant/box/pRef

@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       uniformDimensionedScalarField;
+    location    "constant";
+    object      pRef;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+value           101325;
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/constant/box/physicalProperties

@@ -0,0 +1,47 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      physicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+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/modules/CHT/rivuletBox/constant/film/g

@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       uniformDimensionedVectorField;
+    location    "constant";
+    object      g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -2 0 0 0 0];
+value           (0 -9.81 0);
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/constant/film/momentumTransport

@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      momentumTransport;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType  laminar;
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/constant/film/physicalProperties

@@ -0,0 +1,39 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      physicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            heRhoThermo;
+    mixture         pureMixture;
+    properties      liquid;
+    energy          sensibleInternalEnergy;
+}
+
+mixture
+{
+    H2O;
+}
+
+sigma
+{
+    type    constant;
+    sigma   0.07;
+}
+
+deltaWet    1e-8;
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/constant/panel/physicalProperties

@@ -0,0 +1,51 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant/metal";
+    object      physicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            heSolidThermo;
+    mixture         pureMixture;
+    transport       constIsoSolid;
+    thermo          eConst;
+    equationOfState rhoConst;
+    specie          specie;
+    energy          sensibleInternalEnergy;
+}
+
+mixture
+{
+    // Aluminium
+
+    specie
+    {
+        molWeight       27;
+    }
+    equationOfState
+    {
+        rho             2700;
+    }
+    transport
+    {
+        kappa           200;
+    }
+    thermodynamics
+    {
+        Hf              0;
+        Cv              900;
+    }
+}
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/box/blockMeshDict

@@ -0,0 +1,106 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+    // front
+    (     0  0  0.02)
+    ( 0.125  0  0.02)
+    ( 0.625  0  0.02)
+    ( 0.750  0  0.02)
+    (     0  1  0.02)
+    ( 0.125  1  0.02)
+    ( 0.625  1  0.02)
+    ( 0.750  1  0.02)
+
+    // back
+    (     0  0  0)
+    ( 0.125  0  0)
+    ( 0.625  0  0)
+    ( 0.750  0  0)
+    (     0  1  0)
+    ( 0.125  1  0)
+    ( 0.625  1  0)
+    ( 0.750  1  0)
+);
+
+blocks
+(
+    hex (0 1 9 8 4 5 13 12) (30 10 240) simpleGrading (1 1 1)
+    hex (1 2 10 9 5 6 14 13) (120 10 240) simpleGrading (1 1 1)
+    hex (2 3 11 10 6 7 15 14) (30 10 240) simpleGrading (1 1 1)
+);
+
+boundary
+(
+    inlet
+    {
+        type patch;
+        faces
+        (
+            (5 6 14 13)
+        );
+    }
+
+    outlet
+    {
+        type patch;
+        faces
+        (
+            (0 1 9 8)
+            (1 2 10 9)
+            (2 3 11 10)
+        );
+    }
+
+    sides
+    {
+        type patch;
+        faces
+        (
+            (8 0 4 12)
+            (15 7 3 11)
+            (13 5 4 12)
+            (15 7 6 14)
+        );
+    }
+
+    film
+    {
+        type wall;
+        faces
+        (
+            (0 1 5 4)
+            (1 2 6 5)
+            (2 3 7 6)
+        );
+    }
+
+    window
+    {
+        type wall;
+        faces
+        (
+            (8 12 13 9)
+            (9 13 14 10)
+            (10 14 15 11)
+        );
+    }
+);
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/box/fvSchemes

@@ -0,0 +1,58 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default         Euler;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+    grad(p)         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+    div(phi,U)      Gauss upwind;
+    div(phi,K)      Gauss upwind;
+    div(phi,h)      Gauss upwind;
+    div(phi,k)      Gauss upwind;
+    div(phi,epsilon) Gauss upwind;
+    div(U)          Gauss linear;
+    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+    div(phi,Yi_h)  Gauss upwind;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear orthogonal;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         orthogonal;
+}
+
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/box/fvSolution

@@ -0,0 +1,83 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "rho.*"
+    {
+        solver          diagonal;
+    }
+
+    p_rgh
+    {
+        solver          GAMG;
+        smoother        GaussSeidel;
+
+        tolerance       1e-6;
+        relTol          0.01;
+    }
+
+    p_rghFinal
+    {
+        $p_rgh;
+        relTol          0;
+    }
+
+    ph_rgh
+    {
+        $p_rgh;
+    }
+
+    "(U|h)"
+    {
+        solver          PBiCGStab;
+        preconditioner  DILU;
+
+        tolerance       1e-5;
+        relTol          0.1;
+    }
+
+    "(U|h)Final"
+    {
+        $U;
+        relTol          0;
+    }
+
+    "(k|epsilon)"
+    {
+        $UFinal;
+    }
+}
+
+PIMPLE
+{
+    momentumPredictor yes;
+    nCorrectors     2;
+    nNonOrthogonalCorrectors 0;
+
+    hydrostaticInitialisation yes;
+}
+
+relaxationFactors
+{
+    equations
+    {
+        ".*"            1;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/controlDict

@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application     foamMultiRun;
+
+regionSolvers
+{
+    film            film;
+    panel           solid;
+    box             fluid;
+}
+
+startFrom       startTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         5;
+
+deltaT          1e-4;
+
+writeControl    adjustableRunTime;
+
+writeInterval   0.1;
+
+purgeWrite      0;
+
+writeFormat     binary;
+
+writePrecision  10;
+
+writeCompression off;
+
+timeFormat      general;
+
+timePrecision   6;
+
+runTimeModifiable yes;
+
+adjustTimeStep  yes;
+
+maxCo           0.2;
+
+maxDeltaT       5e-3;
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/decomposeParDict

@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 8;
+
+method          scotch;
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/extrudeToRegionMeshDict.film

@@ -0,0 +1,42 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    object      extrudeToRegionMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+region          film;
+
+patches         (filmWall);
+
+adaptMesh       yes;
+
+patchTypes      (mappedWall);
+patchNames      (wall);
+
+regionPatchTypes   (mappedFilmWall);
+regionPatchNames   (wall);
+
+regionOppositePatchTypes    (patch);
+regionOppositePatchNames    (surface);
+
+extrudeModel    linearNormal;
+
+nLayers         1;
+
+expansionRatio  1;
+
+linearNormalCoeffs
+{
+    thickness       0.01;
+}
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/extrudeToRegionMeshDict.panel

@@ -0,0 +1,39 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    object      extrudeToRegionMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+region          panel;
+
+patches         (film);
+
+adaptMesh       no;
+
+regionPatchTypes   (wall);
+regionPatchNames   (filmWall);
+
+regionOppositePatchTypes    (wall);
+regionOppositePatchNames    (insulatedWall);
+
+extrudeModel    linearNormal;
+
+nLayers         1;
+
+expansionRatio  1;
+
+linearNormalCoeffs
+{
+    thickness       0.002;
+}
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/film/fvSchemes

@@ -0,0 +1,47 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default         Euler;
+}
+
+gradSchemes
+{
+    default         filmGauss linear;
+}
+
+divSchemes
+{
+    default         none;
+
+    div(phid,alpha) Gauss upwind; // vanLeer;
+    div(alphaRhoPhi,U)  Gauss upwind;
+    div(alphaRhoPhi,e)  Gauss upwind;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear orthogonal;
+}
+
+snGradSchemes
+{
+    default         orthogonal;
+}
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/film/fvSolution

@@ -0,0 +1,55 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "alpha.*"
+    {
+        solver          PBiCGStab;
+        preconditioner  DILU;
+
+        tolerance       1e-10;
+        relTol          0;
+    }
+
+    "(U|e).*"
+    {
+        solver          PBiCGStab;
+        preconditioner  DILU;
+
+        tolerance       1e-10;
+        relTol          0;
+    }
+}
+
+PIMPLE
+{
+    momentumPredictor yes;
+    nOuterCorrectors  2;
+    nCorrectors       1;
+    nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+    equations
+    {
+        ".*"        1;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/fvSolution

@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+PIMPLE
+{
+    nOuterCorrectors 1;
+}
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/panel/fvSchemes

@@ -0,0 +1,47 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system/metal";
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default         Euler;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         corrected;
+}
+
+// ************************************************************************* //

tutorials/modules/CHT/rivuletBox/system/panel/fvSolution

@@ -0,0 +1,40 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system/metal";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    e
+    {
+        solver           GAMG;
+        smoother         symGaussSeidel;
+        tolerance        1e-6;
+        relTol           0.1;
+        maxIter          10;
+    }
+
+    eFinal
+    {
+        $e;
+        relTol           0;
+    }
+}
+
+PIMPLE
+{
+    nNonOrthogonalCorrectors 0;
+}
+
+// ************************************************************************* //