nonConformalCHT: new template case for CHT using NCC interface

The nonConformalCHT template case is designed to help create a conjugate
heat transfer (CHT) simulation in which fluid and solid regions are
coupled with non-conformal coupled (NCC) interfaces.  It includes an
Allmesh script which provides example commands to generate the meshes
for the fluid and solid regions using the 'snappyHexMeshConfig' utility,
and to generate NCC interfaces using 'createNonConformalCouples'.  The
remaining workflow to configure and run the CHT simulation is similar to
the 'singleFluidCHT' template case.

etc/templates/nonConformalCHT/Allclean

@@ -0,0 +1,27 @@
+#!/bin/sh
+cd "${0%/*}" || exit 1    # run from this directory
+
+# Source tutorial clean functions
+. "$WM_PROJECT_DIR/bin/tools/CleanFunctions"
+
+removeRegionDirs ()
+{
+    _regionDirs="$(foamDictionary -keywords constant/materialProperties)"
+
+    for d in system constant
+    do
+        for r in $_regionDirs
+        do
+            dir="${d}/${r}"
+            [ -d "$dir" ] && rm -rf "$dir"
+        done
+    done
+}
+
+cleanCase
+removeRegionDirs
+rm -rf 0 > /dev/null 2>&1
+rm -rf system/regionSolvers > /dev/null 2>&1
+rm -rf constant/extendedFeatureEdgeMesh > /dev/null 2>&1
+
+# ----------------------------------------------------------------- end-of-file

etc/templates/nonConformalCHT/Allmesh

@@ -0,0 +1,33 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. "$WM_PROJECT_DIR/bin/tools/RunFunctions"
+
+# !! Example !! meshing workflow for one solid and one fluid region
+# !! Requires customization !!
+
+region=solid
+runApplication -suffix $region snappyHexMeshConfig \
+    -surface "constant/geometry/$region.obj" \
+    -region $region \
+    -defaultPatch "($region wall)"
+
+# Other common options
+#    -minDimCells <n>
+#    -insidePoint '<(0 0 0)>'
+
+region=fluid
+runApplication -suffix $region snappyHexMeshConfig \
+    -region $region \
+    -layers '((solid 2))'
+
+for region in solid fluid
+do
+    runApplication -suffix $region blockMesh -region $region
+    runApplication -suffix $region snappyHexMesh -region $region -overwrite
+done
+
+runApplication createNonConformalCouples -overwrite
+
+# ----------------------------------------------------------------- end-of-file

etc/templates/nonConformalCHT/Allrun

@@ -0,0 +1,18 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. "$WM_PROJECT_DIR/bin/tools/RunFunctions"
+
+./Allmesh
+
+runApplication foamSetupCHT
+
+runApplication "$(getApplication)"
+
+echo
+echo "Creating files for paraview post-processing"
+echo
+paraFoam -touchAll
+
+# ----------------------------------------------------------------- end-of-file

etc/templates/nonConformalCHT/README

@@ -0,0 +1,84 @@
+Overview
+========
++ This is a template case for conjugate heat transfer (CHT), where mesh
+  regions are connected with non-conformal coupled (NCC) interfaces
++ The case is setup for a single solid region and a single fluid region; it
+  can be extended to include multiple solid and fluid regions
++ The Allmesh script demonstrates an example workflow for meshing the solid
+  and fluid regions
++ The foamSetupCHT utility is used to setup the field and material property
+  files, by copying them from the templates directory
++ The Allrun script demonstrates the commands to be run
+
+Meshing Strategy
+================
++ snappyHexMeshConfig is used to create blockMeshDict and snappyHexMeshDict
+  files for each of the solid and fluid regions
++ blockMesh and snappyHexMesh are used to create meshes for the individual
+  regions separately
++ snappyHexMeshConfig requires a surface geometry file for each of the mesh
+  regions. In the example provided in the 'Allmesh' script, 'solid.obj' is the
+  geometry file for the solid region
++ The .obj files should be saved in the 'constant/geometry' directory
++ The blockMeshDict and snappyHexMeshDict files are created by
+  snappyHexMeshConfig in sub-directories of the system directory
+  e.g. system/solid/blockMeshDict for the solid region
++ The regions are meshed separately by providing the '-region' flag to
+  blockMesh and snappyHexMesh e.g 'blockMesh -region solid'
++ The solid and fluid meshes are created in sub-directories of the constant
+  directory e.g. constant/solid/polyMesh
++ The Allmesh script can be extended to add more regions, or modified to
+  change the meshing strategy for individual regions
++ After the region meshes have been created, createNonConformalCouples is used
+  to connect the region meshes together
+
+Initialisation
+==============
++ The majority of the case initialisation is performed by the foamSetupCHT
+  utility, after the region meshes have been created
++ foamSetupCHT requires the user to configure a 'materialProperties' file
+  that includes a dictionary entry for each region
++ The dictionary entry for each region should contain:
+  + name of solver: e.g. fluid or solid
+  + name of material: e.g. air or aluminium
++ The material for each region can be selected from the configured materials
+  in the templates/materials directory
++ After configuring the materialProperties file, run the foamSetupCHT utility
++ foamSetupCHT generates region sub-directories in the 0, system and constant
+  directories
++ The default models and configuration (e.g. fvSchemes) for each region are
+  generally reliable
++ However, the user must pay attention to field files (U, T, k, omega, etc),
+  as the boundary conditions and initial conditions in these files are common
+  causes of numerical problems
++ The NCC patches (e.g. NCC1) are added to the "mapped" group when they are
+  created
++ The patches which aren't coupled are added to the "wall" group when they are
+  created
++ External wall boundaries are added to the "externalWall" group when they are
+  created
++ The patch groups are used to simplify the boundary conditions in the field
+  files (e.g. 0/fluid/T), and clearly distinguish between NCC patches and
+  other patches
+
+Source Terms
+============
++ Example fvModels files are included:
+  + solid region: 'heatSourceTotal' and 'heatSourceDensity' heat sources
+  + fluid region: 'thermalRadiation' radiative heat transfer
++ The example fvModels are switched off by default
+
+Running the Solver
+==================
++ The case uses foamMultiRun, which can run either as a steady-state solver,
+  or as a transient solver
++ The default setup is to run steady-state
++ To run transient, the user needs to modify:
+  + fvSchemes: select a suitable ddtScheme (e.g. Euler)
+  + controlDict: select a suitable deltaT and endTime
+
+Post-Processing
+===============
++ In order to post-process with ParaView, run "paraFoam -touchAll", then open
+  paraview and open the individual ".OpenFOAM" dummy files for individual mesh
+  regions.

etc/templates/nonConformalCHT/constant/heatSourceDensity

@@ -0,0 +1,23 @@
+/*--------------------------------*- 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      heatSource;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+type        heatSource;
+
+select      all;
+
+// Power per unit volume [W/m^3]
+q          <10>;
+
+//************************************************************************** //

etc/templates/nonConformalCHT/constant/heatSourceTotal

@@ -0,0 +1,23 @@
+/*--------------------------------*- 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      heatSource;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+type        heatSource;
+
+select      all;
+
+// Total power [W]
+Q           <100>;
+
+//************************************************************************** //

etc/templates/nonConformalCHT/constant/initialConditions

@@ -0,0 +1,19 @@
+/*--------------------------------*- 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      initialConditions;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+Tinitial       300;
+pInitial       1e5;
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/constant/materialProperties

@@ -0,0 +1,28 @@
+/*--------------------------------*- 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      materialProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+fluid
+{
+    solver          fluid;
+    material        air;
+}
+
+solid
+{
+    solver          solid;
+    material        copper;
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/constant/thermalRadiation

@@ -0,0 +1,19 @@
+/*--------------------------------*- 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      heatSource;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+type    radiation;
+libs    ("libradiationModels.so");
+
+//************************************************************************** //

etc/templates/nonConformalCHT/system/controlDict

@@ -0,0 +1,49 @@
+/*--------------------------------*- 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      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application     foamMultiRun;
+
+#includeIfPresent "regionSolvers"
+
+startFrom       startTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         500;
+
+deltaT          1;
+
+writeControl    timeStep;
+
+writeInterval   50;
+
+purgeWrite      5;
+
+writeFormat     ascii;
+
+writePrecision  8;
+
+writeCompression off;
+
+timeFormat      general;
+
+timePrecision   6;
+
+runTimeModifiable true;
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/system/createNonConformalCouplesDict

@@ -0,0 +1,28 @@
+/*--------------------------------*- 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      createNonConformalCouplesDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+fields  no;
+
+nonConformalCouples
+{
+    NCC1
+    {
+        regions         (solid fluid);
+        patches         (solid solid);
+    }
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/system/decomposeParDict

@@ -0,0 +1,32 @@
+/*--------------------------------*- 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      decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains  4;
+
+method          scotch;
+
+simpleCoeffs
+{
+    n           (2 2 1);
+}
+
+hierarchicalCoeffs
+{
+    n           (2 2 1);
+    order       xyz;
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/system/functions

@@ -0,0 +1,16 @@
+/*--------------------------------*- 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      functions;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/system/fvSchemes

@@ -0,0 +1,45 @@
+/*--------------------------------*- 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      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+}
+
+gradSchemes
+{
+}
+
+divSchemes
+{
+}
+
+laplacianSchemes
+{
+}
+
+interpolationSchemes
+{
+}
+
+snGradSchemes
+{
+}
+
+fluxRequired
+{
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/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;
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/system/meshQualityDict

@@ -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      meshQualityDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#includeEtc "caseDicts/mesh/generation/meshQualityDict.cfg"
+
+//- minFaceWeight (0 -> 0.5)
+//minFaceWeight 0.02;
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/G

@@ -0,0 +1,49 @@
+/*--------------------------------*- 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      G;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 0 -3 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    "(inlet|outlet)"
+    {
+        type            MarshakRadiation;
+        emissivityMode  lookup;
+        emissivity      uniform 1.0;
+        value           uniform 0;
+    }
+
+    wall
+    {
+        type            MarshakRadiation;
+        emissivityMode  lookup;
+        emissivity      uniform 1.0;
+        value           uniform 0;
+    }
+
+    externalWall
+    {
+        type            MarshakRadiation;
+        emissivityMode  lookup;
+        emissivity      uniform 1.0;
+        value           uniform 0;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/IDefault

@@ -0,0 +1,49 @@
+/*--------------------------------*- 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      IDefault;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 0 -3 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    "(inlet|outlet)"
+    {
+        type            greyDiffusiveRadiation;
+        emissivityMode  lookup;
+        emissivity      uniform 1.0;
+        value           uniform 0;
+    }
+
+    wall
+    {
+        type            greyDiffusiveRadiation;
+        emissivityMode  lookup;
+        emissivity      uniform 1.0;
+        value           uniform 0;
+    }
+
+    externalWall
+    {
+        type            greyDiffusiveRadiation;
+        emissivityMode  lookup;
+        emissivity      uniform 1.0;
+        value           uniform 0;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/T

@@ -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       volScalarField;
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "$FOAM_CASE/constant/initialConditions"
+
+dimensions      [0 0 0 1 0 0 0];
+
+internalField   uniform $Tinitial;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform $Tinitial;
+    }
+
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform $Tinitial;
+        value           uniform $Tinitial;
+    }
+
+    wall
+    {
+        type            zeroGradient;
+    }
+
+    mapped
+    {
+        type            coupledTemperature;
+        value           uniform $Tinitial;
+    }
+
+    externalWall
+    {
+        type            fixedValue;
+        value           uniform $Tinitial;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/U

@@ -0,0 +1,46 @@
+/*--------------------------------*- 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;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+Uinlet          1;
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0 0 0);
+
+boundaryField
+{
+    inlet
+    {
+        type            flowRateInletVelocity;
+        meanVelocity    constant $Uinlet;
+        value           uniform (0 0 0);
+    }
+
+    outlet
+    {
+        type            pressureInletOutletVelocity;
+        value           uniform (0 0 0);
+    }
+
+    wall
+    {
+        type            noSlip;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/alphat

@@ -0,0 +1,43 @@
+/*--------------------------------*- 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      alphat;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -1 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    inlet
+    {
+        type            calculated;
+        value           uniform 0;
+    }
+
+    outlet
+    {
+        type            calculated;
+        value           uniform 0;
+    }
+
+    wall
+    {
+        type            compressible::alphatWallFunction;
+        value           uniform 0;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/epsilon

@@ -0,0 +1,49 @@
+/*--------------------------------*- 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      epsilon;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+epsilonInlet      0.001;
+mixingLengthInlet 0.007;
+
+dimensions      [0 2 -3 0 0 0 0];
+
+internalField   uniform $epsilonInlet;
+
+boundaryField
+{
+    inlet
+    {
+        type            turbulentMixingLengthDissipationRateInlet;
+        mixingLength    $mixingLengthInlet;
+        value           uniform $epsilonInlet;
+    }
+
+    outlet
+    {
+        type            inletOutlet;
+        value           uniform $epsilonInlet;
+        inletValue      uniform $epsilonInlet;
+    }
+
+    wall
+    {
+        type            compressible::epsilonWallFunction;
+        value           uniform $epsilonInlet;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/k

@@ -0,0 +1,49 @@
+/*--------------------------------*- 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      k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+kInlet          0.001;
+intensityInlet  0.05;
+
+dimensions      [0 2 -2 0 0 0 0];
+
+internalField   uniform $kInlet;
+
+boundaryField
+{
+    inlet
+    {
+        type            turbulentIntensityKineticEnergyInlet;
+        intensity       $intensityInlet;
+        value           uniform $kInlet;
+    }
+
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform $kInlet;
+        value           uniform $kInlet;
+    }
+
+    wall
+    {
+        type            kqRWallFunction;
+        value           uniform $kInlet;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/nut

@@ -0,0 +1,43 @@
+/*--------------------------------*- 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      nut;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -1 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    inlet
+    {
+        type            calculated;
+        value           uniform 0;
+    }
+
+    outlet
+    {
+        type            calculated;
+        value           uniform 0;
+    }
+
+    wall
+    {
+        type            nutkWallFunction;
+        value           uniform 0;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/omega

@@ -0,0 +1,48 @@
+/*--------------------------------*- 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      omega;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+omegaInlet        1;
+mixingLengthInlet 0.007;
+
+dimensions      [0 0 -1 0 0 0 0];
+
+internalField   uniform $omegaInlet;
+
+boundaryField
+{
+    inlet
+    {
+        type            turbulentMixingLengthFrequencyInlet;
+        mixingLength    $mixingLengthInlet;
+        value           uniform $omegaInlet;
+    }
+
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform $omegaInlet;
+        value           uniform $omegaInlet;
+    }
+
+    wall
+    {
+        type            omegaWallFunction;
+        value           uniform $omegaInlet;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/p

@@ -0,0 +1,45 @@
+/*--------------------------------*- 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;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "$FOAM_CASE/constant/initialConditions"
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform $pInitial;
+
+boundaryField
+{
+    outlet
+    {
+        type            calculated;
+        value           $internalField;
+    }
+
+    inlet
+    {
+        type            calculated;
+        value           $internalField;
+    }
+
+    wall
+    {
+        type            calculated;
+        value           $internalField;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/fluid/p_rgh

@@ -0,0 +1,44 @@
+/*--------------------------------*- 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
+{
+    outlet
+    {
+        type            entrainmentPressure;
+        p0              $internalField;
+        value           $internalField;
+    }
+
+    inlet
+    {
+        type            fixedFluxPressure;
+        value           $internalField;
+    }
+
+    wall
+    {
+        $inlet;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/0/solid/T

@@ -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       volScalarField;
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "$FOAM_CASE/constant/initialConditions"
+
+dimensions      [ 0 0 0 1 0 0 0 ];
+
+internalField   uniform $Tinitial;
+
+boundaryField
+{
+    wall
+    {
+        type            zeroGradient;
+    }
+
+    mapped
+    {
+        type            coupledTemperature;
+        value           $internalField;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/constant/fluid/fvModels

@@ -0,0 +1,18 @@
+/*--------------------------------*- 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      fvModels;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+// #includeModel thermalRadiation
+
+//************************************************************************** //

etc/templates/nonConformalCHT/templates/constant/fluid/g

@@ -0,0 +1,19 @@
+/*--------------------------------*- 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;
+    object      g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -2 0 0 0 0];
+value           (0 0 -9.81);
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/constant/fluid/pRef

@@ -0,0 +1,22 @@
+/*--------------------------------*- 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;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "$FOAM_CASE/constant/initialConditions"
+
+dimensions      [1 -1 -2 0 0 0 0];
+value           $pInitial;
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/constant/solid/fvModels

@@ -0,0 +1,18 @@
+/*--------------------------------*- 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      fvModels;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+// #includeModel heatSourceTotal(Q=100)
+
+//************************************************************************** //

etc/templates/nonConformalCHT/templates/materials/air/momentumTransport

@@ -0,0 +1,48 @@
+/*--------------------------------*- 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      momentumTransport;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType RAS;
+
+RAS
+{
+    model               kOmegaSST;
+
+    turbulence          on;
+}
+
+LES
+{
+    model               SpalartAllmarasDDES;
+    delta               cubeRootVol;
+
+    turbulence          on;
+
+    cubeRootVolCoeffs
+    {
+        deltaCoeff      1;
+    }
+
+    smoothCoeffs
+    {
+        delta           cubeRootVol;
+        cubeRootVolCoeffs
+        {
+            deltaCoeff      1;
+        }
+        maxDeltaRatio   1.1;
+    }
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/air/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;
+    object      physicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            heRhoThermo;
+    mixture         pureMixture;
+    transport       const;
+    thermo          hConst;
+    equationOfState perfectGas;
+    specie          specie;
+    energy          sensibleEnthalpy;
+}
+
+mixture
+{
+    specie
+    {
+        nMoles      1;
+        molWeight   28.9;       // [kg/kmol]
+    }
+    thermodynamics
+    {
+        Cp          1005;       // [J/kg/K]
+        hf          0;
+    }
+    transport
+    {
+        mu          1.8e-05;    // [kg/m/s]
+        Pr          0.7;
+    }
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/air/radiationProperties

@@ -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;
+    location    "constant";
+    object      radiationProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+radiationModel  none; // P1, fvDOM;
+
+solverFreq 10;
+
+absorptionEmissionModel constant;
+
+constantCoeffs
+{
+    absorptivity    absorptivity    [0 -1 0 0 0 0 0] 0.5;
+    emissivity      emissivity      [0 -1 0 0 0 0 0] 0.5;
+    E               E               [1 -1 -3 0 0 0 0] 0;
+}
+
+fvDOMCoeffs
+{
+    nPhi        3;
+    nTheta      3;
+    tolerance   1e-3;
+    maxIter     10;
+}
+
+scatterModel    none;
+
+sootModel       none;
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/air/thermophysicalTransport

@@ -0,0 +1,25 @@
+/*--------------------------------*- 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      thermophysicalTransport;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+RAS
+{
+    model           eddyDiffusivity;
+
+    Prt             0.85;
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/aluminium/physicalProperties

@@ -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       dictionary;
+    object      physicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            heSolidThermo;
+    mixture         pureMixture;
+    transport       constIsoSolid;
+    thermo          eConst;
+    equationOfState rhoConst;
+    specie          specie;
+    energy          sensibleInternalEnergy;
+}
+
+mixture
+{
+    specie
+    {
+        nMoles      1;
+        molWeight   27; // [kg/kmol]
+    }
+
+    transport
+    {
+        kappa   240;    // [W/m/K]
+    }
+
+    thermodynamics
+    {
+        hf      0;
+        Cv      896;    // [J/kg/K]
+    }
+
+    equationOfState
+    {
+        rho     2712;   // [kg/m^3]
+    }
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/aluminium/radiationProperties

@@ -0,0 +1,29 @@
+/*--------------------------------*- 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      radiationProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+radiationModel  none; // opaqueSolid;
+
+absorptionEmissionModel constant;
+
+constantCoeffs
+{
+    absorptivity    absorptivity [ 0 -1 0 0 0 0 0 ] 0.0;
+    emissivity      emissivity [ 0 -1 0 0 0 0 0 ] 0.1;
+    E               E [ 1 -1 -3 0 0 0 0 ] 0;
+}
+
+scatterModel    none;
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/copper/physicalProperties

@@ -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       dictionary;
+    object      physicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            heSolidThermo;
+    mixture         pureMixture;
+    transport       constIsoSolid;
+    thermo          eConst;
+    equationOfState rhoConst;
+    specie          specie;
+    energy          sensibleInternalEnergy;
+}
+
+mixture
+{
+    specie
+    {
+        nMoles      1;
+        molWeight   63.5;   // [kg/kmol]
+    }
+
+    transport
+    {
+        kappa   380;        // [W/m/K]
+    }
+
+    thermodynamics
+    {
+        hf      0;
+        Cv      385;        // [J/kg/K]
+    }
+
+    equationOfState
+    {
+        rho     8940;       // [kg/m^3]
+    }
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/copper/radiationProperties

@@ -0,0 +1,29 @@
+/*--------------------------------*- 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      radiationProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+radiationModel  none; // opaqueSolid;
+
+absorptionEmissionModel constant;
+
+constantCoeffs
+{
+    absorptivity    absorptivity [ 0 -1 0 0 0 0 0 ] 0.0;
+    emissivity      emissivity [ 0 -1 0 0 0 0 0 ] 0.1;
+    E               E [ 1 -1 -3 0 0 0 0 ] 0;
+}
+
+scatterModel    none;
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/water/momentumTransport

@@ -0,0 +1,48 @@
+/*--------------------------------*- 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      momentumTransport;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType RAS;
+
+RAS
+{
+    model               kOmegaSST;
+
+    turbulence          on;
+}
+
+LES
+{
+    model               SpalartAllmarasDDES;
+    delta               cubeRootVol;
+
+    turbulence          on;
+
+    cubeRootVolCoeffs
+    {
+        deltaCoeff      1;
+    }
+
+    smoothCoeffs
+    {
+        delta           cubeRootVol;
+        cubeRootVolCoeffs
+        {
+            deltaCoeff      1;
+        }
+        maxDeltaRatio   1.1;
+    }
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/water/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;
+    object      physicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            heRhoThermo;
+    mixture         pureMixture;
+    transport       const;
+    thermo          eConst;
+    equationOfState rPolynomial;
+    specie          specie;
+    energy          sensibleInternalEnergy;
+}
+
+mixture
+{
+    specie
+    {
+        nMoles      1;
+        molWeight   18.0;       // [kg/kmol]
+    }
+    equationOfState
+    {
+        C (0.001278 -2.1055e-06 3.9689e-09 4.3772e-13 -2.0225e-16); // [J/kg/K]
+    }
+    thermodynamics
+    {
+        Cv          4181;      // [J/kg/K] at T = 293 K
+        hf          0;
+    }
+    transport
+    {
+        mu          1.0e-03;    // [kg/m/s]
+        Pr          7;
+    }
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/water/radiationProperties

@@ -0,0 +1,34 @@
+/*--------------------------------*- 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      radiationProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+radiationModel  none; // P1;
+
+solverFreq 10;
+
+absorptionEmissionModel constant;
+
+constantCoeffs
+{
+    absorptivity    absorptivity    [0 -1 0 0 0 0 0] 0.5;
+    emissivity      emissivity      [0 -1 0 0 0 0 0] 0.5;
+    E               E               [1 -1 -3 0 0 0 0] 0;
+}
+
+scatterModel    none;
+
+sootModel       none;
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/materials/water/thermophysicalTransport

@@ -0,0 +1,25 @@
+/*--------------------------------*- 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      thermophysicalTransport;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+RAS
+{
+    model           eddyDiffusivity;
+
+    Prt             0.85;
+}
+
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/system/fluid/fvSchemes

@@ -0,0 +1,96 @@
+/*--------------------------------*- 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      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    // For transient, replace steadyState, e.g. with Euler
+    default         steadyState;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+
+    limited         cellLimited Gauss linear 1;
+    grad(U)         $limited;
+    grad(k)         $limited;
+    grad(omega)     $limited;
+    grad(epsilon)   $limited;
+}
+
+divSchemes
+{
+    default         none;
+
+    // For steady-state, use the bounded form of advection schemes
+#ifeq $!ddtSchemes/default steadyState
+    div(phi,U)      bounded Gauss linearUpwind limited;
+    turbulence      bounded Gauss limitedLinear 1;
+#else
+    div(phi,U)      Gauss linearUpwind limited;
+    turbulence      Gauss limitedLinear 1;
+#endif
+
+    // Schemes for incompressible solvers
+    div(phi,k)      $turbulence;
+    div(phi,omega)  $turbulence;
+    div(phi,epsilon) $turbulence;
+    div((nuEff*dev2(T(grad(U))))) Gauss linear;
+
+    // Additional schemes for compressible solvers
+    div(phi,e)      $turbulence;
+    div(phi,h)      $turbulence;
+    div(phi,K)      $turbulence;
+    div(phi,Ekp)    $turbulence;
+
+    div(phid,p)     Gauss upwind;
+#ifeq $!ddtSchemes/default steadyState
+    div(phi,(p|rho)) bounded Gauss upwind;
+    div(Ji,Ii_h)    bounded Gauss linearUpwind grad(Ii_h);
+#else
+    div(phi,(p|rho)) Gauss upwind;
+    div(Ji,Ii_h)    Gauss linearUpwind grad(Ii_h);
+#endif
+
+    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         corrected;
+}
+
+fluxRequired
+{
+    default         no;
+    p                 ;
+}
+
+wallDist
+{
+    method meshWave;
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/system/fluid/fvSolution

@@ -0,0 +1,116 @@
+/*--------------------------------*- 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;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "(rho|rhoFinal)"
+    {
+        solver          PCG
+        preconditioner  DIC;
+        tolerance       1e-7;
+        relTol          0;
+    }
+
+    p_rgh
+    {
+        solver           GAMG;
+        tolerance        1e-7;
+        relTol           0.01;
+
+        smoother         GaussSeidel;
+        maxIter          100;
+    }
+
+    "(U|h|e|k|omega|epsilon)"
+    {
+        solver          PBiCGStab;
+        preconditioner  DILU;
+        tolerance       1e-6;
+        relTol          0.1;
+    }
+
+    "(G|Ii.*)"
+    {
+        $p_rgh;
+        tolerance       1e-7;
+        relTol          0.1;
+    }
+
+    p_rghFinal
+    {
+        $p_rgh;
+        relTol         0;
+    }
+
+    "(U|h|e|k|omega|epsilon)Final"
+    {
+        $U;
+        relTol         0;
+    }
+
+    GFinal
+    {
+        $G;
+        relTol         0;
+    }
+}
+
+// timeScheme = steadyState for a steady-state simulation; otherwise transient
+timeScheme $fvSchemes!ddtSchemes/default;
+
+PIMPLE
+{
+    momentumPredictor yes;
+    nNonOrthogonalCorrectors 0;
+
+// Steady-state and transient correctors
+#ifeq $timeScheme steadyState
+    nOuterCorrectors 1;
+    nCorrectors     1;
+#else
+    nOuterCorrectors 2;
+    nCorrectors     2;
+#endif
+}
+
+// Relaxation factors for incompressible and compressible solution
+#ifeq $timeScheme steadyState
+relaxationFactors
+{
+    fields
+    {
+        p               0.3;
+        rho             1.0;
+    }
+    equations
+    {
+        U                       0.3;
+        "(e|h|k|epsilon|omega)" 0.7;
+        "G"                     1.0;
+        "ILambda.*"             1.0;
+    }
+}
+#else
+relaxationFactors
+{
+    // Transient relaxation factors
+    equations
+    {
+        ".*"  1;
+    }
+}
+#endif
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/system/solid/fvConstraints

@@ -0,0 +1,29 @@
+/*--------------------------------*- 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      fvConstraints;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+/*
+fixedTemperature
+{
+    type            fixedTemperature;
+
+    select          all;
+
+    mode            uniform;
+
+    temperature     constant 300; // Set temperature (K)
+}
+*/
+
+//************************************************************************** //

etc/templates/nonConformalCHT/templates/system/solid/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;
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    // For transient, replace steadyState, e.g. with Euler
+    default         steadyState;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         corrected;
+}
+
+// ************************************************************************* //

etc/templates/nonConformalCHT/templates/system/solid/fvSolution

@@ -0,0 +1,46 @@
+/*--------------------------------*- 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;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "(h|e)"
+    {
+        solver           GAMG;
+        tolerance        1e-6;
+        relTol           0.1;
+        smoother         GaussSeidel;
+    }
+
+    "(h|e)Final"
+    {
+        $h;
+        relTol         0;
+    }
+}
+
+PIMPLE
+{
+    nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+    equations
+    {
+        ".*"   0.7;
+    }
+}
+
+// ************************************************************************* //