Template inflow-outflow case for compressible flow with rhoSimpleFoam

etc/templates/compressibleInflowOutflow/0/T

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+Tinlet          500;
+Tout            298;    // Used for fixedValue boundary condition on walls
+
+dimensions      [0 0 0 1 0 0 0];
+
+internalField   uniform $Tinlet;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform $Tinlet;
+    }
+
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform $Tout;
+        value           $inletValue;
+    }
+
+    wall
+    {
+        type            fixedValue;
+        value           uniform $Tout;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/compressibleInflowOutflow/0/U

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volVectorField;
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+Uinlet          (10 0 0);
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0 0 0);
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform $Uinlet;
+    }
+
+    outlet
+    {
+        type            pressureInletOutletVelocity;
+        value           uniform (0 0 0);
+    }
+
+    wall
+    {
+        type            fixedValue;
+        value           uniform (0 0 0);
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/compressibleInflowOutflow/0/alphat

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      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/compressibleInflowOutflow/0/epsilon

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      epsilon;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+epsilonInlet    0.001;
+
+dimensions      [0 2 -3 0 0 0 0];
+
+internalField   uniform $epsilonInlet;
+
+boundaryField
+{
+    inlet
+    {
+        type            compressible::turbulentMixingLengthDissipationRateInlet;
+        mixingLength    0.05;
+        value           uniform $epsilonInlet;
+    }
+
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform $epsilonInlet;
+        value           uniform $epsilonInlet;
+    }
+    wall
+    {
+        type            compressible::epsilonWallFunction;
+        value           uniform $epsilonInlet;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/compressibleInflowOutflow/0/k

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+kInlet          0.1;
+
+dimensions      [0 2 -2 0 0 0 0];
+
+internalField   uniform $kInlet;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform $kInlet;
+    }
+
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform $kInlet;
+        value           uniform $kInlet;
+    }
+
+    wall
+    {
+        type            compressible::kqRWallFunction;
+        value           uniform $kInlet;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/compressibleInflowOutflow/0/nut

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      mut;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+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            nutkWallFunction;
+        value           uniform 0;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/compressibleInflowOutflow/0/omega

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      omega;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+omegaInlet      1.0;
+
+dimensions      [0 0 -1 0 0 0 0];
+
+internalField   uniform $omegaInlet;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform $omegaInlet;
+    }
+
+    outlet
+    {
+        type            inletOutlet;
+        inletValue      uniform $omegaInlet;
+        value           uniform $omegaInlet;
+    }
+
+    wall
+    {
+        type            compressible::omegaWallFunction;
+        value           uniform $omegaInlet;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/compressibleInflowOutflow/0/p

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+pOut            1.0e5;
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform $pOut;
+
+boundaryField
+{
+    inlet
+    {
+        type            zeroGradient;
+    }
+
+    outlet
+    {
+        type            fixedValue;
+        value           uniform $pOut;
+    }
+
+    wall
+    {
+        type            zeroGradient;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

etc/templates/compressibleInflowOutflow/README

+Overview
+========
++ This is a template case with single inlet and outlet
++ Setup to run the compressible rhoSimpleFoam solver
++ The case is designed to be meshed with snappyHexMesh
++ snappyHexMesh is setup to use a single trisurface file named CAD.obj
++ Copy the CAD.obj file to the constant/triSurface directory
++ The CAD.obj should contain an inlet and outlet region to create the relevant
+  patches in the mesh
+
+Background Mesh
+===============
++ The user should establish the bounds of their CAD.obj file
++ The blockMeshDict file contains a backgroundMesh subditionary
++ Set xMin, xMax, etc to be beyond the CAD.obj bounds
++ Set background mesh density with xCells, yCells, zCells
++ Run blockMesh
+
+Background Mesh (alternative)
+=============================
++ The user can adopt the background mesh patches in the mesh
++ For example, the background mesh can provide external patches of an external
+  flow
++ An alternative blockMeshDict file is set up for this: blockMeshDict.extPatches
++ Simply copy blockMeshDict.extPatches to blockMeshDict and edit inlet, outlet
+  patches accordingly
+
+Castellated Mesh
+================
++ In the snappyHexMeshDict file, replace <inletPatch> with the name of the inlet
+  region in the CAD.obj file
++ Replace <outletPatch> with the name of the outlet region
++ run snappyHexMesh to obtain a castellatedMesh
++ Review the mesh; modify refinement levels and regenerate the mesh as required
+  (levels are set in refinementSurfaces and refinementRegions)
+
+Snapped Mesh
+============
++ In snappyHexMeshDict, set castellatedMesh off; snap on;
++ Run the snapping phase of snappyHexMesh
++ Review the mesh
+
+Layers
+======
++ To add layers to the mesh along wall boundary patches...
++ Switch on addLayers; switch snap off;
++ Run snappyHexMesh
++ The number of layers can be changed by modifying nSurfaceLayers
+
+Initialisation
+==============
++ In the field files in the 0 directory, set inlet values
++ For example, in 0/U, set the inlet velocity Uinlet
++ Set the viscosity in constant/transportProperties
\ No newline at end of file

etc/templates/compressibleInflowOutflow/constant/RASProperties

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      RASProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+RASModel        kEpsilon;
+
+turbulence      on;
+
+printCoeffs     on;
+
+// ************************************************************************* //

etc/templates/compressibleInflowOutflow/constant/polyMesh/blockMeshDict

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+backgroundMesh
+{
+    xMin    -1;
+    xMax     1;
+    yMin    -1;
+    yMax     1;
+    zMin    -1;
+    zMax     1;
+    xCells  20;
+    yCells  20;
+    zCells  20;
+}
+
+convertToMeters 1;
+
+vertices
+(
+    ($:backgroundMesh.xMin $:backgroundMesh.yMin $:backgroundMesh.zMin)
+    ($:backgroundMesh.xMax $:backgroundMesh.yMin $:backgroundMesh.zMin)
+    ($:backgroundMesh.xMax $:backgroundMesh.yMax $:backgroundMesh.zMin)
+    ($:backgroundMesh.xMin $:backgroundMesh.yMax $:backgroundMesh.zMin)
+
+    ($:backgroundMesh.xMin $:backgroundMesh.yMin $:backgroundMesh.zMax)
+    ($:backgroundMesh.xMax $:backgroundMesh.yMin $:backgroundMesh.zMax)
+    ($:backgroundMesh.xMax $:backgroundMesh.yMax $:backgroundMesh.zMax)
+    ($:backgroundMesh.xMin $:backgroundMesh.yMax $:backgroundMesh.zMax)
+);
+
+blocks
+(
+    hex (0 1 2 3 4 5 6 7)
+    (
+        $:backgroundMesh.xCells
+        $:backgroundMesh.yCells
+        $:backgroundMesh.zCells
+    )
+    simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //

etc/templates/compressibleInflowOutflow/constant/polyMesh/blockMeshDict.extPatches

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+backgroundMesh
+{
+    xMin    -1;
+    xMax     1;
+    yMin    -1;
+    yMax     1;
+    zMin    -1;
+    zMax     1;
+    xCells  20;
+    yCells  20;
+    zCells  20;
+}
+
+convertToMeters 1;
+
+vertices
+(
+    ($:backgroundMesh.xMin $:backgroundMesh.yMin $:backgroundMesh.zMin)
+    ($:backgroundMesh.xMax $:backgroundMesh.yMin $:backgroundMesh.zMin)
+    ($:backgroundMesh.xMax $:backgroundMesh.yMax $:backgroundMesh.zMin)
+    ($:backgroundMesh.xMin $:backgroundMesh.yMax $:backgroundMesh.zMin)
+
+    ($:backgroundMesh.xMin $:backgroundMesh.yMin $:backgroundMesh.zMax)
+    ($:backgroundMesh.xMax $:backgroundMesh.yMin $:backgroundMesh.zMax)
+    ($:backgroundMesh.xMax $:backgroundMesh.yMax $:backgroundMesh.zMax)
+    ($:backgroundMesh.xMin $:backgroundMesh.yMax $:backgroundMesh.zMax)
+);
+
+blocks
+(
+    hex (0 1 2 3 4 5 6 7)
+    (
+        $:backgroundMesh.xCells
+        $:backgroundMesh.yCells
+        $:backgroundMesh.zCells
+    )
+    simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+    left
+    {
+        type patch;
+        faces
+        (
+            (0 3 7 4)
+        );
+    }
+
+    right
+    {
+        type patch;
+        faces
+        (
+            (1 5 6 2)
+        );
+    }
+
+    bottom
+    {
+        type patch;
+        faces
+        (
+            (0 1 2 3)
+        );
+    }
+
+    top
+    {
+        type patch;
+        faces
+        (
+            (4 7 6 5)
+        );
+    }
+
+    back
+    {
+        type patch;