New tutorial case for compressibleLesInterFoam: depthCharge3D

tutorials/compressibleLesInterFoam/depthCharge3D/0/U

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

tutorials/compressibleLesInterFoam/depthCharge3D/0/alpha1.org

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      alpha1.org;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 0 0 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    walls
+    {
+        type            zeroGradient;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/compressibleLesInterFoam/depthCharge3D/0/pd.org

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

tutorials/compressibleLesInterFoam/depthCharge3D/Allclean

+#!/bin/sh
+
+foamCleanTutorials cases
+rm -rf processor*
+rm 0/pd.gz 0/alpha1.gz

tutorials/compressibleLesInterFoam/depthCharge3D/Allrun

+#!/bin/sh
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+# Get application name from directory
+application="compressibleLesInterFoam"
+
+runApplication blockMesh
+cp 0/alpha1.org 0/alpha1
+cp 0/pd.org 0/pd
+runApplication setFields
+runApplication decomposePar
+hostname > system/machines
+runParallel $application 4 system/machines
+runApplication reconstructPar

tutorials/compressibleLesInterFoam/depthCharge3D/constant/LESProperties

+/*---------------------------------------------------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  1.0                                   |
+|   \\  /    A nd           | Web:      http://www.openfoam.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+
+FoamFile
+{
+    version         2.0;
+    format          ascii;
+
+    root            "";
+    case            "";
+    instance        "";
+    local           "";
+
+    class           dictionary;
+    object          LESProperties;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+LESModel        laminar;
+
+delta           smooth;
+
+laminarCoeffs
+{
+}
+
+oneEqEddyCoeffs
+{
+    ck               0.07;
+    ce               1.05;
+}
+
+dynOneEqEddyCoeffs
+{
+    ce               1.05;
+    filter          simple;
+}
+
+locDynOneEqEddyCoeffs
+{
+    ce               1.05;
+    filter          simple;
+}
+
+SmagorinskyCoeffs
+{
+    ce               1.05;
+    ck               0.07;
+}
+
+Smagorinsky2Coeffs
+{
+    ce               1.05;
+    ck               0.07;
+    cD2              0.02;
+}
+
+spectEddyViscCoeffs
+{
+    ce               1.05;
+    cB               8.22;
+    cK1              0.83;
+    cK2              1.03;
+    cK3              4.75;
+    cK4              2.55;
+}
+
+dynSmagorinskyCoeffs
+{
+    ce               1.05;
+    filter          simple;
+}
+
+mixedSmagorinskyCoeffs
+{
+    ce               1.05;
+    ck               0.07;
+    filter          simple;
+}
+
+dynMixedSmagorinskyCoeffs
+{
+    ce               1.05;
+    filter          simple;
+}
+
+LRRDiffStressCoeffs
+{
+    ce               1.05;
+    ck               0.09;
+    c1               1.8;
+    c2               0.6;
+}
+
+DeardorffDiffStressCoeffs
+{
+    ce               1.05;
+    ck               0.09;
+    cm               4.13;
+}
+
+SpalartAllmarasCoeffs
+{
+    alphaNut         1.5;
+    Cb1              0.1355;
+    Cb2              0.622;
+    Cw2              0.3;
+    Cw3              2;
+    Cv1              7.1;
+    CDES             0.65;
+    ck               0.07;
+}
+
+cubeRootVolCoeffs
+{
+    deltaCoeff      1;
+}
+
+PrandtlCoeffs
+{
+    delta           cubeRootVol;
+    cubeRootVolCoeffs
+    {
+        deltaCoeff      1;
+    }
+    smoothCoeffs
+    {
+        delta           cubeRootVol;
+        cubeRootVolCoeffs
+        {
+            deltaCoeff      1;
+        }
+        maxDeltaRatio   1.1;
+    }
+    Cdelta           0.158;
+}
+
+vanDriestCoeffs
+{
+    delta           cubeRootVol;
+    cubeRootVolCoeffs
+    {
+        deltaCoeff      1;
+    }
+    smoothCoeffs
+    {
+        delta           cubeRootVol;
+        cubeRootVolCoeffs
+        {
+            deltaCoeff      1;
+        }
+        maxDeltaRatio   1.1;
+    }
+    Aplus            26;
+    Cdelta           0.158;
+}
+
+smoothCoeffs
+{
+    delta           cubeRootVol;
+    cubeRootVolCoeffs
+    {
+        deltaCoeff      1;
+    }
+    maxDeltaRatio   1.1;
+}
+
+kappa            0.4187;
+
+wallFunctionCoeffs
+{
+    E                9;
+}
+
+
+// ************************************************************************* //

tutorials/compressibleLesInterFoam/depthCharge3D/constant/environmentalProperties

+/*---------------------------------------------------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  1.0                                   |
+|   \\  /    A nd           | Web:      http://www.openfoam.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+
+FoamFile
+{
+    version         2.0;
+    format          ascii;
+
+    root            "";
+    case            "";
+    instance        "";
+    local           "";
+
+    class           dictionary;
+    object          environmentalProperties;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+g               g [0 1 -2 0 0 0 0] (0 -9.81 0);
+
+// ************************************************************************* //

tutorials/compressibleLesInterFoam/depthCharge3D/constant/polyMesh/blockMeshDict

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+    (0 0 0)
+    (1 0 0)
+    (1 2 0)
+    (0 2 0)
+    (0 0 1)
+    (1 0 1)
+    (1 2 1)
+    (0 2 1)
+);
+
+blocks
+(
+    hex (0 1 2 3 4 5 6 7) (80 160 80) simpleGrading (1 1 1)
+);
+
+patches
+(
+    wall walls
+    (
+        (3 7 6 2)
+        (0 4 7 3)
+        (2 6 5 1)
+        (1 5 4 0)
+        (0 3 2 1)
+        (4 5 6 7)
+    )
+);
+
+// ************************************************************************* //

tutorials/compressibleLesInterFoam/depthCharge3D/constant/polyMesh/boundary

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       polyBoundaryMesh;
+    location    "constant/polyMesh";
+    object      boundary;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+1
+(
+    walls
+    {
+        type            wall;
+        nFaces          64000;
+        startFace       3040000;
+    }
+)
+
+// ************************************************************************* //

tutorials/compressibleLesInterFoam/depthCharge3D/constant/transportProperties

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phase1 //water
+{
+    transportModel  Newtonian;
+    nu              nu [0 2 -1 0 0 0 0] 1e-6;
+    rho             rho [1 -3 0 0 0 0 0] 1000;
+    rho0            rho0 [1 -3 0 0 0 0 0] 1000;
+    psi             psi [0 -2 2 0 0] 1e-5;
+}
+
+phase2 //air
+{
+    transportModel  Newtonian;
+    nu              nu [0 2 -1 0 0 0 0] 1.589e-5;
+    rho             rho [1 -3 0 0 0 0 0] 1;
+    rho0            rho0 [1 -3 0 0 0 0 0] 0;
+    psi             psi [0 -2 2 0 0] 1e-5;
+}
+
+pMin           pMin [1 -1 -2 0 0 0 0] 1e4;
+
+sigma           sigma [1 0 -2 0 0 0 0] 0.07;
+
+// ************************************************************************* //

tutorials/compressibleLesInterFoam/depthCharge3D/system/controlDict

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application lesInterFoam;
+
+startFrom       latestTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         0.5;
+
+deltaT          1e-04;
+
+writeControl    adjustableRunTime;
+
+writeInterval   5e-03;
+
+purgeWrite      0;
+
+writeFormat     ascii;
+
+writePrecision  8;
+
+writeCompression compressed;
+
+timeFormat      general;
+
+timePrecision   10;
+
+runTimeModifiable yes;
+
+adjustTimeStep  yes;
+
+maxCo           0.25;
+
+maxDeltaT       1;
+
+// ************************************************************************* //

tutorials/compressibleLesInterFoam/depthCharge3D/system/decomposeParDict

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  1.5                                   |
+|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 4;
+
+method          hierarchical;
+//method          metis;
+//method          parMetis;
+
+simpleCoeffs
+{
+    n               (1 4 1);
+    delta           0.001;
+}
+
+hierarchicalCoeffs
+{
+    n               (1 4 1);
+    delta           0.001;
+    order           xyz;
+}
+
+metisCoeffs
+{}
+
+manualCoeffs
+{
+    dataFile        "";
+}
+
+distributed     no;
+
+roots
+(
+);
+
+// ************************************************************************* //

tutorials/compressibleLesInterFoam/depthCharge3D/system/fvSchemes

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default    Euler;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    div(rho*phi,U)  Gauss upwind; //linear;
+
+    div(phi,alpha)  Gauss vanLeer;
+    div(phirb,alpha) Gauss interfaceCompression 1.0;
+
+    div(phi,pd)     Gauss upwind; //vanLeer; //linear;
+
+    div(phi,k)      Gauss vanLeer;
+
+    div((nuEff*dev(grad(U).T()))) Gauss linear;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear uncorrected;
+}
+
+interpolationSchemes
+{
+    default           linear;
+}
+
+snGradSchemes
+{
+    default         uncorrected;
+}
+
+fluxRequired
+{
+    default         no;
+    pd;
+    pcorr;
+    gamma;
+}
+
+// ************************************************************************* //

tutorials/compressibleLesInterFoam/depthCharge3D/system/fvSolution

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    pcorr PCG
+    {
+        preconditioner   GAMG
+        {
+            tolerance        1e-5;
+            relTol           0;
+
+            smoother         DICGaussSeidel;
+            nPreSweeps       0;
+            nPostSweeps      2;
+            nBottomSweeps    2;
+
+            cacheAgglomeration false;
+            nCellsInCoarsestLevel 10;
+            agglomerator     faceAreaPair;
+            mergeLevels      1;
+        };
+
+        tolerance        1e-5;
+        relTol           0;
+        maxIter          100;
+    };
+
+    rho diagonal
+    {};
+
+    pd GAMG
+    {
+        tolerance        1e-7;
+        relTol           0.01;
+
+        smoother         DIC; //GaussSeidel;
+        nPreSweeps       0;
+        nPostSweeps      2;
+        nFinestSweeps    2;
+
+        cacheAgglomeration true;
+        nCellsInCoarsestLevel 10;
+        agglomerator     faceAreaPair;
+        mergeLevels      1;
+    };
+
+    pdFinal PCG
+    {
+        preconditioner GAMG
+        {
+            tolerance        1e-7;
+            relTol           0;
+
+            nVcycles         2;
+
+            smoother         DICGaussSeidel;
+            nPreSweeps       2;
+            nPostSweeps      2;
+            nFinestSweeps    2;
+
+            cacheAgglomeration true;
+            nCellsInCoarsestLevel 10;
+            agglomerator     faceAreaPair;
+            mergeLevels      1;
+        };
+
+        tolerance        1e-7;
+        relTol           0;
+        maxIter          20;
+    };
+
+    U smoothSolver
+    {
+        smoother         GaussSeidel;
+        tolerance        1e-6;
+        relTol           0;
+        nSweeps          1;
+    };
+
+    k PBiCG
+    {
+        preconditioner   DILU;
+        tolerance        1e-08;
+        relTol           0;
+    };
+    B PBiCG
+    {
+        preconditioner   DILU;
+        tolerance        1e-08;
+        relTol           0;
+    };
+    nuTilda PBiCG
+    {
+        preconditioner   DILU;
+        tolerance        1e-08;
+        relTol           0;
+    };
+}
+
+PISO
+{
+    momentumPredictor no;
+    transSonic      no;
+    nOuterCorrectors 3;
+    nCorrectors     1;
+    nNonOrthogonalCorrectors 0;
+    nAlphaCorr      1;
+    nAlphaSubCycles 1;
+    cGamma          1;
+}
+
+// ************************************************************************* //

tutorials/compressibleLesInterFoam/depthCharge3D/system/machines

+noisy

tutorials/compressibleLesInterFoam/depthCharge3D/system/setFieldsDict

+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  dev                                   |
+|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+defaultFieldValues
+(
+    volScalarFieldValue alpha1 1
+    volScalarFieldValue pd 1e5
+);
+
+regions
+(
+    sphereToCell
+    {
+        centre (0.5 0.5 0.5);
+        radius 0.1;
+
+        fieldValues
+        (
+            volScalarFieldValue alpha1 0
+            volScalarFieldValue pd 10e5
+        );
+    }
+
+    boxToCell
+    {
+        box (-10 1 -1) (10 10 1);
+
+        fieldValues
+        (
+            volScalarFieldValue alpha1 0
+        );
+    }
+);
+
+// ************************************************************************* //