solvers::compressibleVoF: New solver module for compressible two-phase flow with VoF

executed with foamRun for single region simulations of foamMultiRun for
multi-region simulations.  Replaces compressibleInterFoam and all the
corresponding tutorials have been updated and moved to
tutorials/modules/compressibleVoF.

Class
    Foam::solvers::compressibleVoF

Description
    Solver module for for 2 compressible, non-isothermal immiscible fluids
    using a VOF (volume of fluid) phase-fraction based interface capturing
    approach, with optional mesh motion and mesh topology changes including
    adaptive re-meshing.

    The momentum and other fluid properties are of the "mixture" and a single
    momentum equation is solved.

    Either mixture or two-phase transport modelling may be selected.  In the
    mixture approach a single laminar, RAS or LES model is selected to model the
    momentum stress.  In the Euler-Euler two-phase approach separate laminar,
    RAS or LES selected models are selected for each of the phases.

    Uses the flexible PIMPLE (PISO-SIMPLE) solution for time-resolved and
    pseudo-transient and steady simulations.

    Optional fvModels and fvConstraints are provided to enhance the simulation
    in many ways including adding various sources, Lagrangian
    particles, surface film etc. and constraining or limiting the solution.

SourceFiles
    compressibleVoF.C

See also
    Foam::solvers::fluidSolver

tutorials/modules/compressibleVoF/damBreak/system/blockMeshDict

@@ -0,0 +1,105 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 0.146;
+
+vertices
+(
+    (0 0 0)
+    (2 0 0)
+    (2.16438 0 0)
+    (4 0 0)
+    (0 0.32876 0)
+    (2 0.32876 0)
+    (2.16438 0.32876 0)
+    (4 0.32876 0)
+    (0 4 0)
+    (2 4 0)
+    (2.16438 4 0)
+    (4 4 0)
+    (0 0 0.1)
+    (2 0 0.1)
+    (2.16438 0 0.1)
+    (4 0 0.1)
+    (0 0.32876 0.1)
+    (2 0.32876 0.1)
+    (2.16438 0.32876 0.1)
+    (4 0.32876 0.1)
+    (0 4 0.1)
+    (2 4 0.1)
+    (2.16438 4 0.1)
+    (4 4 0.1)
+);
+
+blocks
+(
+    hex (0 1 5 4 12 13 17 16) (23 8 1) simpleGrading (1 1 1)
+    hex (2 3 7 6 14 15 19 18) (19 8 1) simpleGrading (1 1 1)
+    hex (4 5 9 8 16 17 21 20) (23 42 1) simpleGrading (1 1 1)
+    hex (5 6 10 9 17 18 22 21) (4 42 1) simpleGrading (1 1 1)
+    hex (6 7 11 10 18 19 23 22) (19 42 1) simpleGrading (1 1 1)
+);
+
+defaultPatch
+{
+    type empty;
+}
+
+boundary
+(
+    leftWall
+    {
+        type wall;
+        faces
+        (
+            (0 12 16 4)
+            (4 16 20 8)
+        );
+    }
+    rightWall
+    {
+        type wall;
+        faces
+        (
+            (7 19 15 3)
+            (11 23 19 7)
+        );
+    }
+    lowerWall
+    {
+        type wall;
+        faces
+        (
+            (0 1 13 12)
+            (1 5 17 13)
+            (5 6 18 17)
+            (2 14 18 6)
+            (2 3 15 14)
+        );
+    }
+    atmosphere
+    {
+        type patch;
+        faces
+        (
+            (8 20 21 9)
+            (9 21 22 10)
+            (10 22 23 11)
+        );
+    }
+);
+
+
+// ************************************************************************* //

tutorials/modules/compressibleVoF/damBreak/system/controlDict

@@ -0,0 +1,57 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application     foamRun;
+
+solver          compressibleVoF;
+
+startFrom       startTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         1;
+
+deltaT          0.001;
+
+writeControl    adjustableRunTime;
+
+writeInterval   0.05;
+
+purgeWrite      0;
+
+writeFormat     ascii;
+
+writePrecision  6;
+
+writeCompression off;
+
+timeFormat      general;
+
+timePrecision   6;
+
+runTimeModifiable yes;
+
+adjustTimeStep  on;
+
+maxCo           1;
+maxAlphaCo      1;
+
+maxDeltaT       1;
+
+
+// ************************************************************************* //

tutorials/modules/compressibleVoF/damBreak/system/decomposeParDict

@@ -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    "system";
+    object      decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 4;
+
+method          simple;
+
+simpleCoeffs
+{
+    n               (2 2 1);
+}
+
+hierarchicalCoeffs
+{
+    n               (1 1 1);
+    order           xyz;
+}
+
+manualCoeffs
+{
+    dataFile        "";
+}
+
+distributed     no;
+
+roots           ( );
+
+
+// ************************************************************************* //

tutorials/modules/compressibleVoF/damBreak/system/fvSchemes

@@ -0,0 +1,59 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default         Euler;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    div(phi,alpha)  Gauss interfaceCompression vanLeer 1;
+
+    div(rhoPhi,U)   Gauss linearUpwind grad(U);Gauss upwind;
+    div(rhoPhi,T)   Gauss upwind;
+    div(rhoPhi,K)   Gauss upwind;
+    div(phi,p)      Gauss upwind;
+
+    div(rhoPhi,k)   Gauss upwind;
+    div(rhoPhi,epsilon) Gauss upwind;
+    div(rhoPhi,omega)   Gauss upwind;
+
+    div(((thermo:rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear uncorrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         uncorrected;
+}
+
+
+// ************************************************************************* //

tutorials/modules/compressibleVoF/damBreak/system/fvSolution

@@ -0,0 +1,81 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "alpha.water.*"
+    {
+        nAlphaCorr      2;
+        nAlphaSubCycles 1;
+
+        MULESCorr       yes;
+        nLimiterIter    3;
+
+        solver          smoothSolver;
+        smoother        symGaussSeidel;
+        tolerance       1e-8;
+        relTol          0;
+    }
+
+    "pcorr.*"
+    {
+        solver          PCG;
+        preconditioner  DIC;
+        tolerance       1e-5;
+        relTol          0;
+    }
+
+    p_rgh
+    {
+        solver          PCG;
+        preconditioner  DIC;
+        tolerance       1e-07;
+        relTol          0.05;
+    }
+
+    p_rghFinal
+    {
+        $p_rgh;
+        relTol          0;
+    }
+
+    "(U|T|k|epsilon|omega).*"
+    {
+        solver          smoothSolver;
+        smoother        symGaussSeidel;
+        tolerance       1e-06;
+        relTol          0;
+        minIter         1;
+    }
+}
+
+PIMPLE
+{
+    momentumPredictor   no;
+    nOuterCorrectors    1;
+    nCorrectors         3;
+    nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+    equations
+    {
+        ".*"                1;
+    }
+}
+
+// ************************************************************************* //

tutorials/modules/compressibleVoF/damBreak/system/setFieldsDict

@@ -0,0 +1,35 @@
+/*--------------------------------*- 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      setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+defaultFieldValues
+(
+    volScalarFieldValue alpha.water 0
+);
+
+regions
+(
+    boxToCell
+    {
+        box (0 0 -1) (0.1461 0.292 1);
+        fieldValues
+        (
+            volScalarFieldValue alpha.water 1
+        );
+    }
+);
+
+
+// ************************************************************************* //