solvers::shockFluid: New solver module for density-based solution of compressible flow

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

Unlike rhoCentralFoam shockFluid supports mesh refinement/unrefinement, topology
change, run-time mesh-to-mesh mapping, load-balancing in addition to general
mesh-motion.

The tutorials/modules/shockFluid/movingCone case has been updated to demonstrate
run-time mesh-to-mesh mapping mesh topology change based on the
tutorials/modules/incompressibleFluid/movingCone.  shockFluid s

Description
    Solver module for density-based solution of compressible flow

    Based on central-upwind schemes of Kurganov and Tadmor with support for
    mesh-motion and topology change.

    Reference:
    \verbatim
        Greenshields, C. J., Weller, H. G., Gasparini, L.,
        & Reese, J. M. (2010).
        Implementation of semi‐discrete, non‐staggered central schemes
        in a colocated, polyhedral, finite volume framework,
        for high‐speed viscous flows.
        International journal for numerical methods in fluids, 63(1), 1-21.
    \endverbatim

SourceFiles
    shockFluid.C

See also
    Foam::solvers::fluidSolver
    Foam::solvers::incompressibleFluid

tutorials/modules/shockFluid/forwardStep/system/blockMeshDict

@@ -0,0 +1,98 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+    (0 0 -0.05)
+    (0.6 0 -0.05)
+    (0 0.2 -0.05)
+    (0.6 0.2 -0.05)
+    (3 0.2 -0.05)
+    (0 1 -0.05)
+    (0.6 1 -0.05)
+    (3 1 -0.05)
+    (0 0 0.05)
+    (0.6 0 0.05)
+    (0 0.2 0.05)
+    (0.6 0.2 0.05)
+    (3 0.2 0.05)
+    (0 1 0.05)
+    (0.6 1 0.05)
+    (3 1 0.05)
+);
+
+blocks
+(
+    hex (0 1 3 2 8 9 11 10) (48 16 1) simpleGrading (1 1 1)
+    hex (2 3 6 5 10 11 14 13) (48 64 1) simpleGrading (1 1 1)
+    hex (3 4 7 6 11 12 15 14) (192 64 1) simpleGrading (1 1 1)
+);
+
+defaultPatch
+{
+    type empty;
+}
+
+boundary
+(
+    inlet
+    {
+        type patch;
+        faces
+        (
+            (0 8 10 2)
+            (2 10 13 5)
+        );
+    }
+    outlet
+    {
+        type patch;
+        faces
+        (
+            (4 7 15 12)
+        );
+    }
+    bottom
+    {
+        type symmetryPlane;
+        faces
+        (
+            (0 1 9 8)
+        );
+    }
+    top
+    {
+        type symmetryPlane;
+        faces
+        (
+            (5 13 14 6)
+            (6 14 15 7)
+        );
+    }
+    obstacle
+    {
+        type patch;
+        faces
+        (
+            (1 3 11 9)
+            (3 4 12 11)
+        );
+    }
+);
+
+
+// ************************************************************************* //

tutorials/modules/shockFluid/forwardStep/system/controlDict

@@ -0,0 +1,56 @@
+/*--------------------------------*- 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          shockFluid;
+
+startFrom       startTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         4;
+
+deltaT          0.002;
+
+writeControl    adjustableRunTime;
+
+writeInterval   0.1;
+
+purgeWrite      0;
+
+writeFormat     ascii;
+
+writePrecision  6;
+
+writeCompression off;
+
+timeFormat      general;
+
+timePrecision   6;
+
+runTimeModifiable true;
+
+adjustTimeStep  yes;
+
+maxCo           0.2;
+
+maxDeltaT       1;
+
+
+// ************************************************************************* //

tutorials/modules/shockFluid/forwardStep/system/fvSchemes

@@ -0,0 +1,54 @@
+/*--------------------------------*- 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;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+fluxScheme      Kurganov;
+
+ddtSchemes
+{
+    default         Euler;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+    div(tauMC)      Gauss linear;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+    reconstruct(rho) vanLeer;
+    reconstruct(U)  vanLeerV;
+    reconstruct(T)  vanLeer;
+}
+
+snGradSchemes
+{
+    default         corrected;
+}
+
+
+// ************************************************************************* //

tutorials/modules/shockFluid/forwardStep/system/fvSolution

@@ -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;
+    location    "system";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "(rho|rhoU|rhoE).*"
+    {
+        solver          diagonal;
+    }
+
+    "U.*"
+    {
+        solver          smoothSolver;
+        smoother        GaussSeidel;
+        nSweeps         2;
+        tolerance       1e-09;
+        relTol          0.01;
+    }
+
+    "e.*"
+    {
+        $U;
+        tolerance       1e-10;
+        relTol          0;
+    }
+}
+
+PIMPLE
+{}
+
+
+// ************************************************************************* //