INT: Integration of rhoPimpleAdiabaticFoam

Solver for low Mach no. flows with adiabatic thermodynamics and updated
pressure-velocity coupling given by the RCM interpolation procedure
described in

    \verbatim
        Knacke, T. (2013).
        Potential effects of Rhie & Chow type interpolations in airframe
        noise simulations. In: Schram, C., Dénos, R., Lecomte E. (ed):
        Accurate and efficient aeroacoustic prediction approaches for
        airframe noise, VKI LS 2013-03.
    \endverbatim

Original code supplied by Thilo Knacke, CFD E+F GmbH
contact: info@cfd-berlin.com

Integrated into OpenFOAM by OpenCFD Ltd.

applications/solvers/compressible/rhoPimpleAdiabaticFoam/EEqn.H

@@ -0,0 +1,50 @@
+{
+    volScalarField& he = thermo.he();
+
+    const tmp<volScalarField>& tCp = thermo.Cp();
+    const tmp<volScalarField>& tCv = thermo.Cv();
+
+    const volScalarField& Cp = tCp();
+    const volScalarField& Cv = tCv();
+    const scalar gamma = max(Cp/Cv).value();
+
+    if (mag(gamma - min(Cp/Cv).value()) > VSMALL)
+    {
+        notImplemented("gamma not constant in space");
+    }
+
+    const dictionary& thermoDict = thermo.subDict("mixture");
+
+    const dictionary& eosDict = thermoDict.subDict("equationOfState");
+
+    bool local = eosDict.lookupOrDefault<bool>("local", false);
+
+    // Evolve T as:
+    //
+    // T_1 = T_0 \frac{p}{p_0}^{\frac{\gamma - 1}{\gamma}}
+
+    if (!local)
+    {
+        const scalar T0 = readScalar(eosDict.lookup("T0"));
+        const scalar p0 = readScalar(eosDict.lookup("p0"));
+
+        he = thermo.he(p, pow(p/p0, (gamma - scalar(1))/gamma)*T0);
+    }
+    else
+    {
+        const volScalarField& T0 = T.oldTime();
+        const volScalarField& p0 = p.oldTime();
+
+        he = thermo.he(p, pow(p/p0, (gamma - scalar(1))/gamma)*T0);
+    }
+
+    thermo.correct();
+
+    psi = 1.0/((Cp - Cv)*T);
+
+    rho = thermo.rho();
+    rho.relax();
+
+    rho.writeMinMax(Info);
+}
+

applications/solvers/compressible/rhoPimpleAdiabaticFoam/Make/files

@@ -0,0 +1,3 @@
+rhoPimpleAdiabaticFoam.C
+
+EXE = $(FOAM_APPBIN)/rhoPimpleAdiabaticFoam

applications/solvers/compressible/rhoPimpleAdiabaticFoam/Make/options

@@ -0,0 +1,20 @@
+EXE_INC = \
+    -I$(LIB_SRC)/transportModels/compressible/lnInclude \
+    -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
+    -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
+    -I$(LIB_SRC)/TurbulenceModels/compressible/lnInclude \
+    -I$(LIB_SRC)/finiteVolume/cfdTools \
+    -I$(LIB_SRC)/finiteVolume/lnInclude \
+    -I$(LIB_SRC)/meshTools/lnInclude \
+    -I$(LIB_SRC)/sampling/lnInclude \
+
+EXE_LIBS = \
+    -lcompressibleTransportModels \
+    -lfluidThermophysicalModels \
+    -lspecie \
+    -lturbulenceModels \
+    -lcompressibleTurbulenceModels \
+    -lfiniteVolume \
+    -lmeshTools \
+    -lsampling \
+    -lfvOptions

applications/solvers/compressible/rhoPimpleAdiabaticFoam/UEqn.H

@@ -0,0 +1,24 @@
+// Solve the Momentum equation
+
+MRF.correctBoundaryVelocity(U);
+
+tmp<fvVectorMatrix> tUEqn
+(
+    fvm::ddt(rho, U) + fvm::div(phi, U)
+  + MRF.DDt(rho, U)
+  + turbulence->divDevRhoReff(U)
+ ==
+    fvOptions(rho, U)
+);
+fvVectorMatrix& UEqn = tUEqn.ref();
+
+UEqn.relax();
+
+fvOptions.constrain(UEqn);
+
+if (pimple.momentumPredictor())
+{
+    solve(UEqn == -fvc::grad(p));
+
+    fvOptions.correct(U);
+}

applications/solvers/compressible/rhoPimpleAdiabaticFoam/createFields.H

@@ -0,0 +1,102 @@
+Info<< "Reading thermophysical properties\n" << endl;
+
+autoPtr<fluidThermo> pThermo
+(
+    fluidThermo::New(mesh)
+);
+fluidThermo& thermo = pThermo();
+thermo.validate(args.executable(), "h", "e");
+
+volScalarField& p = thermo.p();
+volScalarField& T = thermo.T();
+
+volScalarField rho
+(
+    IOobject
+    (
+        "rho",
+        runTime.timeName(),
+        mesh,
+        IOobject::READ_IF_PRESENT,
+        IOobject::AUTO_WRITE
+    ),
+    thermo.rho()
+);
+
+Info<< "Reading field U\n" << endl;
+volVectorField U
+(
+    IOobject
+    (
+        "U",
+        runTime.timeName(),
+        mesh,
+        IOobject::MUST_READ,
+        IOobject::AUTO_WRITE
+    ),
+    mesh
+);
+
+Info<< "Calculating face flux field phi\n" << endl;
+
+surfaceScalarField phi
+(
+    IOobject
+    (
+        "phi",
+        runTime.timeName(),
+        mesh,
+        IOobject::READ_IF_PRESENT,
+        IOobject::AUTO_WRITE
+    ),
+    linearInterpolate(rho)*linearInterpolate(U) & mesh.Sf()
+);
+
+Info<< "Calculating face flux field phiByRho\n" << endl;
+
+surfaceScalarField phiByRho
+(
+    IOobject
+    (
+        "phiByRho",
+        runTime.timeName(),
+        mesh,
+        IOobject::READ_IF_PRESENT,
+        IOobject::AUTO_WRITE
+    ),
+    phi/linearInterpolate(rho)
+);
+
+Info<< "Creating turbulence model\n" << endl;
+autoPtr<compressible::turbulenceModel> turbulence
+(
+    compressible::turbulenceModel::New
+    (
+        rho,
+        U,
+        phi,
+        thermo
+    )
+);
+
+mesh.setFluxRequired(p.name());
+
+Info<< "Creating field dpdt\n" << endl;
+volScalarField dpdt
+(
+    IOobject
+    (
+        "dpdt",
+        runTime.timeName(),
+        mesh
+    ),
+    mesh,
+    dimensionedScalar("dpdt", p.dimensions()/dimTime, 0)
+);
+
+#include "createMRF.H"
+
+Info<< "Creating compressibility field psi\n" << endl;
+volScalarField psi("psi", 1.0/((thermo.Cp() - thermo.Cv())*T));
+psi.oldTime() = 1.0/((thermo.Cp() - thermo.Cv())*T.oldTime());
+psi.oldTime().oldTime() = 1.0/((thermo.Cp()-thermo.Cv())*T.oldTime().oldTime());

applications/solvers/compressible/rhoPimpleAdiabaticFoam/pEqn.H

@@ -0,0 +1,95 @@
+{
+    volScalarField rAU(1.0/UEqn.A());
+    volVectorField HbyA("HbyA", U);
+    HbyA = rAU*UEqn.H();
+
+
+    // Define coefficients and pseudo-velocities for RCM interpolation
+    // M[U] = AU - H = -grad(p)
+    // U = H/A - 1/A grad(p)
+    // H/A = U + 1/A grad(p)
+    surfaceScalarField rhorAUf
+    (
+        "rhorAUf",
+        fvc::interpolate(rho)/fvc::interpolate(UEqn.A())
+    );
+
+    surfaceVectorField rhoHbyAf
+    (
+        "rhoHbyAf",
+        fvc::interpolate(rho)*fvc::interpolate(U)
+      + rhorAUf*fvc::interpolate(fvc::grad(p))
+    );
+
+    #include "resetBoundaries.H"
+
+    if (pimple.nCorrPISO() <= 1)
+    {
+        tUEqn.clear();
+    }
+
+    if (pimple.transonic())
+    {
+         FatalError
+             << "\nTransonic option not available for " << args.executable()
+             << exit(FatalError);
+    }
+    else
+    {
+        // Rhie & Chow interpolation (part 1)
+        surfaceScalarField phiHbyA
+        (
+            "phiHbyA",
+            (
+                (rhoHbyAf & mesh.Sf())
+              + rhorAUf*fvc::interpolate(rho)*fvc::ddtCorr(U, phiByRho)
+              + fvc::interpolate(rho)
+              * fvc::alphaCorr(U, phiByRho, pimple.finalInnerIter())
+            )
+        );
+
+        MRF.makeRelative(fvc::interpolate(rho), phiHbyA);
+
+        // Non-orthogonal pressure corrector loop
+        while (pimple.correctNonOrthogonal())
+        {
+            // Pressure corrector
+            fvScalarMatrix pEqn
+            (
+                fvm::ddt(psi, p)
+              + fvc::div(phiHbyA)
+              - fvm::laplacian(rhorAUf, p)
+              ==
+                fvOptions(psi, p, rho.name())
+            );
+
+            pEqn.solve(mesh.solver(p.select(pimple.finalInnerIter())));
+
+            // Rhie & Chow interpolation (part 2)
+            if (pimple.finalNonOrthogonalIter())
+            {
+                phi = phiHbyA + pEqn.flux();
+            }
+        }
+    }
+
+    phiByRho = phi/fvc::interpolate(rho);
+
+    #include "rhoEqn.H"
+    #include "compressibleContinuityErrs.H"
+
+    // Explicitly relax pressure for momentum corrector
+    p.relax();
+
+    U = HbyA - rAU*fvc::grad(p);
+    U.correctBoundaryConditions();
+    fvOptions.correct(U);
+}
+
+rho = thermo.rho();
+
+if (thermo.dpdt())
+{
+    dpdt = fvc::ddt(p);
+}
+

applications/solvers/compressible/rhoPimpleAdiabaticFoam/resetBoundaries.H

@@ -0,0 +1,25 @@
+{
+    // Keep standard formulation on domain boundaries to ensure compatibility
+    // with existing boundary conditions
+    const Foam::FieldField<Foam::fvsPatchField, scalar> rhorAUf_orig
+    (
+        fvc::interpolate(rho.boundaryField()*rAU.boundaryField())
+    );
+
+    const Foam::FieldField<Foam::fvsPatchField, vector> rhoHbyA_orig
+    (
+        fvc::interpolate(rho.boundaryField()*HbyA.boundaryField())
+    );
+
+    surfaceScalarField::Boundary& rhorAUfbf = rhorAUf.boundaryFieldRef();
+    surfaceVectorField::Boundary& rhoHbyAfbf = rhoHbyAf.boundaryFieldRef();
+
+    forAll(U.boundaryField(), patchi)
+    {
+        if (!U.boundaryField()[patchi].coupled())
+        {
+            rhorAUfbf[patchi] = rhorAUf_orig[patchi];
+            rhoHbyAfbf[patchi] = rhoHbyA_orig[patchi];
+        }
+    }
+}

applications/solvers/compressible/rhoPimpleAdiabaticFoam/rhoPimpleAdiabaticFoam.C

@@ -0,0 +1,129 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2017 OpenCFD Ltd.
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+License
+    This file is part of OpenFOAM.
+
+    OpenFOAM is free software: you can redistribute it and/or modify it
+    under the terms of the GNU General Public License as published by
+    the Free Software Foundation, either version 3 of the License, or
+    (at your option) any later version.
+
+    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
+    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
+    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
+    for more details.
+
+    You should have received a copy of the GNU General Public License
+    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.
+
+Application
+    rhoPimpleAdiabaticFoam
+
+Description
+    Transient solver for laminar or turbulent flow of weakly compressible
+    fluids for low Mach number aeroacoustic applications.
+
+    Uses the flexible PIMPLE (PISO-SIMPLE) solution for time-resolved and
+    pseudo-transient simulations. The RCM interpolation is used as in
+
+    \verbatim
+        Knacke, T. (2013).
+        Potential effects of Rhie & Chow type interpolations in airframe
+        noise simulations. In: Schram, C., Dénos, R., Lecomte E. (ed):
+        Accurate and efficient aeroacoustic prediction approaches for
+        airframe noise, VKI LS 2013-03.
+    \endverbatim
+
+
+    Contact:      info@cfd-berlin.com
+
+\*---------------------------------------------------------------------------*/
+
+#include "fvCFD.H"
+#include "fluidThermo.H"
+#include "turbulentFluidThermoModel.H"
+#include "bound.H"
+#include "pimpleControl.H"
+#include "fvOptions.H"
+
+#include "ddtScheme.H"
+#include "fvcCorrectAlpha.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+int main(int argc, char *argv[])
+{
+    #include "postProcess.H"
+
+    #include "setRootCase.H"
+    #include "createTime.H"
+    #include "createMesh.H"
+    #include "createControl.H"
+    #include "createTimeControls.H"
+
+    #include "createFields.H"
+    #include "createFvOptions.H"
+    #include "initContinuityErrs.H"
+
+    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+    Info<< "\nStarting time loop\n" << endl;
+
+    while (runTime.run())
+    {
+        #include "readTimeControls.H"
+        #include "compressibleCourantNo.H"
+        #include "setDeltaT.H"
+
+        runTime++;
+
+        Info<< "Time = " << runTime.timeName() << nl << endl;
+
+        if (pimple.nCorrPIMPLE() <= 1)
+        {
+            #include "rhoEqn.H"
+        }
+
+        // --- Pressure-velocity PIMPLE corrector loop
+        while (pimple.loop())
+        {
+            U.storePrevIter();
+            rho.storePrevIter();
+            phi.storePrevIter();
+            phiByRho.storePrevIter();
+
+            #include "UEqn.H"
+
+            // --- Pressure corrector loop
+            while (pimple.correct())
+            {
+                #include "pEqn.H"
+            }
+
+            #include "EEqn.H"
+
+            if (pimple.turbCorr())
+            {
+                turbulence->correct();
+            }
+        }
+
+        runTime.write();
+
+        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
+            << "  ClockTime = " << runTime.elapsedClockTime() << " s"
+            << nl << endl;
+    }
+
+    Info<< "End\n" << endl;
+
+    return 0;
+}
+
+
+// ************************************************************************* //

src/finiteVolume/Make/files

@@ -401,6 +401,7 @@ finiteVolume/fvc/fvcFlux.C
 finiteVolume/fvc/fvcMeshPhi.C
 finiteVolume/fvc/fvcSmooth/fvcSmooth.C
 finiteVolume/fvc/fvcReconstructMag.C
+finiteVolume/fvc/fvcCorrectAlpha.C
 
 general = cfdTools/general
 $(general)/findRefCell/findRefCell.C

src/finiteVolume/finiteVolume/ddtSchemes/backwardDdtScheme/backwardDdtScheme.H

@@ -3,7 +3,7 @@
   \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
    \\    /   O peration     |
     \\  /    A nd           | Copyright (C) 2011-2017 OpenFOAM Foundation
-     \\/     M anipulation  |
+     \\/     M anipulation  | Copyright (C) 2017 OpenCFD Ltd.
 -------------------------------------------------------------------------------
 License
     This file is part of OpenFOAM.
@@ -98,7 +98,19 @@ public:
         backwardDdtScheme(const fvMesh& mesh, Istream& is)
         :
             ddtScheme<Type>(mesh, is)
-        {}
+        {
+            if (is.good() && !is.eof())
+            {
+                this->ddtPhiCoeff_ = readScalar(is);
+            }
+
+            // Ensure the old-old-time cell volumes are available
+            // for moving meshes
+            if (mesh.moving())
+            {
+                mesh.V00();
+            }
+        }
 
 
     // Member Functions

src/finiteVolume/finiteVolume/ddtSchemes/ddtScheme/ddtScheme.C

@@ -3,7 +3,7 @@
   \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
    \\    /   O peration     |
     \\  /    A nd           | Copyright (C) 2011-2016 OpenFOAM Foundation
-     \\/     M anipulation  |
+     \\/     M anipulation  | Copyright (C) 2017 OpenCFD Ltd.
 -------------------------------------------------------------------------------
 License
     This file is part of OpenFOAM.
@@ -156,13 +156,36 @@ tmp<surfaceScalarField> ddtScheme<Type>::fvcDdtPhiCoeff
     const fluxFieldType& phiCorr
 )
 {
-    tmp<surfaceScalarField> tddtCouplingCoeff = scalar(1)
+    tmp<surfaceScalarField> tddtCouplingCoeff
-      - min
+    (
+        new surfaceScalarField
+        (
+            IOobject
+            (
+                "ddtCouplingCoeff",
+                U.mesh().time().timeName(),
+                U.mesh()
+            ),
+            U.mesh(),
+            dimensionedScalar("one", dimless, 1.0)
+        )
+    );
+
+
+    if (ddtPhiCoeff_ < 0)
+    {
+        tddtCouplingCoeff.ref() =- min
         (
             mag(phiCorr)
            /(mag(phi) + dimensionedScalar("small", phi.dimensions(), SMALL)),
             scalar(1)
         );
+    }
+    else
+    {
+        tddtCouplingCoeff.ref() =
+            dimensionedScalar("ddtPhiCoeff", dimless, ddtPhiCoeff_);
+    }
 
     surfaceScalarField& ddtCouplingCoeff = tddtCouplingCoeff.ref();
 

src/finiteVolume/finiteVolume/ddtSchemes/ddtScheme/ddtScheme.H

@@ -3,7 +3,7 @@
   \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
    \\    /   O peration     |
     \\  /    A nd           | Copyright (C) 2011-2016 OpenFOAM Foundation
-     \\/     M anipulation  |
+     \\/     M anipulation  | Copyright (C) 2017 OpenCFD Ltd.
 -------------------------------------------------------------------------------
 License
     This file is part of OpenFOAM.
@@ -30,6 +30,7 @@ Group
 Description
     Abstract base class for ddt schemes.
 
+
 SourceFiles
     ddtScheme.C
 
@@ -76,6 +77,9 @@ protected:
 
         const fvMesh& mesh_;
 
+        //- Input for fvcDdtPhiCoeff (-1 default)
+        scalar ddtPhiCoeff_;
+
 
     // Private Member Functions
 
@@ -109,13 +113,15 @@ public:
         //- Construct from mesh
         ddtScheme(const fvMesh& mesh)
         :
-            mesh_(mesh)
+            mesh_(mesh),
+            ddtPhiCoeff_(-1)
         {}
 
         //- Construct from mesh and Istream
-        ddtScheme(const fvMesh& mesh, Istream&)
+        ddtScheme(const fvMesh& mesh, Istream& is)
         :
-            mesh_(mesh)
+            mesh_(mesh),
+            ddtPhiCoeff_(-1)
         {}
 
 

src/finiteVolume/finiteVolume/fvc/fvcCorrectAlpha.C

@@ -0,0 +1,80 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2017 OpenCFD Ltd.
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+License
+    This file is part of OpenFOAM.
+
+    OpenFOAM is free software: you can redistribute it and/or modify it
+    under the terms of the GNU General Public License as published by
+    the Free Software Foundation, either version 3 of the License, or
+    (at your option) any later version.
+
+    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
+    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
+    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
+    for more details.
+
+    You should have received a copy of the GNU General Public License
+    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.
+
+InNamespace
+    Foam::fvc
+
+Description
+    Correct flux-U difference in the internal loop  using relaxation factor
+
+SourceFiles
+    fvcCorrectAlpha.C
+
+\*---------------------------------------------------------------------------*/
+
+#include "fvcCorrectAlpha.H"
+#include "fvMesh.H"
+#include "surfaceInterpolate.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace fvc
+{
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+tmp<GeometricField<scalar, fvsPatchField, surfaceMesh>> alphaCorr
+(
+    const GeometricField<vector, fvPatchField, volMesh>& U,
+    const GeometricField<scalar, fvsPatchField, surfaceMesh>& phiU,
+    const bool finalIter
+)
+{
+    const fvMesh& mesh = U.mesh();
+    const word fieldName = U.select(finalIter);
+
+    scalar alpha = 1;
+    if (mesh.relaxEquation(fieldName))
+    {
+        alpha = mesh.equationRelaxationFactor(fieldName);
+    }
+
+    return
+        (1 - alpha)
+       *(phiU.prevIter() - (fvc::interpolate(U.prevIter()) & mesh.Sf()));
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace fvc
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// ************************************************************************* //

src/finiteVolume/finiteVolume/fvc/fvcCorrectAlpha.H

@@ -0,0 +1,71 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2017 OpenCFD Ltd.
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+License
+    This file is part of OpenFOAM.
+
+    OpenFOAM is free software: you can redistribute it and/or modify it
+    under the terms of the GNU General Public License as published by
+    the Free Software Foundation, either version 3 of the License, or
+    (at your option) any later version.
+
+    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
+    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
+    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
+    for more details.
+
+    You should have received a copy of the GNU General Public License
+    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.
+
+InNamespace
+    Foam::fvc
+
+Description
+    Correct flux-U difference in the internal loop  using relaxation factor
+
+SourceFiles
+    fvcCorrectAlpha.C
+
+\*---------------------------------------------------------------------------*/
+
+
+#ifndef fvcCorrectAlpha_H
+#define fvcCorrectAlpha_H
+
+#include "volFieldsFwd.H"
+#include "surfaceFieldsFwd.H"
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+                     Namespace fvc functions Declaration
+\*---------------------------------------------------------------------------*/
+
+namespace fvc
+{
+    tmp<GeometricField<scalar, fvsPatchField, surfaceMesh>> alphaCorr
+    (
+        const GeometricField<vector, fvPatchField, volMesh>& U,
+        const GeometricField<scalar, fvsPatchField, surfaceMesh>& phiU,
+        const bool finalIter
+    );
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/0.orig/T

@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 0 0 1 0 0 0];
+
+internalField   uniform 224;
+
+boundaryField
+{
+    top
+    {
+        type            slip;
+    }
+
+    bottom
+    {
+        type            slip;
+    }
+
+    left
+    {
+        type            fixedValue;
+        value           $internalField;
+    }
+
+    right
+    {
+        type            inletOutlet;
+        inletValue      $internalField;
+        value           $internalField;
+    }
+
+    frontAndBack
+    {
+        type            empty;
+    }
+}
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/0.orig/U

@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volVectorField;
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (50 0 0);
+
+boundaryField
+{
+    top
+    {
+        type            slip;
+    }
+
+    bottom
+    {
+        type            slip;
+    }
+
+    left
+    {
+        type            fixedValue;
+        value           uniform (50 0 0);
+    }
+
+    right
+    {
+        type            inletOutlet;
+        inletValue      uniform (0 0 0);
+        value           uniform (50 0 0);
+    }
+
+    frontAndBack
+    {
+        type            empty;
+    }
+}
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/0.orig/p

@@ -0,0 +1,65 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 101325;
+
+boundaryField
+{
+    top
+    {
+        type            zeroGradient;
+    }
+
+    bottom
+    {
+        type            zeroGradient;
+    }
+
+    left
+    {
+        type            waveTransmissive;
+        field           p;
+        phi             phi;
+        rho             rho;
+        psi             thermo:psi;
+        gamma           1.4;
+        fieldInf        101325;
+        lInf            5.0;
+        value           $internalField;
+    }
+
+    right
+    {
+        type            waveTransmissive;
+        field           p;
+        phi             phi;
+        rho             rho;
+        psi             thermo:psi;
+        gamma           1.4;
+        fieldInf        101325;
+        lInf            5.0;
+        value           $internalField;
+    }
+
+    frontAndBack
+    {
+        type            empty;
+    }
+}
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/Allclean

@@ -0,0 +1,9 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # run from this directory
+
+# Source tutorial clean functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+cleanCase
+\rm -rf 0
+

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/Allrun

@@ -0,0 +1,11 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+restore0Dir
+runApplication blockMesh
+runApplication -s preProcess $(getApplication) -postProcess -dict system/preProcess
+runApplication decomposePar
+runParallel $(getApplication)

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/constant/thermophysicalProperties

@@ -0,0 +1,53 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      thermophysicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+    type            hePsiThermo;
+    mixture         pureMixture;
+    transport       const;
+    thermo          hConst;
+    equationOfState perfectGas;
+    specie          specie;
+    energy          sensibleEnthalpy;
+}
+
+mixture
+{
+    equationOfState
+    {
+        p0          103308.85730683322;
+        T0          225.24440406165331;
+    }
+    specie
+    {
+        molWeight   28.970278977370906;
+    }
+    thermodynamics
+    {
+        Cp          1004.5;
+        Hf          0;
+    }
+    transport
+    {
+        mu          1.4585464649816414e-05;
+        Pr          0.7179;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/constant/turbulenceProperties

@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType  laminar;
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/system/blockMeshDict

@@ -0,0 +1,123 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+// D = 0.57
+convertToMeters 0.57;
+
+x0      -3.5;
+x1      1.8;
+x2      15.7;
+x3      21;
+y0      -5.2;
+y1      5.2;
+
+vertices
+(
+    ($x0 $y0 0)
+    ($x1 $y0 0)
+    ($x2 $y0 0)
+    ($x3 $y0 0)
+
+    ($x3 $y1 0)
+    ($x2 $y1 0)
+    ($x1 $y1 0)
+    ($x0 $y1 0)
+
+    ($x0 $y0 0.1)
+    ($x1 $y0 0.1)
+    ($x2 $y0 0.1)
+    ($x3 $y0 0.1)
+
+    ($x3 $y1 0.1)
+    ($x2 $y1 0.1)
+    ($x1 $y1 0.1)
+    ($x0 $y1 0.1)
+);
+
+xSpacing ((0.5 0.5 5)(0.5 0.5 0.2));
+ySpacing ((1 0.5 0.25)(1 1 1)(1 0.5 4));
+
+
+blocks
+(
+    hex (0 1 6 7 8 9 14 15) (150 200 1) simpleGrading (1 $ySpacing 1)
+    hex (1 2 5 6 9 10 13 14) (150 200 1) simpleGrading ($xSpacing $ySpacing 1)
+    hex (2 3 4 5 10 11 12 13) (150 200 1) simpleGrading (1 $ySpacing 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+    top
+    {
+        type wall;
+        faces
+        (
+            (7 15 14 6)
+            (6 14 13 5)
+            (5 13 12 4)
+        );
+    }
+    bottom
+    {
+        type wall;
+        faces
+        (
+            (1 9 8 0)
+            (2 10 9 1)
+            (3 11 10 2)
+        );
+    }
+    left
+    {
+        type patch;
+        faces
+        (
+            (0 8 15 7)
+        );
+    }
+    right
+    {
+        type patch;
+        faces
+        (
+            (4 12 11 3)
+        );
+    }
+    frontAndBack
+    {
+        type empty;
+        faces
+        (
+            (0 7 6 1)
+            (1 6 5 2)
+            (2 5 4 3)
+
+            (8 9 14 15)
+            (9 10 13 14)
+            (10 11 12 13)
+        );
+    }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/system/controlDict

@@ -0,0 +1,69 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application       rhoPimpleAdiabaticFoam;
+
+startFrom         startTime;
+
+startTime         0;
+
+stopAt            endTime;
+
+endTime           0.22528;
+
+deltaT            3.2e-05;
+
+writeControl      timeStep;
+
+writeInterval     100;
+
+purgeWrite        0;
+
+writeFormat       binary;
+
+writePrecision    10;
+
+writeCompression  uncompressed;
+
+timeFormat        general;
+
+timePrecision     6;
+
+runTimeModifiable true;
+
+functions
+{
+    probes
+    {
+        type probes;
+
+        functionObjectLibs ("libsampling.so");
+
+        probeLocations
+        (
+            (3.0  2.0  0.0)
+            (3.0 -2.0  0.0)
+        );
+
+        fields
+        (
+            p
+        );
+    }
+}
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/system/decomposeParDict

@@ -0,0 +1,29 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 3;
+
+method          hierarchical;
+
+hierarchicalCoeffs
+{
+    n               (3 1 1);
+    delta           0.001;
+    order           xyz;
+}
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/system/fvSchemes

@@ -0,0 +1,54 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    // Note: setting coefficient to 1 for the rhoPimpleAdiabaticFoam solver
+    default         backward 1;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+    div(phi,U)      Gauss LUST grad(U);
+    div(phi,h)      Gauss LUST grad(h);
+    div(phi,K)      Gauss linear;
+    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         corrected;
+}
+
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/system/fvSolution

@@ -0,0 +1,59 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "(p|rho)"
+    {
+        solver          PCG;
+        preconditioner  DIC;
+        tolerance       1e-9;
+        relTol          0.01;
+        minIter         1;
+    }
+
+    "(p|rho)Final"
+    {
+        $p;
+        relTol          0;
+    }
+
+    "(U|e|h)"
+    {
+        solver          smoothSolver;
+        smoother        symGaussSeidel;
+        tolerance       1e-9;
+        relTol          0.01;
+    }
+
+    "(U|e|h)Final"
+    {
+        $U;
+        relTol          0;
+    }
+}
+
+PIMPLE
+{
+    momentumPredictor          yes;
+    nOuterCorrectors           1;
+    nCorrectors                2;
+    nNonOrthogonalCorrectors   0;
+}
+
+
+// ************************************************************************* //

tutorials/compressible/rhoPimpleAdiabaticFoam/rutlandVortex2D/system/preProcess

@@ -0,0 +1,91 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    system;
+    object      preProcess;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+functions
+{
+    createVortex
+    {
+        type            coded;
+        functionObjectLibs ("libutilityFunctionObjects.so");
+        redirectType    createVortices;
+        enabled         yes;
+
+        codeInclude
+        #{
+            #include "volFields.H"
+        #};
+
+        codeWrite
+        #{
+            scalar D = 0.57;
+            scalar UInf = 50;
+            scalar pInf = 101325;
+            scalar TInf = 224;
+            scalar gamma = 1.4;
+            scalar A = 0.3*D*UInf;
+            const dimensionedScalar rhoRef("rhoRef", dimDensity, 1);
+            const volScalarField& rho =
+                mesh().lookupObject<volScalarField>("rho");
+
+            const vectorField& C = mesh().C();
+            const scalarField x(C.component(0));
+            const scalarField y(C.component(1));
+            const scalar r2 = sqr(0.5*D/(Foam::sqrt(Foam::log(10.0))));
+            const scalarField Psi(A*exp(-0.5/r2*(sqr(x) + sqr(y))));
+
+            volVectorField* Uptr =
+                mesh().lookupObjectRefPtr<volVectorField>("U");
+            volScalarField* pPtr =
+                mesh().lookupObjectRefPtr<volScalarField>("p");
+            volScalarField* TPtr =
+                mesh().lookupObjectRefPtr<volScalarField>("T");
+
+
+            if (Uptr && pPtr && TPtr)
+            {
+                volVectorField& U = *Uptr;
+                volScalarField& p = *pPtr;
+                volScalarField& T = *TPtr;
+
+                vectorField& Uc = U.primitiveFieldRef();
+                Uc.replace(0, UInf - rhoRef/rho()*Psi/r2*y);
+                Uc.replace(1, rhoRef/rho()*Psi/r2*x);
+                U.correctBoundaryConditions();
+                U.write();
+
+                scalarField& pc = p.primitiveFieldRef();
+                pc = pInf - 0.5*sqr(rhoRef)/rho()*sqr(Psi)/r2;
+                p.correctBoundaryConditions();
+                p.write();
+
+                scalarField& Tc = T.primitiveFieldRef();
+                Tc = pow(pc/pInf, (gamma - 1)/gamma)*TInf;
+                T.correctBoundaryConditions();
+                T.write();
+            }
+            else
+            {
+                FatalErrorInFunction
+                    << "Unable to find pressure, velocity and temperature"
+                    << " fields" << exit(FatalError);
+            }
+        #};
+    }
+}
+
+
+// ************************************************************************* //