Added pimpleFoam to the collection.

applications/solvers/incompressible/pimpleFoam/Make/files

@@ -0,0 +1,3 @@
+pimpleFoam.C
+
+EXE = $(FOAM_USER_APPBIN)/pimpleFoam

applications/solvers/incompressible/pimpleFoam/Make/options

@@ -0,0 +1,10 @@
+EXE_INC = \
+    -I$(LIB_SRC)/finiteVolume/lnInclude \
+    -I$(LIB_SRC)/turbulenceModels/RAS \
+    -I$(LIB_SRC)/transportModels
+
+EXE_LIBS = \
+    -lincompressibleRASModels \
+    -lincompressibleTransportModels \
+    -lfiniteVolume \
+    -lmeshTools

applications/solvers/incompressible/pimpleFoam/UEqn.H

@@ -0,0 +1,36 @@
+// Solve the Momentum equation
+
+tmp<fvVectorMatrix> UEqn
+(
+    fvm::ddt(U)
+  + fvm::div(phi, U)
+  + turbulence->divDevReff(U)
+);
+
+if (oCorr == nOuterCorr-1)
+{
+    UEqn().relax(1);
+}
+else
+{
+    UEqn().relax();
+}
+
+volScalarField rUA = 1.0/UEqn().A();
+
+if (momentumPredictor)
+{
+    if (oCorr == nOuterCorr-1)
+    {
+        solve(UEqn() == -fvc::grad(p), mesh.solver("UFinal"));
+    }
+    else
+    {
+        solve(UEqn() == -fvc::grad(p));
+    }
+}
+else
+{
+    U = rUA*(UEqn().H() - fvc::grad(p));
+    U.correctBoundaryConditions();
+}

applications/solvers/incompressible/pimpleFoam/createFields.H

@@ -0,0 +1,42 @@
+Info<< "Reading field p\n" << endl;
+volScalarField p
+(
+    IOobject
+    (
+        "p",
+        runTime.timeName(),
+        mesh,
+        IOobject::MUST_READ,
+        IOobject::AUTO_WRITE
+    ),
+    mesh
+);
+
+Info<< "Reading field U\n" << endl;
+volVectorField U
+(
+    IOobject
+    (
+        "U",
+        runTime.timeName(),
+        mesh,
+        IOobject::MUST_READ,
+        IOobject::AUTO_WRITE
+    ),
+    mesh
+);
+
+#include "createPhi.H"
+
+
+label pRefCell = 0;
+scalar pRefValue = 0.0;
+setRefCell(p, mesh.solutionDict().subDict("PISO"), pRefCell, pRefValue);
+
+
+singlePhaseTransportModel laminarTransport(U, phi);
+
+autoPtr<incompressible::RASModel> turbulence
+(
+    incompressible::RASModel::New(U, phi, laminarTransport)
+);

applications/solvers/incompressible/pimpleFoam/pEqn.H

@@ -0,0 +1,53 @@
+U = rUA*UEqn().H();
+
+if (nCorr <= 1)
+{
+    UEqn.clear();
+}
+
+phi = (fvc::interpolate(U) & mesh.Sf())
+    + fvc::ddtPhiCorr(rUA, U, phi);
+
+adjustPhi(phi, U, p);
+
+// Non-orthogonal pressure corrector loop
+for (int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++)
+{
+    // Pressure corrector
+    fvScalarMatrix pEqn
+    (
+        fvm::laplacian(rUA, p) == fvc::div(phi)
+    );
+
+    pEqn.setReference(pRefCell, pRefValue);
+
+    if
+    (
+        oCorr == nOuterCorr-1
+     && corr == nCorr-1
+     && nonOrth == nNonOrthCorr
+    )
+    {
+        pEqn.solve(mesh.solver("pFinal"));
+    }
+    else
+    {
+        pEqn.solve();
+    }
+
+    if (nonOrth == nNonOrthCorr)
+    {
+        phi -= pEqn.flux();
+    }
+}
+
+#include "continuityErrs.H"
+
+// Explicitly relax pressure for momentum corrector except for last corrector
+if (oCorr != nOuterCorr-1)
+{
+    p.relax();
+}
+
+U -= rUA*fvc::grad(p);
+U.correctBoundaryConditions();

applications/solvers/incompressible/pimpleFoam/pimpleFoam.C

@@ -0,0 +1,93 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 1991-2007 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 2 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, write to the Free Software Foundation,
+    Inc., 51 Franklin St, Fifth Floor, Boston, MA 02110-1301 USA
+
+Application
+    pimpleFoam
+
+Description
+    Large time-step transient solver for incompressible, turbulent flow using
+    the PIMPLE (merged PISO-SIMPLE) algorithm.
+
+\*---------------------------------------------------------------------------*/
+
+#include "fvCFD.H"
+#include "incompressible/singlePhaseTransportModel/singlePhaseTransportModel.H"
+#include "incompressible/RASModel/RASModel.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+int main(int argc, char *argv[])
+{
+    #include "setRootCase.H"
+    #include "createTime.H"
+    #include "createMesh.H"
+    #include "createFields.H"
+    #include "initContinuityErrs.H"
+
+    Info<< "\nStarting time loop\n" << endl;
+
+    while (runTime.run())
+    {
+        #include "readTimeControls.H"
+        #include "readPIMPLEControls.H"
+        #include "CourantNo.H"
+        #include "setDeltaT.H"
+
+        runTime++;
+
+        Info<< "Time = " << runTime.timeName() << nl << endl;
+
+        if (nOuterCorr != 1)
+        {
+            p.storePrevIter();
+        }
+
+        // --- Pressure-velocity PIMPLE corrector loop
+        for (int oCorr=0; oCorr<nOuterCorr; oCorr++)
+        {
+            #include "UEqn.H"
+
+            // --- PISO loop
+            for (int corr=0; corr<nCorr; corr++)
+            {
+                #include "pEqn.H"
+            }
+
+            turbulence->correct();
+        }
+
+        runTime.write();
+
+        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
+            << "  ClockTime = " << runTime.elapsedClockTime() << " s"
+            << nl << endl;
+    }
+
+    Info<< "End\n" << endl;
+
+    return 0;
+}
+
+
+// ************************************************************************* //