From 5c58b07f5adaf09af4f04bce9332b1061f4337c8 Mon Sep 17 00:00:00 2001
From: sergio <sergio>
Date: Tue, 4 Jun 2019 12:18:13 -0700
Subject: [PATCH] ENH: Adding overBuoyantPimpleFoam and tutorial
---
.../overBuoyantPimpleFoam/Make/files | 3 +
.../overBuoyantPimpleFoam/Make/options | 30 +++
.../overBuoyantPimpleFoam/correctPhi.H | 91 ++++++++
.../overBuoyantPimpleFoam/createFieldRefs.H | 1 +
.../overBuoyantPimpleFoam/createFields.H | 126 +++++++++++
.../overBuoyantPimpleDyMFoam.C | 212 ++++++++++++++++++
.../overBuoyantPimpleFoam/pEqn.H | 130 +++++++++++
.../overBuoyantPimpleFoam/readControls.H | 9 +
.../overBuoyantPimpleFoam/0.orig/T | 57 +++++
.../overBuoyantPimpleFoam/0.orig/U | 60 +++++
.../overBuoyantPimpleFoam/0.orig/alphat | 61 +++++
.../overBuoyantPimpleFoam/0.orig/epsilon | 61 +++++
.../overBuoyantPimpleFoam/0.orig/k | 61 +++++
.../overBuoyantPimpleFoam/0.orig/nut | 61 +++++
.../overBuoyantPimpleFoam/0.orig/p | 60 +++++
.../overBuoyantPimpleFoam/0.orig/p_rgh | 61 +++++
.../0.orig/pointDisplacement | 63 ++++++
.../overBuoyantPimpleFoam/0.orig/zoneID | 57 +++++
.../overBuoyantPimpleFoam/Allclean | 10 +
.../heatTransfer/overBuoyantPimpleFoam/Allrun | 17 ++
.../overBuoyantPimpleFoam/Allrun.pre | 20 ++
.../constant/dynamicMeshDict | 39 ++++
.../overBuoyantPimpleFoam/constant/g | 22 ++
.../constant/thermophysicalProperties | 49 ++++
.../constant/turbulenceProperties | 28 +++
.../system/blockMeshDict | 122 ++++++++++
.../overBuoyantPimpleFoam/system/controlDict | 58 +++++
.../system/decomposeParDict | 30 +++
.../overBuoyantPimpleFoam/system/fvSchemes | 79 +++++++
.../overBuoyantPimpleFoam/system/fvSolution | 110 +++++++++
.../system/setFieldsDict | 48 ++++
.../overBuoyantPimpleFoam/system/topoSetDict | 69 ++++++
32 files changed, 1905 insertions(+)
create mode 100644 applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/Make/files
create mode 100644 applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/Make/options
create mode 100644 applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/correctPhi.H
create mode 100644 applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/createFieldRefs.H
create mode 100644 applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/createFields.H
create mode 100644 applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/overBuoyantPimpleDyMFoam.C
create mode 100644 applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/pEqn.H
create mode 100644 applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/readControls.H
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/T
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/U
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/alphat
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/epsilon
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/k
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/nut
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/p
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/p_rgh
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/pointDisplacement
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/zoneID
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/Allclean
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/Allrun
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/Allrun.pre
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/constant/dynamicMeshDict
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/constant/g
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/constant/thermophysicalProperties
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/constant/turbulenceProperties
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/system/blockMeshDict
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/system/controlDict
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/system/decomposeParDict
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/system/fvSchemes
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/system/fvSolution
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/system/setFieldsDict
create mode 100755 tutorials/heatTransfer/overBuoyantPimpleFoam/system/topoSetDict
diff --git a/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/Make/files b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/Make/files
new file mode 100644
index 00000000000..3ba66e45f6a
--- /dev/null
+++ b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/Make/files
@@ -0,0 +1,3 @@
+overBuoyantPimpleDyMFoam.C
+
+EXE = $(FOAM_APPBIN)/overBuoyantPimpleDyMFoam
diff --git a/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/Make/options b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/Make/options
new file mode 100644
index 00000000000..1c97aae0837
--- /dev/null
+++ b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/Make/options
@@ -0,0 +1,30 @@
+EXE_INC = \
+ -I$(FOAM_SOLVERS)/heatTransfer/buoyantPimpleFoam \
+ -I$(FOAM_SOLVERS)/compressible/rhoPimpleFoam/overRhoPimpleDyMFoam \
+ -I$(LIB_SRC)/finiteVolume/lnInclude \
+ -I$(LIB_SRC)/sampling/lnInclude \
+ -I$(LIB_SRC)/dynamicFvMesh/lnInclude \
+ -I$(LIB_SRC)/dynamicMesh/lnInclude \
+ -I$(LIB_SRC)/overset/lnInclude \
+ -I$(LIB_SRC)/meshTools/lnInclude \
+ -I$(LIB_SRC)/transportModels/compressible/lnInclude \
+ -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
+ -I$(LIB_SRC)/thermophysicalModels/radiation/lnInclude \
+ -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
+ -I$(LIB_SRC)/TurbulenceModels/compressible/lnInclude
+
+EXE_LIBS = \
+ -lfiniteVolume \
+ -lsampling \
+ -lmeshTools \
+ -lfvOptions \
+ -lcompressibleTransportModels \
+ -lfluidThermophysicalModels \
+ -lradiationModels \
+ -lspecie \
+ -lturbulenceModels \
+ -lcompressibleTurbulenceModels \
+ -latmosphericModels \
+ -loverset \
+ -ldynamicFvMesh \
+ -ltopoChangerFvMesh
diff --git a/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/correctPhi.H b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/correctPhi.H
new file mode 100644
index 00000000000..a49eebc7ea5
--- /dev/null
+++ b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/correctPhi.H
@@ -0,0 +1,91 @@
+if (mesh.changing())
+{
+ volVectorField::Boundary& bfld = U.boundaryFieldRef();
+ forAll(bfld, patchi)
+ {
+ if (bfld[patchi].fixesValue())
+ {
+ bfld[patchi].initEvaluate();
+ }
+ }
+
+ surfaceScalarField::Boundary& phiBfld = phi.boundaryFieldRef();
+ forAll(bfld, patchi)
+ {
+ if (bfld[patchi].fixesValue())
+ {
+ bfld[patchi].evaluate();
+
+ phiBfld[patchi] =
+ rho.boundaryField()[patchi]
+ * (
+ bfld[patchi]
+ & mesh.Sf().boundaryField()[patchi]
+ );
+ }
+ }
+}
+ // Initialize BCs list for pcorr to zero-gradient
+ wordList pcorrTypes
+ (
+ p.boundaryField().size(),
+ zeroGradientFvPatchScalarField::typeName
+ );
+
+ // Set BCs of pcorr to fixed-value for patches at which p is fixed
+ forAll(p.boundaryField(), patchi)
+ {
+ if (p.boundaryField()[patchi].fixesValue())
+ {
+ pcorrTypes[patchi] = fixedValueFvPatchScalarField::typeName;
+ }
+ }
+
+ volScalarField pcorr
+ (
+ IOobject
+ (
+ "pcorr",
+ runTime.timeName(),
+ mesh,
+ IOobject::NO_READ,
+ IOobject::NO_WRITE
+ ),
+ mesh,
+ dimensionedScalar(p.dimensions(), Zero),
+ pcorrTypes
+ );
+
+ mesh.setFluxRequired(pcorr.name());
+
+{
+ dimensionedScalar rAUf("rAUf", dimTime, 1.0);
+
+ while (pimple.correctNonOrthogonal())
+ {
+ fvScalarMatrix pcorrEqn
+ (
+ fvm::ddt(psi, pcorr)
+ + fvc::div(phi)
+ - fvm::laplacian(rAUf, pcorr)
+ ==
+ divrhoU()
+ );
+
+ //pcorrEqn.solve(mesh.solver(pcorr.select(pimple.finalInnerIter())));
+ //Bypass virtual layer
+ const dictionary& d = mesh.solver
+ (
+ pcorr.select
+ (
+ pimple.finalInnerIter()
+ )
+ );
+ mesh.fvMesh::solve(pcorrEqn, d);
+
+ if (pimple.finalNonOrthogonalIter())
+ {
+ phi += pcorrEqn.flux();
+ }
+ }
+}
diff --git a/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/createFieldRefs.H b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/createFieldRefs.H
new file mode 100644
index 00000000000..502b3b42300
--- /dev/null
+++ b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/createFieldRefs.H
@@ -0,0 +1 @@
+const volScalarField& psi = thermo.psi();
diff --git a/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/createFields.H b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/createFields.H
new file mode 100644
index 00000000000..4c203d0266a
--- /dev/null
+++ b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/createFields.H
@@ -0,0 +1,126 @@
+Info<< "Reading thermophysical properties\n" << endl;
+
+autoPtr<rhoThermo> pThermo(rhoThermo::New(mesh));
+rhoThermo& thermo = pThermo();
+thermo.validate(args.executable(), "h", "e");
+
+volScalarField rho
+(
+ IOobject
+ (
+ "rho",
+ runTime.timeName(),
+ mesh,
+ IOobject::NO_READ,
+ IOobject::NO_WRITE
+ ),
+ thermo.rho()
+);
+
+volScalarField& p = thermo.p();
+
+Info<< "Reading field U\n" << endl;
+volVectorField U
+(
+ IOobject
+ (
+ "U",
+ runTime.timeName(),
+ mesh,
+ IOobject::MUST_READ,
+ IOobject::AUTO_WRITE
+ ),
+ mesh
+);
+
+#include "compressibleCreatePhi.H"
+
+
+Info<< "Creating turbulence model\n" << endl;
+autoPtr<compressible::turbulenceModel> turbulence
+(
+ compressible::turbulenceModel::New
+ (
+ rho,
+ U,
+ phi,
+ thermo
+ )
+);
+
+
+#include "readGravitationalAcceleration.H"
+#include "readhRef.H"
+#include "gh.H"
+
+
+Info<< "Reading field p_rgh\n" << endl;
+volScalarField p_rgh
+(
+ IOobject
+ (
+ "p_rgh",
+ runTime.timeName(),
+ mesh,
+ IOobject::MUST_READ,
+ IOobject::AUTO_WRITE
+ ),
+ mesh
+);
+
+// Force p_rgh to be consistent with p
+p_rgh = p - rho*gh;
+
+mesh.setFluxRequired(p_rgh.name());
+
+label pRefCell = 0;
+scalar pRefValue = 0.0;
+
+if (p_rgh.needReference())
+{
+ setRefCell
+ (
+ p,
+ p_rgh,
+ pimple.dict(),
+ pRefCell,
+ pRefValue
+ );
+
+ p += dimensionedScalar
+ (
+ "p",
+ p.dimensions(),
+ pRefValue - getRefCellValue(p, pRefCell)
+ );
+}
+
+dimensionedScalar initialMass("initialMass", fvc::domainIntegrate(rho));
+
+#include "createDpdt.H"
+
+#include "createK.H"
+
+#include "createMRF.H"
+#include "createRadiationModel.H"
+#include "createFvOptions.H"
+
+//- Overset specific
+
+// Add solver-specific interpolations
+{
+ wordHashSet& nonInt =
+ const_cast<wordHashSet&>(Stencil::New(mesh).nonInterpolatedFields());
+
+ nonInt.insert("HbyA");
+ nonInt.insert("grad(p_rgh)");
+ nonInt.insert("surfaceIntegrate(phi)");
+ nonInt.insert("surfaceIntegrate(phiHbyA)");
+ nonInt.insert("cellMask");
+ nonInt.insert("cellDisplacement");
+ nonInt.insert("interpolatedCells");
+ nonInt.insert("cellInterpolationWeight");
+}
+
+// Mask field for zeroing out contributions on hole cells
+#include "createCellMask.H"
diff --git a/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/overBuoyantPimpleDyMFoam.C b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/overBuoyantPimpleDyMFoam.C
new file mode 100644
index 00000000000..329fa7bcb82
--- /dev/null
+++ b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/overBuoyantPimpleDyMFoam.C
@@ -0,0 +1,212 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2019 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
+ overBuoyantPimpleDymFoam
+
+Group
+ grpHeatTransferSolvers
+
+Description
+ Transient solver for buoyant, turbulent flow of compressible fluids for
+ ventilation and heat-transfer with overset feature
+
+ Turbulence is modelled using a run-time selectable compressible RAS or
+ LES model.
+
+\*---------------------------------------------------------------------------*/
+
+#include "fvCFD.H"
+#include "dynamicFvMesh.H"
+#include "rhoThermo.H"
+#include "turbulentFluidThermoModel.H"
+#include "radiationModel.H"
+#include "fvOptions.H"
+#include "pimpleControl.H"
+#include "pressureControl.H"
+
+#include "CorrectPhi.H"
+#include "cellCellStencilObject.H"
+#include "localMin.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+int main(int argc, char *argv[])
+{
+ argList::addNote
+ (
+ "Transient solver for buoyant, turbulent fluid flow"
+ " of compressible fluids, including radiation."
+ );
+
+ #include "postProcess.H"
+
+ #include "addCheckCaseOptions.H"
+ #include "setRootCaseLists.H"
+ #include "createTime.H"
+ #include "createDynamicFvMesh.H"
+ #include "createDyMControls.H"
+ #include "createFields.H"
+ #include "createFieldRefs.H"
+ #include "initContinuityErrs.H"
+
+ #include "createRhoUfIfPresent.H"
+ #include "createControls.H"
+
+ #include "compressibleCourantNo.H"
+ #include "setInitialDeltaT.H"
+
+ turbulence->validate();
+
+ // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ Info<< "\nStarting time loop\n" << endl;
+
+ while (runTime.run())
+ {
+ #include "readTimeControls.H"
+
+ #include "readControls.H"
+ #include "readDyMControls.H"
+
+ #include "compressibleCourantNo.H"
+ #include "setDeltaT.H"
+
+ // Store divrhoU from the previous mesh so that it can be mapped
+ // and used in correctPhi to ensure the corrected phi has the
+ // same divergence
+ autoPtr<volScalarField> divrhoU;
+ if (correctPhi)
+ {
+ divrhoU.reset
+ (
+ new volScalarField
+ (
+ "divrhoU",
+ fvc::div(fvc::absolute(phi, rho, U))
+ )
+ );
+ }
+
+
+ ++runTime;
+
+ Info<< "Time = " << runTime.timeName() << nl << endl;
+
+ // --- Pressure-velocity PIMPLE corrector loop
+ while (pimple.loop())
+ {
+ if (pimple.firstIter() || moveMeshOuterCorrectors)
+ {
+ // Do any mesh changes
+ mesh.update();
+
+ if (mesh.changing())
+ {
+ MRF.update();
+
+ #include "setCellMask.H"
+
+ const surfaceScalarField faceMaskOld
+ (
+ localMin<scalar>(mesh).interpolate(cellMask.oldTime())
+ );
+
+ // Zero Uf on old faceMask (H-I)
+ rhoUf() *= faceMaskOld;
+
+ //fvc::correctRhoUf(rhoUfint, rho, U, phi);
+ surfaceVectorField rhoUfint(fvc::interpolate(rho*U));
+
+ // Update Uf and phi on new C-I faces
+ rhoUf() += (1-faceMaskOld)*rhoUfint;
+
+ // Update Uf boundary
+ forAll(rhoUf().boundaryField(), patchI)
+ {
+ rhoUf().boundaryFieldRef()[patchI] =
+ rhoUfint.boundaryField()[patchI];
+ }
+
+ // Calculate absolute flux from the mapped surface velocity
+ phi = mesh.Sf() & rhoUf();
+
+ if (correctPhi)
+ {
+ #include "correctPhi.H"
+ }
+
+ // Zero phi on current H-I
+ const surfaceScalarField faceMask
+ (
+ localMin<scalar>(mesh).interpolate(cellMask)
+ );
+
+ phi *= faceMask;
+ U *= cellMask;
+
+ // Make the fluxes relative to the mesh-motion
+ fvc::makeRelative(phi, rho, U);
+ }
+
+ if (checkMeshCourantNo)
+ {
+ #include "meshCourantNo.H"
+ }
+ }
+
+ if (pimple.firstIter())
+ {
+ #include "rhoEqn.H"
+ }
+
+ #include "UEqn.H"
+ #include "EEqn.H"
+
+ // --- Pressure corrector loop
+ while (pimple.correct())
+ {
+ #include "pEqn.H"
+ }
+
+ if (pimple.turbCorr())
+ {
+ turbulence->correct();
+ }
+ }
+
+ rho = thermo.rho();
+
+ runTime.write();
+
+ runTime.printExecutionTime(Info);
+ }
+
+ Info<< "End\n" << endl;
+
+ return 0;
+}
+
+
+// ************************************************************************* //
diff --git a/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/pEqn.H b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/pEqn.H
new file mode 100644
index 00000000000..854b4418d89
--- /dev/null
+++ b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/pEqn.H
@@ -0,0 +1,130 @@
+
+dimensionedScalar compressibility = fvc::domainIntegrate(psi);
+bool compressible = (compressibility.value() > SMALL);
+
+rho = thermo.rho();
+
+// Thermodynamic density needs to be updated by psi*d(p) after the
+// pressure solution
+const volScalarField psip0(psi*p);
+
+volScalarField rAU(1.0/UEqn.A());
+mesh.interpolate(rAU);
+
+surfaceScalarField rhorAUf("rhorAUf", fvc::interpolate(rho*rAU));
+volVectorField HbyA(constrainHbyA(rAU*UEqn.H(), U, p_rgh));
+
+surfaceScalarField phig(-rhorAUf*ghf*fvc::snGrad(rho)*mesh.magSf());
+
+surfaceScalarField phiHbyA
+(
+ "phiHbyA",
+ fvc::flux(rho*HbyA) + phig
+);
+
+if (ddtCorr)
+{
+ surfaceScalarField faceMaskOld
+ (
+ localMin<scalar>(mesh).interpolate(cellMask.oldTime())
+ );
+
+ phiHbyA +=
+ faceMaskOld*MRF.zeroFilter(rhorAUf*fvc::ddtCorr(rho, U, phi));
+}
+
+MRF.makeRelative(fvc::interpolate(rho), phiHbyA);
+
+// Update the pressure BCs to ensure flux consistency
+constrainPressure(p_rgh, rho, U, phiHbyA, rhorAUf, MRF);
+
+fvScalarMatrix p_rghDDtEqn
+(
+ fvc::ddt(rho) + psi*correction(fvm::ddt(p_rgh))
+ + fvc::div(phiHbyA)
+ ==
+ fvOptions(psi, p_rgh, rho.name())
+);
+
+while (pimple.correctNonOrthogonal())
+{
+ fvScalarMatrix p_rghEqn
+ (
+ p_rghDDtEqn
+ - fvm::laplacian(rhorAUf, p_rgh)
+ );
+
+ p_rghEqn.solve(mesh.solver(p_rgh.select(pimple.finalInnerIter())));
+
+ if (pimple.finalNonOrthogonalIter())
+ {
+ // Calculate the conservative fluxes
+ phi = phiHbyA + p_rghEqn.flux();
+
+ // Explicitly relax pressure for momentum corrector
+ p_rgh.relax();
+
+ // Correct the momentum source with the pressure gradient flux
+ // calculated from the relaxed pressure
+ U =
+ cellMask*
+ (
+ HbyA + rAU*fvc::reconstruct((phig + p_rghEqn.flux())/rhorAUf)
+ );
+ U.correctBoundaryConditions();
+ fvOptions.correct(U);
+ K = 0.5*magSqr(U);
+ }
+}
+
+p = p_rgh + rho*gh;
+
+#include "rhoEqn.H"
+#include "compressibleContinuityErrs.H"
+
+if (p_rgh.needReference())
+{
+ if (!compressible)
+ {
+ p += dimensionedScalar
+ (
+ "p",
+ p.dimensions(),
+ pRefValue - getRefCellValue(p, pRefCell)
+ );
+ }
+ else
+ {
+ p += (initialMass - fvc::domainIntegrate(psi*p))
+ /compressibility;
+ thermo.correctRho(psi*p - psip0);
+ rho = thermo.rho();
+ p_rgh = p - rho*gh;
+ }
+}
+else
+{
+ thermo.correctRho(psi*p - psip0);
+}
+
+rho = thermo.rho();
+
+{
+ fvc::correctRhoUf(rhoUf, rho, U, phi);
+}
+
+if (thermo.dpdt())
+{
+ dpdt = fvc::ddt(p);
+
+ if (mesh.moving())
+ {
+ dpdt -= fvc::div(fvc::meshPhi(rho, U), p);
+ }
+}
+
+surfaceScalarField faceMask
+(
+ localMin<scalar>(mesh).interpolate(cellMask)
+);
+phi *= faceMask;
diff --git a/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/readControls.H b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/readControls.H
new file mode 100644
index 00000000000..8f43318cabe
--- /dev/null
+++ b/applications/solvers/heatTransfer/buoyantPimpleFoam/overBuoyantPimpleFoam/readControls.H
@@ -0,0 +1,9 @@
+#include "readTimeControls.H"
+
+correctPhi = pimple.dict().lookupOrDefault("correctPhi", false);
+
+checkMeshCourantNo =
+ pimple.dict().lookupOrDefault("checkMeshCourantNo", false);
+
+
+ddtCorr = pimple.dict().lookupOrDefault("ddtCorr", true);
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/T b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/T
new file mode 100755
index 00000000000..476b66adb64
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/T
@@ -0,0 +1,57 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 0 0 1 0 0 0];
+
+
+internalField uniform 300;
+
+boundaryField
+{
+ overset1
+ {
+ type overset;
+ }
+ walls
+ {
+ type zeroGradient;
+ }
+ inlet
+ {
+ type zeroGradient;
+ }
+ outlet
+ {
+ type zeroGradient;
+ }
+ hole
+ {
+ type fixedValue;
+ value uniform 400;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+ frontAndBack1
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/U b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/U
new file mode 100755
index 00000000000..57a41f946fb
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/U
@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ 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
+{
+ overset1
+ {
+ type overset;
+ }
+ walls
+ {
+ type uniformFixedValue;
+ uniformValue uniform (0 0 0);
+ }
+ inlet
+ {
+ type uniformFixedValue;
+ uniformValue uniform (0 0 0);
+ }
+ outlet
+ {
+ type uniformFixedValue;
+ uniformValue uniform (0 0 0);
+ }
+ hole
+ {
+ type movingWallVelocity;
+ value uniform (0 0 0);
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+ frontAndBack1
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/alphat b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/alphat
new file mode 100755
index 00000000000..ab6b28d14fc
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/alphat
@@ -0,0 +1,61 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object alphat;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -1 0 0 0 0];
+
+
+internalField uniform 0;
+
+boundaryField
+{
+ overset1
+ {
+ type overset;
+ value uniform 0;
+ }
+ walls
+ {
+ type compressible::alphatWallFunction;
+ value uniform 0;
+ }
+ inlet
+ {
+ type compressible::alphatWallFunction;
+ value uniform 0;
+ }
+ outlet
+ {
+ type compressible::alphatWallFunction;
+ value uniform 0;
+ }
+ hole
+ {
+ type compressible::alphatWallFunction;
+ value uniform 0;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+ frontAndBack1
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/epsilon b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/epsilon
new file mode 100755
index 00000000000..62b26d4b23a
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/epsilon
@@ -0,0 +1,61 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object epsilon;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 2 -3 0 0 0 0];
+
+
+internalField uniform 0.1;
+
+boundaryField
+{
+ overset1
+ {
+ type overset;
+ value uniform 0.1;
+ }
+ walls
+ {
+ type epsilonWallFunction;
+ value uniform 0.1;
+ }
+ inlet
+ {
+ type epsilonWallFunction;
+ value uniform 0.1;
+ }
+ outlet
+ {
+ type epsilonWallFunction;
+ value uniform 0.1;
+ }
+ hole
+ {
+ type epsilonWallFunction;
+ value uniform 0.1;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+ frontAndBack1
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/k b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/k
new file mode 100755
index 00000000000..3fbc2d9b89f
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/k
@@ -0,0 +1,61 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 2 -2 0 0 0 0];
+
+
+internalField uniform 0.01;
+
+boundaryField
+{
+ overset1
+ {
+ type overset;
+ value uniform 0.01;
+ }
+ walls
+ {
+ type kqRWallFunction;
+ value uniform 0.01;
+ }
+ inlet
+ {
+ type kqRWallFunction;
+ value uniform 0.01;
+ }
+ outlet
+ {
+ type kqRWallFunction;
+ value uniform 0.01;
+ }
+ hole
+ {
+ type kqRWallFunction;
+ value uniform 0.01;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+ frontAndBack1
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/nut b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/nut
new file mode 100755
index 00000000000..b76fdda7af1
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/nut
@@ -0,0 +1,61 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object nut;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 2 -1 0 0 0 0];
+
+
+internalField uniform 0;
+
+boundaryField
+{
+ overset1
+ {
+ type overset;
+ value uniform 0;
+ }
+ walls
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ inlet
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ outlet
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ hole
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+ frontAndBack1
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/p b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/p
new file mode 100755
index 00000000000..4da47078823
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/p
@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -2 0 0 0 0];
+
+
+internalField uniform 100000;
+
+boundaryField
+{
+ overset1
+ {
+ type overset;
+ }
+ walls
+ {
+ type calculated;
+ value uniform 100000;
+ }
+ inlet
+ {
+ type calculated;
+ value uniform 100000;
+ }
+ outlet
+ {
+ type calculated;
+ value uniform 100000;
+ }
+ hole
+ {
+ type calculated;
+ value uniform 100000;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+ frontAndBack1
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/p_rgh b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/p_rgh
new file mode 100755
index 00000000000..ffb7949e836
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/p_rgh
@@ -0,0 +1,61 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -2 0 0 0 0];
+
+
+internalField uniform 100000;
+
+boundaryField
+{
+ overset1
+ {
+ type overset;
+ value uniform 100000;
+ }
+ walls
+ {
+ type fixedFluxPressure;
+ value uniform 100000;
+ }
+ inlet
+ {
+ type fixedFluxPressure;
+ value uniform 100000;
+ }
+ outlet
+ {
+ type fixedFluxPressure;
+ value uniform 100000;
+ }
+ hole
+ {
+ type fixedFluxPressure;
+ value uniform 100000;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+ frontAndBack1
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/pointDisplacement b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/pointDisplacement
new file mode 100755
index 00000000000..9566eccf905
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/pointDisplacement
@@ -0,0 +1,63 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class pointVectorField;
+ location "0";
+ object pointDisplacement;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 0 0 0 0 0];
+
+
+internalField uniform (0 0 0);
+
+boundaryField
+{
+ overset1
+ {
+ type zeroGradient;
+ patchType overset;
+ }
+ walls
+ {
+ type uniformFixedValue;
+ value uniform (0 0 0);
+ uniformValue constant (0 0 0);
+ }
+ inlet
+ {
+ type uniformFixedValue;
+ value uniform (0 0 0);
+ uniformValue constant (0 0 0);
+ }
+ outlet
+ {
+ type uniformFixedValue;
+ value uniform (0 0 0);
+ uniformValue constant (0 0 0);
+ }
+ hole
+ {
+ type zeroGradient;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+ frontAndBack1
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/zoneID b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/zoneID
new file mode 100755
index 00000000000..374c2ca4578
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/0.orig/zoneID
@@ -0,0 +1,57 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object zoneID;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 0 0 0 0 0 0];
+
+
+internalField uniform 0;
+
+boundaryField
+{
+ overset1
+ {
+ type overset;
+ value uniform 1;
+ }
+ walls
+ {
+ type zeroGradient;
+ }
+ inlet
+ {
+ type zeroGradient;
+ }
+ outlet
+ {
+ type zeroGradient;
+ }
+ hole
+ {
+ type zeroGradient;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+ frontAndBack1
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/Allclean b/tutorials/heatTransfer/overBuoyantPimpleFoam/Allclean
new file mode 100755
index 00000000000..fad073e1431
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/Allclean
@@ -0,0 +1,10 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions # Tutorial clean functions
+
+cleanCase0
+
+rm -f constant/polyMesh/boundary
+rm -f constant/polyMesh/zoneID
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/Allrun b/tutorials/heatTransfer/overBuoyantPimpleFoam/Allrun
new file mode 100755
index 00000000000..ad941f4ac5a
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/Allrun
@@ -0,0 +1,17 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/RunFunctions # Tutorial run functions
+
+./Allrun.pre
+
+# Serial
+runApplication $(getApplication)
+
+# Parallel
+#runApplication decomposePar -cellDist
+#runParallel $(getApplication)
+
+#post
+runApplication foamToVTK
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/Allrun.pre b/tutorials/heatTransfer/overBuoyantPimpleFoam/Allrun.pre
new file mode 100755
index 00000000000..abccd3163c9
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/Allrun.pre
@@ -0,0 +1,20 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/RunFunctions # Tutorial run functions
+
+runApplication blockMesh
+
+# Select cellSets
+runApplication -s 1 topoSet
+
+runApplication subsetMesh box -patch hole -overwrite
+
+# Select cellSets
+runApplication -s 2 topoSet
+
+restore0Dir
+
+# Use cellSets to write zoneID
+runApplication setFields
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/dynamicMeshDict b/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/dynamicMeshDict
new file mode 100755
index 00000000000..9e47aa2c1c1
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/dynamicMeshDict
@@ -0,0 +1,39 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus-overset |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object dynamicMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dynamicFvMesh dynamicOversetFvMesh;
+
+dynamicOversetFvMeshCoeffs
+{
+// layerRelax 0.3;
+}
+
+solver multiSolidBodyMotionSolver;
+
+multiSolidBodyMotionSolverCoeffs
+{
+ movingZone1
+ {
+ solidBodyMotionFunction oscillatingLinearMotion;
+ oscillatingLinearMotionCoeffs
+ {
+ amplitude (0.035 0 0);
+ omega 2.094395;
+ }
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/g b/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/g
new file mode 100755
index 00000000000..14b9f5393e5
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/g
@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class uniformDimensionedVectorField;
+ location "constant";
+ object g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -2 0 0 0 0];
+value (0 -9.81 0);
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/thermophysicalProperties b/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/thermophysicalProperties
new file mode 100755
index 00000000000..7dd52e2b0d6
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/thermophysicalProperties
@@ -0,0 +1,49 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object thermophysicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+ type heRhoThermo;
+ mixture pureMixture;
+ transport sutherland;
+ thermo hConst;
+ equationOfState perfectGas;
+ specie specie;
+ energy sensibleEnthalpy;
+}
+
+mixture
+{
+ specie
+ {
+ molWeight 28.9;
+ }
+ thermodynamics
+ {
+ Cp 1007;
+ Hf 0;
+ }
+ transport
+ {
+ As 1.4792e-06;
+ Ts 116;
+ }
+}
+
+dpdt true;
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/turbulenceProperties b/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/turbulenceProperties
new file mode 100755
index 00000000000..58cf4dbc885
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/constant/turbulenceProperties
@@ -0,0 +1,28 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType laminar;
+
+RAS
+{
+ RASModel kEpsilon;
+
+ turbulence on;
+
+ printCoeffs on;
+}
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/system/blockMeshDict b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/blockMeshDict
new file mode 100755
index 00000000000..1a61ee13c52
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/blockMeshDict
@@ -0,0 +1,122 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+scale 0.001;
+
+vertices
+(
+ ( -2.00 0.0 0)
+ ( 107.00 0.0 0)
+ ( 107.00 45.0 0)
+ ( -2.00 45.0 0)
+ ( -2.00 0.0 10)
+ ( 107.00 0.0 10)
+ ( 107.00 45.0 10)
+ ( -2.00 45.0 10)
+
+ // movingZone1
+ ( 44.5 5.0 0)
+ ( 60.5 5.0 0)
+ ( 60.5 40.0 0)
+ ( 44.5 40.0 0)
+ ( 44.5 5.0 10)
+ ( 60.5 5.0 10)
+ ( 60.5 40.0 10)
+ ( 44.5 40.0 10)
+);
+
+blocks
+(
+ hex (0 1 2 3 4 5 6 7) (109 55 1) simpleGrading (1 1 1)
+ hex (8 9 10 11 12 13 14 15) movingZone1 (16 48 1) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+ overset1
+ {
+ type overset;
+ faces
+ (
+ ( 8 12 15 11)
+ (10 14 13 9)
+ (11 15 14 10)
+ ( 9 13 12 8)
+ );
+ }
+
+
+ walls
+ {
+ type wall;
+ faces
+ (
+ (3 7 6 2)
+ (1 5 4 0)
+ );
+ }
+
+ inlet
+ {
+ type wall;
+ faces
+ (
+ (0 4 7 3)
+ );
+ }
+
+ outlet
+ {
+ type wall;
+ faces
+ (
+ (2 6 5 1)
+ );
+ }
+
+ // Populated by subsetMesh
+ hole
+ {
+ type wall;
+ faces ();
+ }
+
+ frontAndBack
+ {
+ type empty;
+ faces
+ (
+ (0 3 2 1)
+ (4 5 6 7)
+ );
+ }
+
+ frontAndBack1
+ {
+ type empty;
+ faces
+ (
+ ( 8 11 10 9)
+ (12 13 14 15)
+ );
+ }
+);
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/system/controlDict b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/controlDict
new file mode 100755
index 00000000000..da8c0a38d4e
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/controlDict
@@ -0,0 +1,58 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+DebugSwitches
+{
+ overset 0;
+ dynamicOversetFvMesh 0;
+ cellVolumeWeight 0;
+}
+
+application overBuoyantPimpleDyMFoam;
+
+startFrom startTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 1.5;
+
+deltaT 0.001;
+
+writeControl adjustableRunTime;
+
+writeInterval 0.05;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 10;
+
+writeCompression off;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable true;
+
+adjustTimeStep no;
+
+maxCo 1;
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/system/decomposeParDict b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/decomposeParDict
new file mode 100755
index 00000000000..daf891ae5af
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/decomposeParDict
@@ -0,0 +1,30 @@
+/*--------------------------------*- 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;
+ note "mesh decomposition control dictionary";
+ object decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 4;
+
+
+method scotch;
+
+hierarchicalCoeffs
+{
+ n (2 1 1);
+ delta 0.001;
+ order xyz;
+}
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/system/fvSchemes b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/fvSchemes
new file mode 100755
index 00000000000..322d3343c6f
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/fvSchemes
@@ -0,0 +1,79 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default Euler;
+}
+
+gradSchemes
+{
+ default Gauss linear;
+}
+
+divSchemes
+{
+ default none;
+ div(phi,U) Gauss upwind;
+
+ div(phi,epsilon) Gauss limitedLinear 1;
+ div(phi,k) Gauss limitedLinear 1;
+ div(phi,h) Gauss limitedLinear 1;
+ div(phi,K) Gauss linear;
+
+ div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+ div(meshPhi,p) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear corrected;
+ laplacian(diffusivity,cellDisplacement) Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default corrected;
+}
+
+oversetInterpolation
+{
+ method cellVolumeWeight;
+ //method inverseDistance;
+
+ searchBox (-0.002 0 0)(0.107 0.5 0.01);
+ searchBoxDivisions (200 200 1);
+}
+
+fluxRequired
+{
+ default no;
+ pcorr ;
+ p ;
+}
+
+oversetInterpolationSuppressed
+{
+ grad(p_rgh);
+ surfaceIntegrate(phiHbyA);
+}
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/system/fvSolution b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/fvSolution
new file mode 100755
index 00000000000..57a735b1880
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/fvSolution
@@ -0,0 +1,110 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ cellDisplacement
+ {
+ solver PCG;
+ preconditioner DIC;
+
+ tolerance 1e-06;
+ relTol 0;
+ maxIter 100;
+ }
+
+ "(rho|h)"
+ {
+ solver PBiCGStab;
+ preconditioner DILU;
+ tolerance 1e-8;
+ relTol 0.1;
+ }
+
+ "(rho|h)Final"
+ {
+ $rho;
+ tolerance 1e-8;
+ relTol 0;
+ }
+
+ p_rgh
+ {
+ solver PBiCGStab;
+ preconditioner DILU;
+ tolerance 1e-11;
+ relTol 0.01;
+ }
+
+ p_rghFinal
+ {
+ $p_rgh;
+ relTol 0;
+ }
+
+ pcorr
+ {
+ $p_rghFinal;
+ preconditioner DIC;
+ }
+
+ pcorrFinal
+ {
+ $pcorr;
+ relTol 0;
+ }
+
+ "(U|k|epsilon)"
+ {
+ solver smoothSolver;
+ smoother symGaussSeidel;
+ tolerance 1e-6;
+ relTol 0;
+ }
+
+ "(U|k|epsilon)Final"
+ {
+ $U;
+ tolerance 1e-6;
+ relTol 0;
+ }
+}
+
+PIMPLE
+{
+ momentumPredictor true;
+ correctPhi false;
+ checkMeshCourantNo yes;
+ nOuterCorrectors 1;
+ nCorrectors 4;
+ nNonOrthogonalCorrectors 0;
+ ddtCorr true;
+ pRefCell 0;
+ pRefValue 1e5;
+}
+
+relaxationFactors
+{
+ fields
+ {
+ }
+ equations
+ {
+ ".*" 1;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/system/setFieldsDict b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/setFieldsDict
new file mode 100755
index 00000000000..3f6cb9534fd
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/setFieldsDict
@@ -0,0 +1,48 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+defaultFieldValues
+(
+ volScalarFieldValue zoneID 123
+);
+
+regions
+(
+ // Set cell values
+ // (does zerogradient on boundaries)
+ cellToCell
+ {
+ set c0;
+
+ fieldValues
+ (
+ volScalarFieldValue zoneID 0
+ );
+ }
+
+ cellToCell
+ {
+ set c1;
+
+ fieldValues
+ (
+ volScalarFieldValue zoneID 1
+ );
+ }
+
+);
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/overBuoyantPimpleFoam/system/topoSetDict b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/topoSetDict
new file mode 100755
index 00000000000..d824673724b
--- /dev/null
+++ b/tutorials/heatTransfer/overBuoyantPimpleFoam/system/topoSetDict
@@ -0,0 +1,69 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1812 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object topoSetDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+actions
+(
+ {
+ name c0;
+ type cellSet;
+ action new;
+ source regionToCell;
+ insidePoints ((0.0001 0.0001 0.0001));
+ }
+
+ {
+ name c1;
+ type cellSet;
+ action new;
+ source cellToCell;
+ set c0;
+ }
+
+ {
+ name c1;
+ type cellSet;
+ action invert;
+ }
+
+ // Select box to remove from region 1 and 2
+
+ {
+ name box;
+ type cellSet;
+ action new;
+ source cellToCell;
+ set c1;
+ }
+
+ {
+ name box;
+ type cellSet;
+ action subset;
+ source boxToCell;
+ boxes
+ (
+ (0.0485 0.01 -100)(0.0565 0.035 100)
+ );
+ }
+
+ {
+ name box;
+ type cellSet;
+ action invert;
+ }
+);
+
+// ************************************************************************* //
--
GitLab