songtianlun/openfoam
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity

Adding new buoyantBoussinesqSimpleFoam

Browse Source 
- incompressible, Boussinesq variant of buoyantSimpleFoam
    - requires new fixedFluxBoussinesqBuoyantPressure bc on pd at walls
      to balance the flux generated by the temperature gradient
This commit is contained in:
andy 2009-01-28 15:11:43 +00:00
parent 8ccd361f56
commit d0e99ff347
14 changed files with 623 additions and 0 deletions
Show Stats Download Patch File Download Diff File Expand all files Collapse all files

3
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/Make/files Normal file
View File

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

12
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/Make/options Normal file
View File

@ -0,0 +1,12 @@
EXE_INC = \
-I$(LIB_SRC)/finiteVolume/lnInclude \
-I$(LIB_SRC)/turbulenceModels \
-I$(LIB_SRC)/turbulenceModels/incompressible/RAS/lnInclude \
-I$(LIB_SRC)/transportModels \
-I$(LIB_SRC)/transportModels/incompressible/singlePhaseTransportModel
EXE_LIBS = \
-lfiniteVolume \
-lmeshTools \
-lincompressibleRASModels \
-lincompressibleTransportModels

19
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/TEqn.H Normal file
View File

@ -0,0 +1,19 @@
{
volScalarField kappaEff
(
"kappaEff",
turbulence->nu() + turbulence->nut()/Pr
);
fvScalarMatrix TEqn
(
fvm::div(phi, T)
- fvm::Sp(fvc::div(phi), T)
- fvm::laplacian(kappaEff, T)
);
TEqn.relax();
eqnResidual = TEqn.solve().initialResidual();
maxResidual = max(eqnResidual, maxResidual);
}

20
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/UEqn.H Normal file
View File

@ -0,0 +1,20 @@
// Solve the Momentum equation
tmp<fvVectorMatrix> UEqn
(
fvm::div(phi, U)
- fvm::Sp(fvc::div(phi), U)
+ turbulence->divDevReff(U)
);
UEqn().relax();
eqnResidual = solve
(
UEqn()
==
-fvc::grad(pd)
+ beta*gh*fvc::grad(T)
).initialResidual();
maxResidual = max(eqnResidual, maxResidual);

105
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/buoyantBoussinesqSimpleFoam.C Normal file
View File

@ -0,0 +1,105 @@
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 1991-2009 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
buoyantBoussinesqSimpleFoam
Description
Steady-state solver for buoyant, turbulent flow of incompressible fluids
Uses the Boussinesq approximation:
\f[
rho_{eff} = 1 - beta(T - T_{ref})
\f]
where:
\f$ rho_{eff} \f$ = the effective (driving) density
beta = thermal expansion coefficient [1/K]
T = temperature [K]
\f$ T_{ref} \f$ = reference temperature [K]
Valid when:
\f[
rho_{eff} << 1
\f]
\*---------------------------------------------------------------------------*/
#include "fvCFD.H"
#include "singlePhaseTransportModel.H"
#include "RASModel.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
int main(int argc, char *argv[])
{
# include "setRootCase.H"
# include "createTime.H"
# include "createMesh.H"
# include "readEnvironmentalProperties.H"
# include "createFields.H"
# include "initContinuityErrs.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Info<< "\nStarting time loop\n" << endl;
for (runTime++; !runTime.end(); runTime++)
{
Info<< "Time = " << runTime.timeName() << nl << endl;
# include "readSIMPLEControls.H"
# include "initConvergenceCheck.H"
pd.storePrevIter();
// Pressure-velocity SIMPLE corrector
{
# include "UEqn.H"
# include "TEqn.H"
# include "pdEqn.H"
}
turbulence->correct();
if (runTime.write())
{
# include "writeAdditionalFields.H"
}
Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
<< " ClockTime = " << runTime.elapsedClockTime() << " s"
<< nl << endl;
# include "convergenceCheck.H"
}
Info<< "End\n" << endl;
return 0;
}
// ************************************************************************* //

9
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/convergenceCheck.H Normal file
View File

@ -0,0 +1,9 @@
// check convergence
if (maxResidual < convergenceCriterion)
{
Info<< "reached convergence criterion: " << convergenceCriterion << endl;
runTime.writeAndEnd();
Info<< "latestTime = " << runTime.timeName() << endl;
}

67
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/createFields.H Normal file
View File

@ -0,0 +1,67 @@
Info<< "Reading thermophysical properties\n" << endl;
Info<< "Reading field T\n" << endl;
volScalarField T
(
IOobject
(
"T",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
// kinematic pd
Info<< "Reading field pd\n" << endl;
volScalarField pd
(
IOobject
(
"pd",
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"
# include "readTransportProperties.H"
Info<< "Creating turbulence model\n" << endl;
autoPtr<incompressible::RASModel> turbulence
(
incompressible::RASModel::New(U, phi, laminarTransport)
);
Info<< "Calculating field g.h\n" << endl;
volScalarField gh("gh", g & mesh.C());
label pdRefCell = 0;
scalar pdRefValue = 0.0;
setRefCell
(
pd,
mesh.solutionDict().subDict("SIMPLE"),
pdRefCell,
pdRefValue
);

7
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/initConvergenceCheck.H Normal file
View File

@ -0,0 +1,7 @@
// initialize values for convergence checks
scalar eqnResidual = 1, maxResidual = 0;
scalar convergenceCriterion = 0;
simple.readIfPresent("convergence", convergenceCriterion);

41
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/pdEqn.H Normal file
View File

@ -0,0 +1,41 @@
volScalarField rUA = 1.0/UEqn().A();
U = rUA*UEqn().H();
UEqn.clear();
phi = fvc::interpolate(U) & mesh.Sf();
adjustPhi(phi, U, pd);
phi += fvc::interpolate(beta*gh*rUA)*fvc::snGrad(T)*mesh.magSf();
for (int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++)
{
fvScalarMatrix pdEqn
(
fvm::laplacian(rUA, pd) == fvc::div(phi)
);
pdEqn.setReference(pdRefCell, pdRefValue);
// retain the residual from the first iteration
if (nonOrth == 0)
{
eqnResidual = pdEqn.solve().initialResidual();
maxResidual = max(eqnResidual, maxResidual);
}
else
{
pdEqn.solve();
}
if (nonOrth == nNonOrthCorr)
{
phi -= pdEqn.flux();
}
}
#include "continuityErrs.H"
// Explicitly relax pressure for momentum corrector
pd.relax();
U -= rUA*(fvc::grad(pd) - beta*gh*fvc::grad(T));
U.correctBoundaryConditions();

13
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/readTransportProperties.H Normal file
View File

@ -0,0 +1,13 @@
singlePhaseTransportModel laminarTransport(U, phi);
// thermal expansion coefficient [1/K]
dimensionedScalar beta(laminarTransport.lookup("beta"));
// reference temperature [K]
dimensionedScalar TRef(laminarTransport.lookup("TRef"));
// reference kinematic pressure [m2/s2]
dimensionedScalar pRef(laminarTransport.lookup("pRef"));
// Prandtl number
dimensionedScalar Pr(laminarTransport.lookup("Pr"));

29
applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam/writeAdditionalFields.H Normal file
View File

@ -0,0 +1,29 @@
{
volScalarField rhoEff
(
IOobject
(
"rhoEff",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
1.0 - beta*(T - TRef)
);
rhoEff.write();
volScalarField p
(
IOobject
(
"p",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
pd + rhoEff*gh + pRef
);
p.write();
}

1
src/finiteVolume/Make/files
View File

@ -93,6 +93,7 @@ $(derivedFvPatchFields)/directMappedFixedValue/directMappedFixedValueFvPatchFiel
$(derivedFvPatchFields)/directMappedVelocityFluxFixedValue/directMappedVelocityFluxFixedValueFvPatchField.C
$(derivedFvPatchFields)/fan/fanFvPatchFields.C
$(derivedFvPatchFields)/fixedFluxBuoyantPressure/fixedFluxBuoyantPressureFvPatchScalarField.C
$(derivedFvPatchFields)/fixedFluxBoussinesqBuoyantPressure/fixedFluxBoussinesqBuoyantPressureFvPatchScalarField.C
$(derivedFvPatchFields)/fixedFluxPressure/fixedFluxPressureFvPatchScalarField.C
$(derivedFvPatchFields)/fixedInternalValueFvPatchField/fixedInternalValueFvPatchFields.C
$(derivedFvPatchFields)/fixedNormalSlip/fixedNormalSlipFvPatchFields.C

149
src/finiteVolume/fields/fvPatchFields/derived/fixedFluxBoussinesqBuoyantPressure/fixedFluxBoussinesqBuoyantPressureFvPatchScalarField.C Normal file
View File

@ -0,0 +1,149 @@
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 1991-2009 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
\*---------------------------------------------------------------------------*/
#include "fixedFluxBoussinesqBuoyantPressureFvPatchScalarField.H"
#include "addToRunTimeSelectionTable.H"
#include "fvPatchFieldMapper.H"
#include "volFields.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField::
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
const fvPatch& p,
const DimensionedField<scalar, volMesh>& iF
)
:
fixedGradientFvPatchScalarField(p, iF)
{}
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField::
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
const fixedFluxBoussinesqBuoyantPressureFvPatchScalarField& ptf,
const fvPatch& p,
const DimensionedField<scalar, volMesh>& iF,
const fvPatchFieldMapper& mapper
)
:
fixedGradientFvPatchScalarField(ptf, p, iF, mapper)
{}
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField::
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
const fvPatch& p,
const DimensionedField<scalar, volMesh>& iF,
const dictionary&
)
:
fixedGradientFvPatchScalarField(p, iF)
{
fvPatchField<scalar>::operator=(patchInternalField());
gradient() = 0.0;
}
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField::
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
const fixedFluxBoussinesqBuoyantPressureFvPatchScalarField& wbppsf
)
:
fixedGradientFvPatchScalarField(wbppsf)
{}
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField::
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
const fixedFluxBoussinesqBuoyantPressureFvPatchScalarField& wbppsf,
const DimensionedField<scalar, volMesh>& iF
)
:
fixedGradientFvPatchScalarField(wbppsf, iF)
{}
// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
void fixedFluxBoussinesqBuoyantPressureFvPatchScalarField::updateCoeffs()
{
if (updated())
{
return;
}
const dictionary& environmentalProperties
= db().lookupObject<IOdictionary>("environmentalProperties");
dimensionedVector g(environmentalProperties.lookup("g"));
const dictionary& transportProperties
= db().lookupObject<IOdictionary>("transportProperties");
dimensionedScalar beta(transportProperties.lookup("beta"));
const fvPatchField<scalar>& T =
patch().lookupPatchField<volScalarField, scalar>("T");
gradient() = beta.value()*T.snGrad()*(g.value() & patch().Cf());
fixedGradientFvPatchScalarField::updateCoeffs();
}
void fixedFluxBoussinesqBuoyantPressureFvPatchScalarField::write
(
Ostream& os
) const
{
fixedGradientFvPatchScalarField::write(os);
writeEntry("value", os);
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
makePatchTypeField
(
fvPatchScalarField,
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
);
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace Foam
// ************************************************************************* //

148
src/finiteVolume/fields/fvPatchFields/derived/fixedFluxBoussinesqBuoyantPressure/fixedFluxBoussinesqBuoyantPressureFvPatchScalarField.H Normal file
View File

@ -0,0 +1,148 @@
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 1991-2009 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
Class
Foam::fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
Description
Boundary condition on pressure for use with buoyant solvers employing the
Boussinesq approximation to balance the flux generated by the temperature
gradient.
SourceFiles
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField.C
\*---------------------------------------------------------------------------*/
#ifndef fixedFluxBoussinesqBuoyantPressureFvPatchScalarFields_H
#define fixedFluxBoussinesqBuoyantPressureFvPatchScalarFields_H
#include "fvPatchFields.H"
#include "fixedGradientFvPatchFields.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
/*---------------------------------------------------------------------------*\
Class fixedFluxBoussinesqBuoyantPressureFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/
class fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
:
public fixedGradientFvPatchScalarField
{
public:
//- Runtime type information
TypeName("fixedFluxBoussinesqBuoyantPressure");
// Constructors
//- Construct from patch and internal field
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
const fvPatch&,
const DimensionedField<scalar, volMesh>&
);
//- Construct from patch, internal field and dictionary
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
const fvPatch&,
const DimensionedField<scalar, volMesh>&,
const dictionary&
);
//- Construct by mapping given
// fixedFluxBoussinesqBuoyantPressureFvPatchScalarField onto a new
// patch
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
const fixedFluxBoussinesqBuoyantPressureFvPatchScalarField&,
const fvPatch&,
const DimensionedField<scalar, volMesh>&,
const fvPatchFieldMapper&
);
//- Construct as copy
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
const fixedFluxBoussinesqBuoyantPressureFvPatchScalarField&
);
//- Construct and return a clone
virtual tmp<fvPatchScalarField> clone() const
{
return tmp<fvPatchScalarField>
(
new fixedFluxBoussinesqBuoyantPressureFvPatchScalarField(*this)
);
}
//- Construct as copy setting internal field reference
fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
const fixedFluxBoussinesqBuoyantPressureFvPatchScalarField&,
const DimensionedField<scalar, volMesh>&
);
//- Construct and return a clone setting internal field reference
virtual tmp<fvPatchScalarField> clone
(
const DimensionedField<scalar, volMesh>& iF
) const
{
return tmp<fvPatchScalarField>
(
new fixedFluxBoussinesqBuoyantPressureFvPatchScalarField
(
*this,
iF
)
);
}
// Member functions
//- Update the coefficients associated with the patch field
virtual void updateCoeffs();
//- Write
virtual void write(Ostream&) const;
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //