Commit 151f641f authored by Henry Weller's avatar Henry Weller Committed by Andrew Heather
Browse files

compressibleInterFilmFoam::VoFSolidificationMeltingSource: New VoF solidification fvOption

parent 577593ea
VoFPatchTransfer/VoFPatchTransfer.C
VoFSolidificationMeltingSource/VoFSolidificationMeltingSource.C
VoFSolidificationMeltingSource/VoFSolidificationMeltingSourceIO.C
compressibleInterFilmFoam.C
EXE = $(FOAM_APPBIN)/compressibleInterFilmFoam
......@@ -21,6 +21,7 @@ EXE_INC = \
-I$(LIB_SRC)/dynamicFvMesh/lnInclude \
-I$(LIB_SRC)/finiteVolume/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
-I$(LIB_SRC)/fvOptions/lnInclude
EXE_LIBS = \
-ltwoPhaseMixtureThermo \
......
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2017 OpenFOAM Foundation
\\/ 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/>.
\*---------------------------------------------------------------------------*/
#include "VoFSolidificationMeltingSource.H"
#include "twoPhaseMixtureThermo.H"
#include "zeroGradientFvPatchFields.H"
#include "addToRunTimeSelectionTable.H"
// * * * * * * * * * * * * * Static Member Functions * * * * * * * * * * * * //
namespace Foam
{
namespace fv
{
defineTypeNameAndDebug(VoFSolidificationMeltingSource, 0);
addToRunTimeSelectionTable
(
option,
VoFSolidificationMeltingSource,
dictionary
);
}
}
// * * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * //
void Foam::fv::VoFSolidificationMeltingSource::update()
{
if (curTimeIndex_ == mesh_.time().timeIndex())
{
return;
}
if (debug)
{
Info<< type() << ": " << name_
<< " - updating solid phase fraction" << endl;
}
alphaSolid_.oldTime();
const twoPhaseMixtureThermo& thermo
(
mesh_.lookupObject<twoPhaseMixtureThermo>
(
twoPhaseMixtureThermo::dictName
)
);
const volScalarField& TVoF = thermo.thermo1().T();
const volScalarField CpVoF(thermo.thermo1().Cp());
const volScalarField& alphaVoF = thermo.alpha1();
forAll(cells_, i)
{
const label celli = cells_[i];
alphaSolid_[celli] = min
(
relax_*alphaVoF[celli]*alphaSolidT_->value(TVoF[celli])
+ (1 - relax_)*alphaSolid_[celli],
alphaVoF[celli]
);
}
alphaSolid_.correctBoundaryConditions();
curTimeIndex_ = mesh_.time().timeIndex();
}
Foam::word Foam::fv::VoFSolidificationMeltingSource::alphaSolidName() const
{
const twoPhaseMixtureThermo& thermo
(
mesh_.lookupObject<twoPhaseMixtureThermo>
(
twoPhaseMixtureThermo::dictName
)
);
const volScalarField& alphaVoF = thermo.alpha1();
return IOobject::groupName(alphaVoF.name(), "solid");
}
// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
Foam::fv::VoFSolidificationMeltingSource::VoFSolidificationMeltingSource
(
const word& sourceName,
const word& modelType,
const dictionary& dict,
const fvMesh& mesh
)
:
cellSetOption(sourceName, modelType, dict, mesh),
alphaSolidT_(Function1<scalar>::New("alphaSolidT", coeffs_)),
L_("L", dimEnergy/dimMass, coeffs_),
relax_(coeffs_.lookupOrDefault("relax", 0.9)),
Cu_(coeffs_.lookupOrDefault<scalar>("Cu", 100000)),
q_(coeffs_.lookupOrDefault("q", 0.001)),
alphaSolid_
(
IOobject
(
alphaSolidName(),
mesh.time().timeName(),
mesh,
IOobject::READ_IF_PRESENT,
IOobject::AUTO_WRITE
),
mesh,
dimensionedScalar("alpha1", dimless, 0.0),
zeroGradientFvPatchScalarField::typeName
),
curTimeIndex_(-1)
{
fieldNames_.setSize(2);
fieldNames_[0] = "U";
fieldNames_[1] = "T";
applied_.setSize(fieldNames_.size(), false);
}
// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
void Foam::fv::VoFSolidificationMeltingSource::addSup
(
fvMatrix<scalar>& eqn,
const label fieldi
)
{
apply(geometricOneField(), eqn);
}
void Foam::fv::VoFSolidificationMeltingSource::addSup
(
const volScalarField& rho,
fvMatrix<scalar>& eqn,
const label fieldi
)
{
apply(rho, eqn);
}
void Foam::fv::VoFSolidificationMeltingSource::addSup
(
fvMatrix<vector>& eqn,
const label fieldi
)
{
if (debug)
{
Info<< type() << ": applying source to " << eqn.psi().name() << endl;
}
update();
scalarField& Sp = eqn.diag();
const scalarField& V = mesh_.V();
forAll(cells_, i)
{
const label celli = cells_[i];
const scalar Vc = V[celli];
const scalar alphaFluid = 1 - alphaSolid_[celli];
const scalar S = Cu_*sqr(1 - alphaFluid)/(pow3(alphaFluid) + q_);
Sp[celli] -= Vc*S;
}
}
void Foam::fv::VoFSolidificationMeltingSource::addSup
(
const volScalarField& rho,
fvMatrix<vector>& eqn,
const label fieldi
)
{
// Momentum source uses a Boussinesq approximation - redirect
addSup(eqn, fieldi);
}
// ************************************************************************* //
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2017 OpenFOAM Foundation
\\/ 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/>.
Class
Foam::fv::VoFSolidificationMeltingSource
Description
Solidification and melting model for VoF simulations.
The presence of the solid phase in the flow field is incorporated into the
model as a momentum porosity contribution; the energy associated with the
phase change is added as an enthalpy contribution. The solid fraction as a
function of temperature \c alphaSolidT is specified as a Foam::Function1.
The model writes the field \c alpha[01].solid which can be visualised to to
show the solid distribution.
Usage
Example usage:
\verbatim
VoFSolidificationMeltingSource1
{
type VoFSolidificationMeltingSource;
active yes;
selectionMode cellZone;
cellZone solidZone;
alphaSolidT table
(
(330 1)
(335 0)
);
L 334000;
}
\endverbatim
Where:
\table
Property | Description | Required | Default value
alphaSolidT | Solid fraction as function of temperature | yes |
L | Latent heat of fusion [J/kg] | yes |
relax | Relaxation coefficient [0-1] | no | 0.9
Cu | Model coefficient | no | 100000
q | Model coefficient | no | 0.001
\endtable
See also
Foam::fv::solidificationMeltingSource
Foam::Function1
SourceFiles
VoFSolidificationMeltingSource.C
VoFSolidificationMeltingSourceIO.C
\*---------------------------------------------------------------------------*/
#ifndef VoFSolidificationMeltingSource_H
#define VoFSolidificationMeltingSource_H
#include "fvMesh.H"
#include "volFields.H"
#include "cellSetOption.H"
#include "Function1.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
namespace fv
{
/*---------------------------------------------------------------------------*\
Class VoFSolidificationMeltingSource Declaration
\*---------------------------------------------------------------------------*/
class VoFSolidificationMeltingSource
:
public cellSetOption
{
// Private data
//- Solid fraction as a function of temperature
autoPtr<Function1<scalar>> alphaSolidT_;
//- Latent heat of fusion [J/kg]
dimensionedScalar L_;
//- Phase fraction under-relaxation coefficient
scalar relax_;
//- Mushy region momentum sink coefficient [1/s]; default = 10^5
scalar Cu_;
//- Coefficient used in porosity calc - default = 0.001
scalar q_;
//- Solid phase fraction
volScalarField alphaSolid_;
//- Current time index (used for updating)
label curTimeIndex_;
// Private Member Functions
//- Return the name of the solid phase fraction
word alphaSolidName() const;
//- Update the model
void update();
//- Helper function to apply to the energy equation
template<class RhoFieldType>
void apply(const RhoFieldType& rho, fvMatrix<scalar>& eqn);
//- Disallow default bitwise copy construct
VoFSolidificationMeltingSource(const VoFSolidificationMeltingSource&);
//- Disallow default bitwise assignment
void operator=(const VoFSolidificationMeltingSource&);
public:
//- Runtime type information
TypeName("VoFSolidificationMeltingSource");
// Constructors
//- Construct from explicit source name and mesh
VoFSolidificationMeltingSource
(
const word& sourceName,
const word& modelType,
const dictionary& dict,
const fvMesh& mesh
);
// Member Functions
// Add explicit and implicit contributions
//- Add explicit contribution to enthalpy equation
virtual void addSup(fvMatrix<scalar>& eqn, const label fieldi);
//- Add implicit contribution to momentum equation
virtual void addSup(fvMatrix<vector>& eqn, const label fieldi);
// Add explicit and implicit contributions to compressible equation
//- Add explicit contribution to compressible enthalpy equation
virtual void addSup
(
const volScalarField& rho,
fvMatrix<scalar>& eqn,
const label fieldi
);
//- Add implicit contribution to compressible momentum equation
virtual void addSup
(
const volScalarField& rho,
fvMatrix<vector>& eqn,
const label fieldi
);
// IO
//- Read source dictionary
virtual bool read(const dictionary& dict);
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace fv
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#ifdef NoRepository
#include "VoFSolidificationMeltingSourceTemplates.C"
#endif
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2017 OpenFOAM Foundation
\\/ 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/>.
\*---------------------------------------------------------------------------*/
#include "VoFSolidificationMeltingSource.H"
// * * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * //
bool Foam::fv::VoFSolidificationMeltingSource::read(const dictionary& dict)
{
if (cellSetOption::read(dict))
{
alphaSolidT_ = Function1<scalar>::New("alphaSolidT", coeffs_);
coeffs_.lookup("L") >> L_;
coeffs_.readIfPresent("relax", relax_);
coeffs_.readIfPresent("Cu", Cu_);
coeffs_.readIfPresent("q", q_);
return true;
}
else
{
return false;
}
return false;
}
// ************************************************************************* //
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2017 OpenFOAM Foundation
\\/ 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/>.
\*---------------------------------------------------------------------------*/
#include "fvcDdt.H"
#include "twoPhaseMixtureThermo.H"
// * * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * //
template<class RhoFieldType>
void Foam::fv::VoFSolidificationMeltingSource::apply
(
const RhoFieldType& rho,
fvMatrix<scalar>& eqn
)
{
if (debug)
{
Info<< type() << ": applying source to " << eqn.psi().name() << endl;
}
update();
const twoPhaseMixtureThermo& thermo
(
mesh_.lookupObject<twoPhaseMixtureThermo>
(
twoPhaseMixtureThermo::dictName
)
);