Commit 97462476 authored by Henry Weller's avatar Henry Weller
Browse files

porosityModels::solidification: New porosity model to simulate solidification

Description
    Simple solidification porosity model

    This is a simple approximation to solidification where the solid phase
    is represented as a porous blockage with the drag-coefficient evaluated from

        \f[
            S = - \rho D(T) U
        \f]

    where
    \vartable
        D(T) | User-defined drag-coefficient as function of temperature
    \endvartable

    Note that the latent heat of solidification is not included and the
    temperature is unchanged by the modelled change of phase.

    Example of the solidification model specification:
    \verbatim
        type            solidification;

        solidificationCoeffs
        {
            // Solidify between 330K and 330.5K
            D table
            (
                (330.0     10000) // Solid below 330K
                (330.5     0)     // Liquid above 330.5K
            );

            // Solidification porosity is isotropic
            // use the global coordinate system
            coordinateSystem
            {
                type    cartesian;
                origin  (0 0 0);
                coordinateRotation
                {
                    type    axesRotation;
                    e1      (1 0 0);
                    e2      (0 1 0);
                }
            }
        }
    \endverbatim
parent c5e7f356
......@@ -417,6 +417,7 @@ $(porosity)/porosityModel/IOporosityModelList.C
$(porosity)/DarcyForchheimer/DarcyForchheimer.C
$(porosity)/fixedCoeff/fixedCoeff.C
$(porosity)/powerLaw/powerLaw.C
$(porosity)/solidification/solidification.C
MRF = $(general)/MRF
$(MRF)/MRFZone.C
......
/*---------------------------------------------------------------------------*\
========= |
\\ / 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 "addToRunTimeSelectionTable.H"
#include "solidification.H"
#include "geometricOneField.H"
#include "fvMatrices.H"
// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
namespace Foam
{
namespace porosityModels
{
defineTypeNameAndDebug(solidification, 0);
addToRunTimeSelectionTable(porosityModel, solidification, mesh);
}
}
// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
Foam::porosityModels::solidification::solidification
(
const word& name,
const word& modelType,
const fvMesh& mesh,
const dictionary& dict,
const word& cellZoneName
)
:
porosityModel(name, modelType, mesh, dict, cellZoneName),
TName_(coeffs_.lookupOrDefault<word>("T", "T")),
rhoName_(coeffs_.lookupOrDefault<word>("rho", "rho")),
D_(Function1<scalar>::New("D", coeffs_))
{}
// * * * * * * * * * * * * * * * * Destructor * * * * * * * * * * * * * * * //
Foam::porosityModels::solidification::~solidification()
{}
// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
void Foam::porosityModels::solidification::calcTransformModelData()
{}
void Foam::porosityModels::solidification::calcForce
(
const volVectorField& U,
const volScalarField& rho,
const volScalarField& mu,
vectorField& force
) const
{
scalarField Udiag(U.size(), 0.0);
const scalarField& V = mesh_.V();
apply(Udiag, V, rho, U);
force = Udiag*U;
}
void Foam::porosityModels::solidification::correct
(
fvVectorMatrix& UEqn
) const
{
const volVectorField& U = UEqn.psi();
const scalarField& V = mesh_.V();
scalarField& Udiag = UEqn.diag();
if (UEqn.dimensions() == dimForce)
{
const volScalarField& rho = mesh_.lookupObject<volScalarField>
(
IOobject::groupName(rhoName_, U.group())
);
apply(Udiag, V, rho, U);
}
else
{
apply(Udiag, V, geometricOneField(), U);
}
}
void Foam::porosityModels::solidification::correct
(
fvVectorMatrix& UEqn,
const volScalarField& rho,
const volScalarField& mu
) const
{
const volVectorField& U = UEqn.psi();
const scalarField& V = mesh_.V();
scalarField& Udiag = UEqn.diag();
apply(Udiag, V, rho, U);
}
void Foam::porosityModels::solidification::correct
(
const fvVectorMatrix& UEqn,
volTensorField& AU
) const
{
const volVectorField& U = UEqn.psi();
if (UEqn.dimensions() == dimForce)
{
const volScalarField& rho = mesh_.lookupObject<volScalarField>
(
IOobject::groupName(rhoName_, U.group())
);
apply(AU, rho, U);
}
else
{
apply(AU, geometricOneField(), U);
}
}
bool Foam::porosityModels::solidification::writeData(Ostream& os) const
{
os << indent << name_ << endl;
dict_.write(os);
return true;
}
// ************************************************************************* //
/*---------------------------------------------------------------------------*\
========= |
\\ / 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::porosityModels::solidification
Description
Simple solidification porosity model
This is a simple approximation to solidification where the solid phase
is represented as a porous blockage with the drag-coefficient evaluated from
\f[
S = - \rho D(T) U
\f]
where
\vartable
D(T) | User-defined drag-coefficient as function of temperature
\endvartable
Note that the latent heat of solidification is not included and the
temperature is unchanged by the modelled change of phase.
Example of the solidification model specification:
\verbatim
type solidification;
solidificationCoeffs
{
// Solidify between 330K and 330.5K
D table
(
(330.0 10000) // Solid below 330K
(330.5 0) // Liquid above 330.5K
);
// Solidification porosity is isotropic
// use the global coordinate system
coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type axesRotation;
e1 (1 0 0);
e2 (0 1 0);
}
}
}
\endverbatim
SourceFiles
solidification.C
solidificationTemplates.C
\*---------------------------------------------------------------------------*/
#ifndef solidification_H
#define solidification_H
#include "porosityModel.H"
#include "Function1.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
namespace porosityModels
{
/*---------------------------------------------------------------------------*\
Class solidification Declaration
\*---------------------------------------------------------------------------*/
class solidification
:
public porosityModel
{
// Private data
//- Name of temperature field, default = "T"
word TName_;
//- Name of density field, default = "rho"
word rhoName_;
//- User-defined drag-coefficient as function of temperature
autoPtr<Function1<scalar>> D_;
// Private Member Functions
//- Apply resistance
template<class RhoFieldType>
void apply
(
scalarField& Udiag,
const scalarField& V,
const RhoFieldType& rho,
const volVectorField& U
) const;
//- Apply resistance
template<class RhoFieldType>
void apply
(
tensorField& AU,
const RhoFieldType& rho,
const volVectorField& U
) const;
//- Disallow default bitwise copy construct
solidification(const solidification&);
//- Disallow default bitwise assignment
void operator=(const solidification&);
public:
//- Runtime type information
TypeName("solidification");
//- Constructor
solidification
(
const word& name,
const word& modelType,
const fvMesh& mesh,
const dictionary& dict,
const word& cellZoneName
);
//- Destructor
virtual ~solidification();
// Member Functions
//- Transform the model data wrt mesh changes
virtual void calcTransformModelData();
//- Calculate the porosity force
virtual void calcForce
(
const volVectorField& U,
const volScalarField& rho,
const volScalarField& mu,
vectorField& force
) const;
//- Add resistance
virtual void correct(fvVectorMatrix& UEqn) const;
//- Add resistance
virtual void correct
(
fvVectorMatrix& UEqn,
const volScalarField& rho,
const volScalarField& mu
) const;
//- Add resistance
virtual void correct
(
const fvVectorMatrix& UEqn,
volTensorField& AU
) const;
// I-O
//- Write
bool writeData(Ostream& os) const;
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace porosityModels
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#ifdef NoRepository
#include "solidificationTemplates.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 "volFields.H"
// * * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * //
template<class RhoFieldType>
void Foam::porosityModels::solidification::apply
(
scalarField& Udiag,
const scalarField& V,
const RhoFieldType& rho,
const volVectorField& U
) const
{
const volScalarField& T = mesh_.lookupObject<volScalarField>
(
IOobject::groupName(TName_, U.group())
);
forAll(cellZoneIDs_, zoneI)
{
const labelList& cells = mesh_.cellZones()[cellZoneIDs_[zoneI]];
forAll(cells, i)
{
const label celli = cells[i];
Udiag[celli] += V[celli]*rho[celli]*D_->value(T[celli]);
}
}
}
template<class RhoFieldType>
void Foam::porosityModels::solidification::apply
(
tensorField& AU,
const RhoFieldType& rho,
const volVectorField& U
) const
{
const volScalarField& T = mesh_.lookupObject<volScalarField>
(
IOobject::groupName(TName_, U.group())
);
forAll(cellZoneIDs_, zoneI)
{
const labelList& cells = mesh_.cellZones()[cellZoneIDs_[zoneI]];
forAll(cells, i)
{
const label celli = cells[i];
AU[celli] += tensor::I*rho[celli]*D_->value(T[celli]);
}
}
}
// ************************************************************************* //
Supports Markdown
0% or .
You are about to add 0 people to the discussion. Proceed with caution.
Finish editing this message first!
Please register or to comment