New lumpedMassTemperature boundary condition
This boundary condition is applied to a patch which bounds a solid body, wholly or partially. It represents the body as a lumped mass, i.e. by a single temperature which is fixed across the patch. The body has a volume which is either specified by the user, or is calculated when the patch describes a closed volume (including in 2D meshes). Starting from an initial temperature, the change in temperature is the calculated over time according to a specified applied power source and the heat transferred across the boundary, using a specified density and specific heat capacity of the lumped mass.
This commit is contained in:
Chris Greenshields
@ -1,4 +1,5 @@
|
||||
externalTemperature/externalTemperatureFvPatchScalarField.C
|
||||
coupledTemperature/coupledTemperatureFvPatchScalarField.C
|
||||
lumpedMassTemperature/lumpedMassTemperatureFvPatchScalarField.C
|
||||
|
||||
LIB = $(FOAM_LIBBIN)/libcoupledThermophysicalTransportModels
|
||||
|
||||
@ -0,0 +1,219 @@
|
||||
/*---------------------------------------------------------------------------*\
|
||||
========= |
|
||||
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
|
||||
\\ / O peration | Website: https://openfoam.org
|
||||
\\ / A nd | Copyright (C) 2024 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 "lumpedMassTemperatureFvPatchScalarField.H"
|
||||
#include "addToRunTimeSelectionTable.H"
|
||||
#include "fieldMapper.H"
|
||||
#include "thermophysicalTransportModel.H"
|
||||
#include "ZeroConstant.H"
|
||||
|
||||
// * * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * //
|
||||
|
||||
bool Foam::lumpedMassTemperatureFvPatchScalarField::closed() const
|
||||
{
|
||||
return mag(gSum(patch().Sf()))/gSum(patch().magSf()) < rootSmall;
|
||||
}
|
||||
|
||||
Foam::scalar Foam::lumpedMassTemperatureFvPatchScalarField::V() const
|
||||
{
|
||||
return -gSum(patch().Sf() & patch().Cf())
|
||||
/patch().boundaryMesh().mesh().nSolutionD();
|
||||
}
|
||||
|
||||
// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
|
||||
|
||||
Foam::lumpedMassTemperatureFvPatchScalarField::
|
||||
lumpedMassTemperatureFvPatchScalarField
|
||||
(
|
||||
const fvPatch& p,
|
||||
const DimensionedField<scalar, volMesh>& iF,
|
||||
const dictionary& dict
|
||||
)
|
||||
:
|
||||
fixedValueFvPatchScalarField(p, iF),
|
||||
rho_(dict.lookup<scalar>("rho")),
|
||||
Cv_(dict.lookup<scalar>("Cv")),
|
||||
T_
|
||||
(
|
||||
IOobject
|
||||
(
|
||||
"T_" + patch().name(),
|
||||
db().time().name(),
|
||||
db()
|
||||
),
|
||||
dimensionedScalar(dimTemperature, dict.lookup<scalar>("T"))
|
||||
),
|
||||
Q_
|
||||
(
|
||||
dict.found("Q")
|
||||
? Function1<scalar>::New("Q", dict)
|
||||
: autoPtr<Function1<scalar>>
|
||||
(
|
||||
new Function1s::ZeroConstant<scalar>("Q", dict)
|
||||
)
|
||||
),
|
||||
V_(NaN)
|
||||
{
|
||||
if (!dict.readIfPresent("volume", V_))
|
||||
{
|
||||
if (closed())
|
||||
{
|
||||
V_ = V();
|
||||
Info<< "Volume for the thermal mass, enclosed by patch '"
|
||||
<< patch().name() << "', = " << V_;
|
||||
}
|
||||
else
|
||||
{
|
||||
FatalErrorInFunction
|
||||
<< "Patch '" << patch().name()
|
||||
<< "' corresponding to a thermal mass is not closed." << nl
|
||||
<< "Please specify the volume with the optional 'volume' entry."
|
||||
<< exit(FatalError);
|
||||
}
|
||||
}
|
||||
|
||||
fvPatchScalarField::operator=(T_.value());
|
||||
}
|
||||
|
||||
|
||||
Foam::lumpedMassTemperatureFvPatchScalarField::
|
||||
lumpedMassTemperatureFvPatchScalarField
|
||||
(
|
||||
const lumpedMassTemperatureFvPatchScalarField& ptf,
|
||||
const fvPatch& p,
|
||||
const DimensionedField<scalar, volMesh>& iF,
|
||||
const fieldMapper& mapper
|
||||
)
|
||||
:
|
||||
fixedValueFvPatchScalarField(ptf, p, iF, mapper),
|
||||
rho_(ptf.rho_),
|
||||
Cv_(ptf.Cv_),
|
||||
T_(ptf.T_),
|
||||
Q_(ptf.Q_),
|
||||
V_(ptf.V_)
|
||||
{}
|
||||
|
||||
|
||||
Foam::lumpedMassTemperatureFvPatchScalarField::
|
||||
lumpedMassTemperatureFvPatchScalarField
|
||||
(
|
||||
const lumpedMassTemperatureFvPatchScalarField& ptf,
|
||||
const DimensionedField<scalar, volMesh>& iF
|
||||
)
|
||||
:
|
||||
fixedValueFvPatchScalarField(ptf, iF),
|
||||
rho_(ptf.rho_),
|
||||
Cv_(ptf.Cv_),
|
||||
T_(ptf.T_),
|
||||
Q_(ptf.Q_),
|
||||
V_(ptf.V_)
|
||||
{}
|
||||
|
||||
|
||||
// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
|
||||
|
||||
void Foam::lumpedMassTemperatureFvPatchScalarField::map
|
||||
(
|
||||
const fvPatchScalarField& ptf,
|
||||
const fieldMapper& mapper
|
||||
)
|
||||
{
|
||||
fixedValueFvPatchScalarField::map(ptf, mapper);
|
||||
}
|
||||
|
||||
|
||||
void Foam::lumpedMassTemperatureFvPatchScalarField::reset
|
||||
(
|
||||
const fvPatchScalarField& ptf
|
||||
)
|
||||
{
|
||||
fixedValueFvPatchScalarField::reset(ptf);
|
||||
}
|
||||
|
||||
|
||||
void Foam::lumpedMassTemperatureFvPatchScalarField::updateCoeffs()
|
||||
{
|
||||
if
|
||||
(
|
||||
updated()
|
||||
)
|
||||
{
|
||||
return;
|
||||
}
|
||||
|
||||
const thermophysicalTransportModel& ttm =
|
||||
db().lookupType<thermophysicalTransportModel>
|
||||
(
|
||||
internalField().group()
|
||||
);
|
||||
|
||||
const label patchi = patch().index();
|
||||
const scalarField Hf
|
||||
(
|
||||
ttm.kappaEff(patchi)*patch().magSf()*patch().deltaCoeffs()
|
||||
);
|
||||
const scalar Hs = rho_*Cv_*V_/db().time().deltaTValue();
|
||||
|
||||
const scalar t = db().time().userTimeValue();
|
||||
|
||||
T_.value() =
|
||||
(
|
||||
Q_->value(t) + gSum(Hf*patchInternalField())
|
||||
+ Hs*T_.oldTime().value()
|
||||
)/(Hs + gSum(Hf));
|
||||
|
||||
operator==(T_.value());
|
||||
|
||||
fixedValueFvPatchScalarField::updateCoeffs();
|
||||
}
|
||||
|
||||
|
||||
void Foam::lumpedMassTemperatureFvPatchScalarField::write
|
||||
(
|
||||
Ostream& os
|
||||
) const
|
||||
{
|
||||
fvPatchScalarField::write(os);
|
||||
writeEntry(os, "rho", rho_);
|
||||
writeEntry(os, "Cv", Cv_);
|
||||
writeEntry(os, "T", T_.value());
|
||||
writeEntry(os, Q_());
|
||||
writeEntry(os, "volume", V_);
|
||||
writeEntry(os, "value", *this);
|
||||
}
|
||||
|
||||
|
||||
// * * * * * * * * * * * * * * Build Macro Function * * * * * * * * * * * * //
|
||||
|
||||
namespace Foam
|
||||
{
|
||||
makePatchTypeField
|
||||
(
|
||||
fvPatchScalarField,
|
||||
lumpedMassTemperatureFvPatchScalarField
|
||||
);
|
||||
}
|
||||
|
||||
// ************************************************************************* //
|
||||
@ -0,0 +1,213 @@
|
||||
/*---------------------------------------------------------------------------*\
|
||||
========= |
|
||||
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
|
||||
\\ / O peration | Website: https://openfoam.org
|
||||
\\ / A nd | Copyright (C) 2024 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::lumpedMassTemperatureFvPatchScalarField
|
||||
|
||||
Description
|
||||
This boundary condition is applied to a patch which bounds a solid body,
|
||||
wholly or partially. It represents the body as a lumped mass, i.e. by a
|
||||
single temperature \c T which is fixed across the patch. The body has a
|
||||
volume \c V which is either specified by the user, or is calculated when
|
||||
the patch describes a closed volume (including in 2D meshes). Starting from
|
||||
an initial, specified \c T, the change in temperature is calculated over
|
||||
time according to an applied power source \c Q and the heat transferred
|
||||
across the boundary \Q_{b} (positive into the lumped mass):
|
||||
|
||||
\f[
|
||||
dT/dt = frac{Q + Q_{b}}{\rho C_{v} V}
|
||||
\f]
|
||||
|
||||
where
|
||||
\vartable
|
||||
Q | specified power source [W]
|
||||
Q_{b} | total calculated heat transferred across the boundary [W]
|
||||
\rho | density [kg/m^3]
|
||||
C_{v} | specific heat capacity [J/(kg K)]
|
||||
V | volume of the lumped mass [m^3}
|
||||
\endtable
|
||||
|
||||
Usage
|
||||
\table
|
||||
Property | Description | Req'd? | Default
|
||||
rho | density | yes |
|
||||
Cv | specific heat capacity | yes |
|
||||
T | temperature | yes |
|
||||
Q | power source | no | 0
|
||||
volume | volume of the lumped mass | no | calculated
|
||||
\endtable
|
||||
|
||||
Example of the boundary condition specification:
|
||||
\verbatim
|
||||
<patchName>
|
||||
{
|
||||
type lumpedMassTemperature;
|
||||
rho 1000;
|
||||
Cv 1300;
|
||||
T 500;
|
||||
Q constant 0.5;
|
||||
value uniform $T; // placeholder
|
||||
}
|
||||
\endverbatim
|
||||
|
||||
SourceFiles
|
||||
lumpedMassTemperatureFvPatchScalarField.C
|
||||
|
||||
\*---------------------------------------------------------------------------*/
|
||||
|
||||
#ifndef BC_H
|
||||
#define BC_H
|
||||
|
||||
#include "fixedValueFvPatchFields.H"
|
||||
#include "UniformDimensionedField.H"
|
||||
#include "Function1.H"
|
||||
|
||||
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
|
||||
|
||||
namespace Foam
|
||||
{
|
||||
|
||||
/*---------------------------------------------------------------------------*\
|
||||
Class lumpedMassTemperatureFvPatchScalarField Declaration
|
||||
\*---------------------------------------------------------------------------*/
|
||||
|
||||
class lumpedMassTemperatureFvPatchScalarField
|
||||
:
|
||||
public fixedValueFvPatchScalarField
|
||||
{
|
||||
// Private Data
|
||||
|
||||
//- Density
|
||||
const scalar rho_;
|
||||
|
||||
//- Specific heat capacity
|
||||
const scalar Cv_;
|
||||
|
||||
//- Temperature of the thermal mass
|
||||
UniformDimensionedField<scalar> T_;
|
||||
|
||||
//- Heat source (optional)
|
||||
autoPtr<Function1<scalar>> Q_;
|
||||
|
||||
//- Volume of the lumped mass, defaults when enclosed by the patch
|
||||
scalar V_;
|
||||
|
||||
|
||||
// Private Member Functions
|
||||
|
||||
//- Does the patch form a closed volume, including in a 2D case?
|
||||
bool closed() const;
|
||||
|
||||
//- Return volume formed by the enclosed patch
|
||||
scalar V() const;
|
||||
|
||||
|
||||
public:
|
||||
|
||||
//- Runtime type information
|
||||
TypeName("lumpedMassTemperature");
|
||||
|
||||
|
||||
// Constructors
|
||||
|
||||
//- Construct from patch, internal field and dictionary
|
||||
lumpedMassTemperatureFvPatchScalarField
|
||||
(
|
||||
const fvPatch&,
|
||||
const DimensionedField<scalar, volMesh>&,
|
||||
const dictionary&
|
||||
);
|
||||
|
||||
//- Construct by mapping given fixedValueTypeFvPatchField
|
||||
// onto a new patch
|
||||
lumpedMassTemperatureFvPatchScalarField
|
||||
(
|
||||
const lumpedMassTemperatureFvPatchScalarField&,
|
||||
const fvPatch&,
|
||||
const DimensionedField<scalar, volMesh>&,
|
||||
const fieldMapper&
|
||||
);
|
||||
|
||||
//- Disallow copy without setting internal field reference
|
||||
lumpedMassTemperatureFvPatchScalarField
|
||||
(
|
||||
const lumpedMassTemperatureFvPatchScalarField&
|
||||
) = delete;
|
||||
|
||||
//- Copy constructor setting internal field reference
|
||||
lumpedMassTemperatureFvPatchScalarField
|
||||
(
|
||||
const lumpedMassTemperatureFvPatchScalarField&,
|
||||
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 lumpedMassTemperatureFvPatchScalarField
|
||||
(
|
||||
*this,
|
||||
iF
|
||||
)
|
||||
);
|
||||
}
|
||||
|
||||
|
||||
// Member Functions
|
||||
|
||||
// Mapping functions
|
||||
|
||||
//- Map the given fvPatchField onto this fvPatchField
|
||||
virtual void map(const fvPatchScalarField&, const fieldMapper&);
|
||||
|
||||
//- Reset the fvPatchField to the given fvPatchField
|
||||
// Used for mesh to mesh mapping
|
||||
virtual void reset(const fvPatchScalarField&);
|
||||
|
||||
|
||||
// Evaluation functions
|
||||
|
||||
//- Update the coefficients associated with the patch field
|
||||
virtual void updateCoeffs();
|
||||
|
||||
|
||||
//- Write
|
||||
virtual void write(Ostream&) const;
|
||||
};
|
||||
|
||||
|
||||
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
|
||||
|
||||
} // End namespace Foam
|
||||
|
||||
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
|
||||
|
||||
|
||||
#endif
|
||||
|
||||
// ************************************************************************* //
|
||||
Reference in New Issue
Block a user