Commit 7f18c263 authored by Henry Weller's avatar Henry Weller Committed by Andrew Heather
Browse files

matchedFlowRateOutletVelocity: New flow-rate outlet BC

Velocity outlet boundary condition which corrects the extrapolated velocity
to match the flow rate of the specified corresponding inlet patch.
parent 77b7beb6
/*---------------------------------------------------------------------------*\
========= |
\\ / 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 "matchedFlowRateOutletVelocityFvPatchVectorField.H"
#include "volFields.H"
#include "one.H"
#include "addToRunTimeSelectionTable.H"
// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
Foam::matchedFlowRateOutletVelocityFvPatchVectorField::
matchedFlowRateOutletVelocityFvPatchVectorField
(
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF
)
:
fixedValueFvPatchField<vector>(p, iF),
inletPatchName_(),
volumetric_(false),
rhoName_("rho")
{}
Foam::matchedFlowRateOutletVelocityFvPatchVectorField::
matchedFlowRateOutletVelocityFvPatchVectorField
(
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF,
const dictionary& dict
)
:
fixedValueFvPatchField<vector>(p, iF, dict, false),
inletPatchName_(dict.lookup("inletPatch")),
volumetric_(dict.lookupOrDefault("volumetric", true))
{
if (volumetric_)
{
rhoName_ = "none";
}
else
{
rhoName_ = word(dict.lookupOrDefault<word>("rho", "rho"));
}
// Value field require if mass based
if (dict.found("value"))
{
fvPatchField<vector>::operator=
(
vectorField("value", dict, p.size())
);
}
else
{
evaluate(Pstream::commsTypes::blocking);
}
}
Foam::matchedFlowRateOutletVelocityFvPatchVectorField::
matchedFlowRateOutletVelocityFvPatchVectorField
(
const matchedFlowRateOutletVelocityFvPatchVectorField& ptf,
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF,
const fvPatchFieldMapper& mapper
)
:
fixedValueFvPatchField<vector>(ptf, p, iF, mapper),
inletPatchName_(ptf.inletPatchName_),
volumetric_(ptf.volumetric_),
rhoName_(ptf.rhoName_)
{}
Foam::matchedFlowRateOutletVelocityFvPatchVectorField::
matchedFlowRateOutletVelocityFvPatchVectorField
(
const matchedFlowRateOutletVelocityFvPatchVectorField& ptf
)
:
fixedValueFvPatchField<vector>(ptf),
inletPatchName_(ptf.inletPatchName_),
volumetric_(ptf.volumetric_),
rhoName_(ptf.rhoName_)
{}
Foam::matchedFlowRateOutletVelocityFvPatchVectorField::
matchedFlowRateOutletVelocityFvPatchVectorField
(
const matchedFlowRateOutletVelocityFvPatchVectorField& ptf,
const DimensionedField<vector, volMesh>& iF
)
:
fixedValueFvPatchField<vector>(ptf, iF),
inletPatchName_(ptf.inletPatchName_),
volumetric_(ptf.volumetric_),
rhoName_(ptf.rhoName_)
{}
// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
template<class RhoType>
void Foam::matchedFlowRateOutletVelocityFvPatchVectorField::updateValues
(
const label inletPatchID,
const RhoType& rhoOutlet,
const RhoType& rhoInlet
)
{
const fvPatch& p = patch();
const fvPatch& inletPatch = p.boundaryMesh()[inletPatchID];
const vectorField n(p.nf());
// Extrapolate patch velocity
vectorField Up(patchInternalField());
// Patch normal extrapolated velocity
scalarField nUp(n & Up);
// Remove the normal component of the extrapolate patch velocity
Up -= nUp*n;
// Remove any reverse flow
nUp = max(nUp, scalar(0));
// Lookup non-const access to velocity field
volVectorField& U
(
const_cast<volVectorField&>
(
dynamic_cast<const volVectorField&>(internalField())
)
);
// Get the corresponding inlet velocity patch field
fvPatchVectorField& inletPatchU = U.boundaryFieldRef()[inletPatchID];
// Ensure that the corresponding inlet velocity patch field is up-to-date
inletPatchU.updateCoeffs();
// Calculate the inlet patch flow rate
const scalar flowRate = -gSum(rhoInlet*(inletPatch.Sf() & inletPatchU));
// Calculate the extrapolated outlet patch flow rate
const scalar estimatedFlowRate = gSum(rhoOutlet*(patch().magSf()*nUp));
if (estimatedFlowRate/flowRate > 0.5)
{
nUp *= (mag(flowRate)/mag(estimatedFlowRate));
}
else
{
nUp += ((flowRate - estimatedFlowRate)/gSum(rhoOutlet*patch().magSf()));
}
// Add the corrected normal component of velocity to the patch velocity
Up += nUp*n;
// Correct the patch velocity
operator==(Up);
}
void Foam::matchedFlowRateOutletVelocityFvPatchVectorField::updateCoeffs()
{
if (updated())
{
return;
}
// Find corresponding inlet patch
const label inletPatchID =
patch().patch().boundaryMesh().findPatchID(inletPatchName_);
if (inletPatchID < 0)
{
FatalErrorInFunction
<< "Unable to find inlet patch " << inletPatchName_
<< exit(FatalError);
}
if (volumetric_)
{
updateValues(inletPatchID, one(), one());
}
else
{
// Mass flow-rate
if (db().foundObject<volScalarField>(rhoName_))
{
const volScalarField& rho = db().lookupObject<volScalarField>
(
rhoName_
);
updateValues
(
inletPatchID,
rho.boundaryField()[patch().index()],
rho.boundaryField()[inletPatchID]
);
}
else
{
FatalErrorInFunction
<< "Cannot find density field " << rhoName_ << exit(FatalError);
}
}
fixedValueFvPatchVectorField::updateCoeffs();
}
void Foam::matchedFlowRateOutletVelocityFvPatchVectorField::write
(
Ostream& os
) const
{
fvPatchField<vector>::write(os);
os.writeKeyword("inletPatch")
<< inletPatchName_ << token::END_STATEMENT << nl;
if (!volumetric_)
{
os.writeKeyword("volumetric")
<< volumetric_ << token::END_STATEMENT << nl;
writeEntryIfDifferent<word>(os, "rho", "rho", rhoName_);
}
writeEntry("value", os);
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
makePatchTypeField
(
fvPatchVectorField,
matchedFlowRateOutletVelocityFvPatchVectorField
);
}
// ************************************************************************* //
/*---------------------------------------------------------------------------*\
========= |
\\ / 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::matchedFlowRateOutletVelocityFvPatchVectorField
Group
grpOutletBoundaryConditions
Description
Velocity outlet boundary condition which corrects the extrapolated velocity
to match the flow rate of the specified corresponding inlet patch.
Usage
\table
Property | Description | Required | Default value
inletPatch | Corresponding inlet patch name | yes |
volumetric | Set volumetric or mass flow-rate | no | false
rho | density field name | no | rho
\endtable
Example of the boundary condition specification for a volumetric flow rate:
\verbatim
<patchName>
{
type matchedFlowRateOutletVelocity;
inletPatch inlet;
value uniform (0 0 0);
}
\endverbatim
See also
Foam::fixedValueFvPatchField
SourceFiles
matchedFlowRateOutletVelocityFvPatchVectorField.C
\*---------------------------------------------------------------------------*/
#ifndef matchedFlowRateOutletVelocityFvPatchVectorField_H
#define matchedFlowRateOutletVelocityFvPatchVectorField_H
#include "fixedValueFvPatchFields.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
/*---------------------------------------------------------------------------*\
Class matchedFlowRateOutletVelocityFvPatchVectorField Declaration
\*---------------------------------------------------------------------------*/
class matchedFlowRateOutletVelocityFvPatchVectorField
:
public fixedValueFvPatchVectorField
{
// Private data
//- Inlet patch name from which the corresponding flow rate is obtained
word inletPatchName_;
//- Is volumetric?
bool volumetric_;
//- Name of the density field used to normalize the mass flux
word rhoName_;
// Private member functions
//- Update the patch values given the appropriate density type and value
template<class RhoType>
void updateValues
(
const label inletPatchID,
const RhoType& rhoOutlet,
const RhoType& rhoInlet
);
public:
//- Runtime type information
TypeName("matchedFlowRateOutletVelocity");
// Constructors
//- Construct from patch and internal field
matchedFlowRateOutletVelocityFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, volMesh>&
);
//- Construct from patch, internal field and dictionary
matchedFlowRateOutletVelocityFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, volMesh>&,
const dictionary&
);
//- Construct by mapping given
// matchedFlowRateOutletVelocityFvPatchVectorField
// onto a new patch
matchedFlowRateOutletVelocityFvPatchVectorField
(
const matchedFlowRateOutletVelocityFvPatchVectorField&,
const fvPatch&,
const DimensionedField<vector, volMesh>&,
const fvPatchFieldMapper&
);
//- Construct as copy
matchedFlowRateOutletVelocityFvPatchVectorField
(
const matchedFlowRateOutletVelocityFvPatchVectorField&
);
//- Construct and return a clone
virtual tmp<fvPatchVectorField> clone() const
{
return tmp<fvPatchVectorField>
(
new matchedFlowRateOutletVelocityFvPatchVectorField(*this)
);
}
//- Construct as copy setting internal field reference
matchedFlowRateOutletVelocityFvPatchVectorField
(
const matchedFlowRateOutletVelocityFvPatchVectorField&,
const DimensionedField<vector, volMesh>&
);
//- Construct and return a clone setting internal field reference
virtual tmp<fvPatchVectorField> clone
(
const DimensionedField<vector, volMesh>& iF
) const
{
return tmp<fvPatchVectorField>
(
new matchedFlowRateOutletVelocityFvPatchVectorField(*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
// ************************************************************************* //
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