Commit 6d414f11 authored by Henry Weller's avatar Henry Weller Committed by Andrew Heather
Browse files

flowRateOutletVelocityFvPatchVectorField: Outlet equivalent of...

flowRateOutletVelocityFvPatchVectorField: Outlet equivalent of flowRateOutletVelocityFvPatchVectorField BC

Velocity outlet boundary condition which corrects the extrapolated velocity to
match the specified flow rate.
parent b3b12470
......@@ -147,6 +147,7 @@ $(derivedFvPatchFields)/fixedMean/fixedMeanFvPatchFields.C
$(derivedFvPatchFields)/fixedNormalSlip/fixedNormalSlipFvPatchFields.C
$(derivedFvPatchFields)/fixedPressureCompressibleDensity/fixedPressureCompressibleDensityFvPatchScalarField.C
$(derivedFvPatchFields)/flowRateInletVelocity/flowRateInletVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/flowRateOutletVelocity/flowRateOutletVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/fluxCorrectedVelocity/fluxCorrectedVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/freestream/freestreamFvPatchFields.C
$(derivedFvPatchFields)/freestreamPressure/freestreamPressureFvPatchScalarField.C
......
......@@ -2,7 +2,7 @@
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2011-2016 OpenFOAM Foundation
\\ / A nd | Copyright (C) 2011-2017 OpenFOAM Foundation
\\/ M anipulation |
-------------------------------------------------------------------------------
License
......@@ -28,9 +28,9 @@ Group
grpInletBoundaryConditions
Description
This boundary condition provides a velocity boundary condition, derived
from the flux (volumetric or mass-based), whose direction is assumed
to be normal to the patch.
Velocity inlet boundary condition either correcting the extrapolated
velocity or creating a uniform velocity field normal to the patch adjusted
to match the specified flow rate
For a mass-based flux:
- the flow rate should be provided in kg/s
......@@ -87,6 +87,7 @@ Note
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
Foam::flowRateOutletVelocityFvPatchVectorField
SourceFiles
flowRateInletVelocityFvPatchVectorField.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 "flowRateOutletVelocityFvPatchVectorField.H"
#include "volFields.H"
#include "one.H"
#include "addToRunTimeSelectionTable.H"
// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
Foam::flowRateOutletVelocityFvPatchVectorField::
flowRateOutletVelocityFvPatchVectorField
(
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF
)
:
fixedValueFvPatchField<vector>(p, iF),
flowRate_(),
volumetric_(false),
rhoName_("rho"),
rhoOutlet_(0.0)
{}
Foam::flowRateOutletVelocityFvPatchVectorField::
flowRateOutletVelocityFvPatchVectorField
(
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF,
const dictionary& dict
)
:
fixedValueFvPatchField<vector>(p, iF, dict, false),
rhoOutlet_(dict.lookupOrDefault<scalar>("rhoOutlet", -VGREAT))
{
if (dict.found("volumetricFlowRate"))
{
volumetric_ = true;
flowRate_ = Function1<scalar>::New("volumetricFlowRate", dict);
rhoName_ = "rho";
}
else if (dict.found("massFlowRate"))
{
volumetric_ = false;
flowRate_ = Function1<scalar>::New("massFlowRate", dict);
rhoName_ = word(dict.lookupOrDefault<word>("rho", "rho"));
}
else
{
FatalIOErrorInFunction
(
dict
) << "Please supply either 'volumetricFlowRate' or"
<< " 'massFlowRate' and 'rho'" << exit(FatalIOError);
}
// Value field require if mass based
if (dict.found("value"))
{
fvPatchField<vector>::operator=
(
vectorField("value", dict, p.size())
);
}
else
{
evaluate(Pstream::commsTypes::blocking);
}
}
Foam::flowRateOutletVelocityFvPatchVectorField::
flowRateOutletVelocityFvPatchVectorField
(
const flowRateOutletVelocityFvPatchVectorField& ptf,
const fvPatch& p,
const DimensionedField<vector, volMesh>& iF,
const fvPatchFieldMapper& mapper
)
:
fixedValueFvPatchField<vector>(ptf, p, iF, mapper),
flowRate_(ptf.flowRate_, false),
volumetric_(ptf.volumetric_),
rhoName_(ptf.rhoName_),
rhoOutlet_(ptf.rhoOutlet_)
{}
Foam::flowRateOutletVelocityFvPatchVectorField::
flowRateOutletVelocityFvPatchVectorField
(
const flowRateOutletVelocityFvPatchVectorField& ptf
)
:
fixedValueFvPatchField<vector>(ptf),
flowRate_(ptf.flowRate_, false),
volumetric_(ptf.volumetric_),
rhoName_(ptf.rhoName_),
rhoOutlet_(ptf.rhoOutlet_)
{}
Foam::flowRateOutletVelocityFvPatchVectorField::
flowRateOutletVelocityFvPatchVectorField
(
const flowRateOutletVelocityFvPatchVectorField& ptf,
const DimensionedField<vector, volMesh>& iF
)
:
fixedValueFvPatchField<vector>(ptf, iF),
flowRate_(ptf.flowRate_, false),
volumetric_(ptf.volumetric_),
rhoName_(ptf.rhoName_),
rhoOutlet_(ptf.rhoOutlet_)
{}
// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
template<class RhoType>
void Foam::flowRateOutletVelocityFvPatchVectorField::updateValues
(
const RhoType& rho
)
{
const scalar t = db().time().timeOutputValue();
const vectorField n = patch().nf();
// Extrapolate patch velocity
vectorField Up(this->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 = min(nUp, 0.0);
const scalar flowRate = flowRate_->value(t);
const scalar estimatedFlowRate = -gSum(rho*(this->patch().magSf()*nUp));
if (estimatedFlowRate/flowRate > 0.5)
{
nUp *= (mag(flowRate)/mag(estimatedFlowRate));
}
else
{
nUp -= ((flowRate - estimatedFlowRate)/gSum(rho*patch().magSf()));
}
// Add the corrected normal component of velocity to the patch velocity
Up += nUp*n;
// Correct the patch velocity
this->operator==(Up);
}
void Foam::flowRateOutletVelocityFvPatchVectorField::updateCoeffs()
{
if (updated())
{
return;
}
if (volumetric_ || rhoName_ == "none")
{
updateValues(one());
}
else
{
// Mass flow-rate
if (db().foundObject<volScalarField>(rhoName_))
{
const fvPatchField<scalar>& rhop =
patch().lookupPatchField<volScalarField, scalar>(rhoName_);
updateValues(rhop);
}
else
{
// Use constant density
if (rhoOutlet_ < 0)
{
FatalErrorInFunction
<< "Did not find registered density field " << rhoName_
<< " and no constant density 'rhoOutlet' specified"
<< exit(FatalError);
}
updateValues(rhoOutlet_);
}
}
fixedValueFvPatchVectorField::updateCoeffs();
}
void Foam::flowRateOutletVelocityFvPatchVectorField::write(Ostream& os) const
{
fvPatchField<vector>::write(os);
flowRate_->writeData(os);
if (!volumetric_)
{
writeEntryIfDifferent<word>(os, "rho", "rho", rhoName_);
writeEntryIfDifferent<scalar>(os, "rhoOutlet", -VGREAT, rhoOutlet_);
}
writeEntry("value", os);
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
makePatchTypeField
(
fvPatchVectorField,
flowRateOutletVelocityFvPatchVectorField
);
}
// ************************************************************************* //
/*---------------------------------------------------------------------------*\
========= |
\\ / 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::flowRateOutletVelocityFvPatchVectorField
Group
grpOutletBoundaryConditions
Description
Velocity outlet boundary condition which corrects the extrapolated velocity
to match the specified flow rate.
For a mass-based flux:
- the flow rate should be provided in kg/s
- if \c rho is "none" the flow rate is in m^3/s
- otherwise \c rho should correspond to the name of the density field
- if the density field cannot be found in the database, the user must
specify the outlet density using the \c rhoOutlet entry
For a volumetric-based flux:
- the flow rate is in m^3/s
Usage
\table
Property | Description | Required | Default value
massFlowRate | mass flow rate [kg/s] | no |
volumetricFlowRate | volumetric flow rate [m^3/s]| no |
rhoOutlet | outlet density | no |
\endtable
Example of the boundary condition specification for a volumetric flow rate:
\verbatim
<patchName>
{
type flowRateOutletVelocity;
volumetricFlowRate 0.2;
value uniform (0 0 0);
}
\endverbatim
Example of the boundary condition specification for a mass flow rate:
\verbatim
<patchName>
{
type flowRateOutletVelocity;
massFlowRate 0.2;
rhoOutlet 1.0;
value uniform (0 0 0);
}
\endverbatim
The \c flowRate entry is a \c Function1 of time, see Foam::Function1Types.
Note
- \c rhoOutlet is required for the case of a mass flow rate, where the
density field is not available at start-up
- The value is positive out of the domain (as an outlet)
- May not work correctly for transonic outlets
- Strange behaviour with potentialFoam since the U equation is not solved
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
Foam::flowRateInletVelocityFvPatchVectorField
SourceFiles
flowRateOutletVelocityFvPatchVectorField.C
\*---------------------------------------------------------------------------*/
#ifndef flowRateOutletVelocityFvPatchVectorField_H
#define flowRateOutletVelocityFvPatchVectorField_H
#include "fixedValueFvPatchFields.H"
#include "Function1.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
/*---------------------------------------------------------------------------*\
Class flowRateOutletVelocityFvPatchVectorField Declaration
\*---------------------------------------------------------------------------*/
class flowRateOutletVelocityFvPatchVectorField
:
public fixedValueFvPatchVectorField
{
// Private data
//- Outlet integral flow rate
autoPtr<Function1<scalar>> flowRate_;
//- Is volumetric?
bool volumetric_;
//- Name of the density field used to normalize the mass flux
word rhoName_;
//- Rho initialisation value (for start; if value not supplied)
scalar rhoOutlet_;
// Private member functions
//- Update the patch values given the appropriate density type and value
template<class RhoType>
void updateValues(const RhoType& rho);
public:
//- Runtime type information
TypeName("flowRateOutletVelocity");
// Constructors
//- Construct from patch and internal field
flowRateOutletVelocityFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, volMesh>&
);
//- Construct from patch, internal field and dictionary
flowRateOutletVelocityFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, volMesh>&,
const dictionary&
);
//- Construct by mapping given
// flowRateOutletVelocityFvPatchVectorField
// onto a new patch
flowRateOutletVelocityFvPatchVectorField
(
const flowRateOutletVelocityFvPatchVectorField&,
const fvPatch&,
const DimensionedField<vector, volMesh>&,
const fvPatchFieldMapper&
);
//- Construct as copy
flowRateOutletVelocityFvPatchVectorField
(
const flowRateOutletVelocityFvPatchVectorField&
);
//- Construct and return a clone
virtual tmp<fvPatchVectorField> clone() const
{
return tmp<fvPatchVectorField>
(
new flowRateOutletVelocityFvPatchVectorField(*this)
);
}
//- Construct as copy setting internal field reference
flowRateOutletVelocityFvPatchVectorField
(
const flowRateOutletVelocityFvPatchVectorField&,
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 flowRateOutletVelocityFvPatchVectorField(*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