From 5db676551b3a6614cc4b9a5b9cd4011df04e760b Mon Sep 17 00:00:00 2001
From: Henry Weller <http://openfoam.org>
Date: Mon, 17 Jul 2017 15:48:39 +0100
Subject: [PATCH] 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.
---
...FlowRateOutletVelocityFvPatchVectorField.C | 271 ++++++++++++++++++
...FlowRateOutletVelocityFvPatchVectorField.H | 189 ++++++++++++
2 files changed, 460 insertions(+)
create mode 100644 src/finiteVolume/fields/fvPatchFields/derived/matchedFlowRateOutletVelocity/matchedFlowRateOutletVelocityFvPatchVectorField.C
create mode 100644 src/finiteVolume/fields/fvPatchFields/derived/matchedFlowRateOutletVelocity/matchedFlowRateOutletVelocityFvPatchVectorField.H
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/matchedFlowRateOutletVelocity/matchedFlowRateOutletVelocityFvPatchVectorField.C b/src/finiteVolume/fields/fvPatchFields/derived/matchedFlowRateOutletVelocity/matchedFlowRateOutletVelocityFvPatchVectorField.C
new file mode 100644
index 0000000000..4ea359ee5b
--- /dev/null
+++ b/src/finiteVolume/fields/fvPatchFields/derived/matchedFlowRateOutletVelocity/matchedFlowRateOutletVelocityFvPatchVectorField.C
@@ -0,0 +1,271 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / 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
+ );
+}
+
+
+// ************************************************************************* //
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/matchedFlowRateOutletVelocity/matchedFlowRateOutletVelocityFvPatchVectorField.H b/src/finiteVolume/fields/fvPatchFields/derived/matchedFlowRateOutletVelocity/matchedFlowRateOutletVelocityFvPatchVectorField.H
new file mode 100644
index 0000000000..2442e081f5
--- /dev/null
+++ b/src/finiteVolume/fields/fvPatchFields/derived/matchedFlowRateOutletVelocity/matchedFlowRateOutletVelocityFvPatchVectorField.H
@@ -0,0 +1,189 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / 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
+
+// ************************************************************************* //
--
GitLab