From f6abc9b4711f3721c74e8b0260456b8c98925777 Mon Sep 17 00:00:00 2001
From: mattijs <mattijs>
Date: Mon, 23 Nov 2015 17:39:43 +0000
Subject: [PATCH] ENH: pressurePIDControlInletVelocity: new BC to match
velocity to user-provided pressure drop
- user provides two planes and pressure drop across these
- bc assume potential flow and works out inlet velocity that would cause
an equivalent pressure drop
---
src/finiteVolume/Make/files | 1 +
...IDControlInletVelocityFvPatchVectorField.C | 438 ++++++++++++++++++
...IDControlInletVelocityFvPatchVectorField.H | 279 +++++++++++
3 files changed, 718 insertions(+)
create mode 100644 src/finiteVolume/fields/fvPatchFields/derived/pressurePIDControlInletVelocity/pressurePIDControlInletVelocityFvPatchVectorField.C
create mode 100644 src/finiteVolume/fields/fvPatchFields/derived/pressurePIDControlInletVelocity/pressurePIDControlInletVelocityFvPatchVectorField.H
diff --git a/src/finiteVolume/Make/files b/src/finiteVolume/Make/files
index 3dec7db1683..0b23bd4237e 100644
--- a/src/finiteVolume/Make/files
+++ b/src/finiteVolume/Make/files
@@ -168,6 +168,7 @@ $(derivedFvPatchFields)/pressureInletOutletVelocity/pressureInletOutletVelocityF
$(derivedFvPatchFields)/pressureInletUniformVelocity/pressureInletUniformVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/pressureInletVelocity/pressureInletVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/pressureNormalInletOutletVelocity/pressureNormalInletOutletVelocityFvPatchVectorField.C
+$(derivedFvPatchFields)/pressurePIDControlInletVelocity/pressurePIDControlInletVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/fixedNormalInletOutletVelocity/fixedNormalInletOutletVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/rotatingPressureInletOutletVelocity/rotatingPressureInletOutletVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/rotatingTotalPressure/rotatingTotalPressureFvPatchScalarField.C
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/pressurePIDControlInletVelocity/pressurePIDControlInletVelocityFvPatchVectorField.C b/src/finiteVolume/fields/fvPatchFields/derived/pressurePIDControlInletVelocity/pressurePIDControlInletVelocityFvPatchVectorField.C
new file mode 100644
index 00000000000..b7d36f1a6da
--- /dev/null
+++ b/src/finiteVolume/fields/fvPatchFields/derived/pressurePIDControlInletVelocity/pressurePIDControlInletVelocityFvPatchVectorField.C
@@ -0,0 +1,438 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2015 OpenCFD Ltd.
+ \\/ 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 "pressurePIDControlInletVelocityFvPatchVectorField.H"
+#include "volFields.H"
+#include "addToRunTimeSelectionTable.H"
+#include "fvPatchFieldMapper.H"
+#include "surfaceFields.H"
+#include "linear.H"
+#include "steadyStateDdtScheme.H"
+
+// * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * * //
+
+const Foam::surfaceScalarField&
+Foam::pressurePIDControlInletVelocityFvPatchVectorField::facePressure() const
+{
+ const volScalarField& p(db().lookupObject<volScalarField>(pName_));
+
+ const word pfName(pName_ + "f");
+
+ if (!db().foundObject<surfaceScalarField>(pfName))
+ {
+ surfaceScalarField* pfPtr
+ (
+ new surfaceScalarField(pfName, linearInterpolate(p))
+ );
+
+ pfPtr->store();
+ }
+
+ surfaceScalarField& pf
+ (
+ const_cast<surfaceScalarField&>
+ (
+ db().lookupObject<surfaceScalarField>(pfName)
+ )
+ );
+
+ if (!pf.upToDate(p))
+ {
+ pf = linearInterpolate(p);
+ }
+
+ return pf;
+}
+
+
+template <class Type>
+void Foam::pressurePIDControlInletVelocityFvPatchVectorField::faceZoneAverage
+(
+ const word& name,
+ const GeometricField<Type, fvsPatchField, surfaceMesh>& field,
+ scalar& area,
+ Type& average
+) const
+{
+ const fvMesh& mesh(patch().boundaryMesh().mesh());
+
+ const faceZone& zone = mesh.faceZones()[name];
+
+ area = 0;
+ average = pTraits<Type>::zero;
+
+ forAll(zone, faceI)
+ {
+ const label f(zone[faceI]);
+
+ const scalar da(mesh.magSf()[f]);
+
+ area += da;
+ average += da*field[f];
+ }
+
+ reduce(area, sumOp<scalar>());
+ reduce(average, sumOp<Type>());
+
+ average /= area;
+}
+
+
+// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
+
+Foam::pressurePIDControlInletVelocityFvPatchVectorField::
+pressurePIDControlInletVelocityFvPatchVectorField
+(
+ const fvPatch& p,
+ const DimensionedField<vector, volMesh>& iF
+)
+:
+ fixedValueFvPatchField<vector>(p, iF),
+ upstreamName_(word::null),
+ downstreamName_(word::null),
+ deltaP_(1),
+ shapeFactor_(0),
+ pName_("p"),
+ phiName_("phi"),
+ rhoName_("none"),
+ P_(0),
+ I_(0),
+ D_(0),
+ Q_(- gSum(*this & patch().Sf())),
+ error_(0),
+ errorIntegral_(0),
+ oldQ_(0),
+ oldError_(0),
+ oldErrorIntegral_(0),
+ timeIndex_(db().time().timeIndex())
+{}
+
+
+Foam::pressurePIDControlInletVelocityFvPatchVectorField::
+pressurePIDControlInletVelocityFvPatchVectorField
+(
+ const pressurePIDControlInletVelocityFvPatchVectorField& ptf,
+ const fvPatch& p,
+ const DimensionedField<vector, volMesh>& iF,
+ const fvPatchFieldMapper& mapper
+)
+:
+ fixedValueFvPatchField<vector>(ptf, p, iF, mapper),
+ upstreamName_(ptf.upstreamName_),
+ downstreamName_(ptf.downstreamName_),
+ deltaP_(ptf.deltaP_),
+ shapeFactor_(ptf.shapeFactor_),
+ pName_(ptf.pName_),
+ phiName_(ptf.phiName_),
+ rhoName_(ptf.rhoName_),
+ P_(ptf.P_),
+ I_(ptf.I_),
+ D_(ptf.D_),
+ Q_(ptf.Q_),
+ error_(ptf.error_),
+ errorIntegral_(ptf.errorIntegral_),
+ oldQ_(ptf.oldQ_),
+ oldError_(ptf.oldError_),
+ oldErrorIntegral_(ptf.oldErrorIntegral_),
+ timeIndex_(ptf.timeIndex_)
+{}
+
+
+Foam::pressurePIDControlInletVelocityFvPatchVectorField::
+pressurePIDControlInletVelocityFvPatchVectorField
+(
+ const fvPatch& p,
+ const DimensionedField<vector, volMesh>& iF,
+ const dictionary& dict
+)
+:
+ fixedValueFvPatchField<vector>(p, iF, dict),
+ upstreamName_(dict.lookup("upstream")),
+ downstreamName_(dict.lookup("downstream")),
+ deltaP_(readScalar(dict.lookup("deltaP"))),
+ shapeFactor_(dict.lookupOrDefault<scalar>("shapeFactor", 0)),
+ pName_(dict.lookupOrDefault<word>("p", "p")),
+ phiName_(dict.lookupOrDefault<word>("phi", "phi")),
+ rhoName_(dict.lookupOrDefault<word>("rho", "none")),
+ P_(readScalar(dict.lookup("P"))),
+ I_(readScalar(dict.lookup("I"))),
+ D_(readScalar(dict.lookup("D"))),
+ Q_(- gSum(*this & patch().Sf())),
+ error_(dict.lookupOrDefault<scalar>("error", 0)),
+ errorIntegral_(dict.lookupOrDefault<scalar>("errorIntegral", 0)),
+ oldQ_(0),
+ oldError_(0),
+ oldErrorIntegral_(0),
+ timeIndex_(db().time().timeIndex())
+{}
+
+
+Foam::pressurePIDControlInletVelocityFvPatchVectorField::
+pressurePIDControlInletVelocityFvPatchVectorField
+(
+ const pressurePIDControlInletVelocityFvPatchVectorField& ptf
+)
+:
+ fixedValueFvPatchField<vector>(ptf),
+ upstreamName_(ptf.upstreamName_),
+ downstreamName_(ptf.downstreamName_),
+ deltaP_(ptf.deltaP_),
+ shapeFactor_(ptf.shapeFactor_),
+ pName_(ptf.pName_),
+ phiName_(ptf.phiName_),
+ rhoName_(ptf.rhoName_),
+ P_(ptf.P_),
+ I_(ptf.I_),
+ D_(ptf.D_),
+ Q_(ptf.Q_),
+ error_(ptf.error_),
+ errorIntegral_(ptf.errorIntegral_),
+ oldQ_(ptf.oldQ_),
+ oldError_(ptf.oldError_),
+ oldErrorIntegral_(ptf.oldErrorIntegral_),
+ timeIndex_(ptf.timeIndex_)
+{}
+
+
+Foam::pressurePIDControlInletVelocityFvPatchVectorField::
+pressurePIDControlInletVelocityFvPatchVectorField
+(
+ const pressurePIDControlInletVelocityFvPatchVectorField& ptf,
+ const DimensionedField<vector, volMesh>& iF
+)
+:
+ fixedValueFvPatchField<vector>(ptf, iF),
+ upstreamName_(ptf.upstreamName_),
+ downstreamName_(ptf.downstreamName_),
+ deltaP_(ptf.deltaP_),
+ shapeFactor_(ptf.shapeFactor_),
+ pName_(ptf.pName_),
+ phiName_(ptf.phiName_),
+ rhoName_(ptf.rhoName_),
+ P_(ptf.P_),
+ I_(ptf.I_),
+ D_(ptf.D_),
+ Q_(ptf.Q_),
+ error_(ptf.error_),
+ errorIntegral_(ptf.errorIntegral_),
+ oldQ_(ptf.oldQ_),
+ oldError_(ptf.oldError_),
+ oldErrorIntegral_(ptf.oldErrorIntegral_),
+ timeIndex_(ptf.timeIndex_)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
+
+void Foam::pressurePIDControlInletVelocityFvPatchVectorField::updateCoeffs()
+{
+ if (updated())
+ {
+ return;
+ }
+
+ // Get the mesh
+ const fvMesh& mesh(patch().boundaryMesh().mesh());
+
+ // Get the time step
+ const scalar deltaT(db().time().deltaTValue());
+
+ // Get the flux field
+ const surfaceScalarField& phi
+ (
+ db().lookupObject<surfaceScalarField>(phiName_)
+ );
+
+ // Update the old-time quantities
+ if (timeIndex_ != db().time().timeIndex())
+ {
+ timeIndex_ = db().time().timeIndex();
+ oldQ_ = Q_;
+ oldError_ = error_;
+ oldErrorIntegral_ = errorIntegral_;
+ }
+
+ // Get the density
+ scalar rho = 1;
+ if (phi.dimensions() == dimVelocity*dimArea)
+ {
+ // do nothing ...
+ }
+ else if (phi.dimensions() == dimDensity*dimVelocity*dimArea)
+ {
+ const fvPatchField<scalar>& rhoField =
+ patch().lookupPatchField<volScalarField, scalar>(rhoName_);
+
+ rho = gSum(rhoField*patch().magSf())/gSum(patch().magSf());
+ }
+ else
+ {
+ FatalErrorIn
+ (
+ "void Foam::"
+ "pressurePIDControlInletVelocityFvPatchVectorField::"
+ "updateCoeffs()"
+ ) << "The dimensions of the field " << phiName_
+ << "are not recognised. The dimensions are " << phi.dimensions()
+ << ". The dimensions should be either " << dimVelocity*dimArea
+ << " for an incompressible case, or "
+ << dimDensity*dimVelocity*dimArea << " for a compressible case."
+ << exit(FatalError);
+ }
+
+ // Patch properties
+ const scalar patchA = gSum(patch().magSf());
+ Q_ = - gSum(*this & patch().Sf());
+
+ // Face-zone properties (a is upstream, b is downstream)
+ scalar Aa, Ab;
+ vector xa, xb;
+ faceZoneAverage(upstreamName_, mesh.Cf(), Aa, xa);
+ faceZoneAverage(downstreamName_, mesh.Cf(), Ab, xb);
+ const scalar L = mag(xa - xb);
+ const scalar LbyALinear = L/(Aa - Ab)*log(Aa/Ab);
+ const scalar LbyAStep = L/2*(1/Aa + 1/Ab);
+ const scalar LbyA = (1 - shapeFactor_)*LbyALinear + shapeFactor_*LbyAStep;
+
+ // Initialise the pressure drop. If the pressure field does not exist, the
+ // pressure drop is assumed to be that specified. This removes the error,
+ // so there is no control and the analytic inlet velocity is applied. This
+ // scenario only ever going to be applicable to potentialFoam.
+ scalar deltaP = deltaP_;
+ if (db().foundObject<volScalarField>(pName_))
+ {
+ scalar pa, pb;
+ faceZoneAverage(upstreamName_, facePressure(), Aa, pa);
+ faceZoneAverage(downstreamName_, facePressure(), Ab, pb);
+ deltaP = pa - pb;
+ }
+ else
+ {
+ WarningIn
+ (
+ "void Foam::pressurePIDControlInletVelocityFvPatchVectorField::"
+ "updateCoeffs()"
+ ) << "The pressure field name, \"pName\", is \"" << pName_ << "\", "
+ << "but a field of that name was not found. The inlet velocity "
+ << "will be set to an analytical value calculated from the "
+ << "specified pressure drop. No PID control will be done and "
+ << "transient effects will be ignored. This behaviour is designed "
+ << "to be appropriate for potentialFoam solutions. If you are "
+ << "getting this warning from another solver, you have probably "
+ << "specified an incorrect pressure name."
+ << endl << endl;
+ }
+
+ // Target and measured flow rates
+ scalar QTarget, QMeasured;
+ const scalar a = (1/sqr(Ab) - 1/sqr(Aa))/(2*rho);
+ if (!mesh.steady() && db().foundObject<volScalarField>(pName_))
+ {
+ const scalar b = LbyA/deltaT;
+ const scalar c = - LbyA/deltaT*oldQ_ /* - deltaP */;
+ QTarget = (- b + sqrt(sqr(b) - 4*a*(c - deltaP_)))/(2*a);
+ QMeasured = (- b + sqrt(sqr(b) - 4*a*(c - deltaP)))/(2*a);
+ }
+ else
+ {
+ QTarget = sqrt(deltaP_/a);
+ QMeasured = sqrt(deltaP/a);
+ }
+
+ // Errors
+ error_ = QTarget - QMeasured;
+ errorIntegral_ = oldErrorIntegral_ + 0.5*(error_ + oldError_);
+ const scalar errorDifferential = oldError_ - error_;
+
+ // Update the field
+ operator==
+ (
+ - patch().nf()
+ *(
+ QTarget
+ + P_*error_
+ + I_*errorIntegral_
+ + D_*errorDifferential
+ )/patchA
+ );
+
+ // Log output
+ if (debug)
+ {
+ const dimensionSet pDimensions(phi.dimensions()*dimVelocity/dimArea);
+ const scalar error = deltaP/deltaP_ - 1;
+ const scalar newQ = - gSum(*this & patch().Sf());
+ Info<< "pressurePIDControlInletVelocityFvPatchField " << patch().name()
+ << endl << " "
+ << dimensionedScalar("U", dimVelocity, newQ/patchA)
+ << endl << " "
+ << dimensionedScalar("deltaP", pDimensions, deltaP)
+ << " (" << mag(error)*100 << "\% "
+ << (error < 0 ? "below" : "above") << " the target)" << endl;
+ }
+
+ fixedValueFvPatchField<vector>::updateCoeffs();
+}
+
+
+void Foam::pressurePIDControlInletVelocityFvPatchVectorField::write
+(
+ Ostream& os
+) const
+{
+ fvPatchField<vector>::write(os);
+
+ os.writeKeyword("deltaP") << deltaP_ << token::END_STATEMENT << nl;
+ os.writeKeyword("upstream") << upstreamName_ << token::END_STATEMENT << nl;
+ os.writeKeyword("downstream")
+ << downstreamName_ << token::END_STATEMENT << nl;
+ os.writeKeyword("shapeFactor") << shapeFactor_
+ << token::END_STATEMENT << nl;
+ writeEntryIfDifferent<word>(os, "p", "p", pName_);
+ writeEntryIfDifferent<word>(os, "rho", "none", rhoName_);
+ os.writeKeyword("P") << P_ << token::END_STATEMENT << nl;
+ os.writeKeyword("I") << I_ << token::END_STATEMENT << nl;
+ os.writeKeyword("D") << D_ << token::END_STATEMENT << nl;
+ os.writeKeyword("error") << error_ << token::END_STATEMENT << nl;
+ os.writeKeyword("errorIntegral")
+ << errorIntegral_ << token::END_STATEMENT << nl;
+
+ writeEntry("value", os);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+ makePatchTypeField
+ (
+ fvPatchVectorField,
+ pressurePIDControlInletVelocityFvPatchVectorField
+ );
+}
+
+
+// ************************************************************************* //
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/pressurePIDControlInletVelocity/pressurePIDControlInletVelocityFvPatchVectorField.H b/src/finiteVolume/fields/fvPatchFields/derived/pressurePIDControlInletVelocity/pressurePIDControlInletVelocityFvPatchVectorField.H
new file mode 100644
index 00000000000..d6f6cf765e5
--- /dev/null
+++ b/src/finiteVolume/fields/fvPatchFields/derived/pressurePIDControlInletVelocity/pressurePIDControlInletVelocityFvPatchVectorField.H
@@ -0,0 +1,279 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2015 OpenCFD Ltd.
+ \\/ 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::pressurePIDControlInletVelocityFvPatchVectorField
+
+Group
+ grpInletBoundaryConditions
+
+Description
+ This boundary condition tries to generate an inlet velocity that maintains
+ a specified pressure drop between two face zones downstream. The zones
+ should fully span a duct through which all the inlet flow passes.
+
+ An incompressible, lossless analysis of the flow between the inlet and the
+ two face-zones is performed. An ideal inlet velocity is thereby calculated
+ from the user-specified pressure drop. This analysis can include the
+ transient effect of the inlet velocity change. In this case, a shape factor
+ is included to represent non-linearity in the duct cross section.
+
+ The average pressure drop between the two face zones is measured. The same
+ incompressible, lossless analysis is performed using this pressure drop.
+ The difference between the two computed velocities is considered as an
+ error. The ideal inlet is modified so as to drive this error to zero. This
+ is accomplished by means of a PID control algorithm, for which
+ non-dimensional gains are specified by the user.
+
+ The shape factor takes a value of 0 for a linear change in cross sectional
+ area between the two face zones. A value of 1 represents a step change in
+ area at the mid-point between the zones. A smooth cubic or cosine profile
+ between two zones with zero divergence is typically represented by a factor
+ of between 0.2 and 0.25.
+
+ \heading Patch usage
+
+ \table
+ Property | Description | Required | Default value
+ upstream | upstream face zone name | yes |
+ downstream | downstream face zone name | yes |
+ deltaP | desired pressure drop | yes |
+ shapeFactor | non-linearity in the nozzle | no | 0
+ p | pressure field name | no | p
+ phi | flux field name | yes | phi
+ rho | density field name | no | none
+ P | proportional gain | yes |
+ I | integral gain | yes |
+ D | differential gain | yes |
+ \endtable
+
+ Example of the boundary condition specification:
+
+ \verbatim
+ myPatch
+ {
+ type pressurePIDControlInletVelocity;
+ upstream upstream;
+ downstream downstream;
+ deltaP 200;
+ shapeFactor 0;
+ p p;
+ phi phi;
+ rho none;
+ P 0.5;
+ I 0.5;
+ D 0.1;
+ value uniform (0 0 0);
+ }
+
+SeeAlso
+ Foam::fixedValueFvPatchField
+
+SourceFiles
+ pressurePIDControlInletVelocityFvPatchVectorField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef pressurePIDControlInletVelocityFvPatchVectorField_H
+#define pressurePIDControlInletVelocityFvPatchVectorField_H
+
+#include "fixedValueFvPatchFields.H"
+#include "Switch.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+/*---------------------------------------------------------------------------*\
+ Class pressurePIDControlInletVelocityFvPatchVectorField Declaration
+\*---------------------------------------------------------------------------*/
+
+class pressurePIDControlInletVelocityFvPatchVectorField
+:
+ public fixedValueFvPatchVectorField
+{
+ // Private data
+
+ //- Name of the upstream face zone
+ const word upstreamName_;
+
+ //- Name of the downstream face zone
+ const word downstreamName_;
+
+ //- Desired pressure difference between upstream and downstream
+ const scalar deltaP_;
+
+ //- Nozzle shape factor
+ const scalar shapeFactor_;
+
+ //- Name of the pressure field
+ const word pName_;
+
+ //- Name of the flux field
+ const word phiName_;
+
+ //- Name of the density field (if any)
+ const word rhoName_;
+
+ //- Proportional gain
+ const scalar P_;
+
+ //- Integral gain
+ const scalar I_;
+
+ //- Derivative gain
+ const scalar D_;
+
+ //- Volumetric flow rate
+ scalar Q_;
+
+ //- Error
+ scalar error_;
+
+ //- Error integral w.r.t. time
+ scalar errorIntegral_;
+
+ //- Old volumetric flow rate
+ scalar oldQ_;
+
+ //- Old error
+ scalar oldError_;
+
+ //- Old error integral w.r.t. time
+ scalar oldErrorIntegral_;
+
+ //- Time index of the last update
+ label timeIndex_;
+
+
+ // Private member functions
+
+ //- Return the pressure interpolated to the faces
+ const surfaceScalarField& facePressure() const;
+
+ //- Calculate the average on a face zone
+ template <class Type>
+ void faceZoneAverage
+ (
+ const word& name,
+ const GeometricField<Type, fvsPatchField, surfaceMesh>& field,
+ scalar& area,
+ Type& average
+ ) const;
+
+
+public:
+
+ //- Runtime type information
+ TypeName("pressurePIDControlInletVelocity");
+
+
+ // Constructors
+
+ //- Construct from patch and internal field
+ pressurePIDControlInletVelocityFvPatchVectorField
+ (
+ const fvPatch&,
+ const DimensionedField<vector, volMesh>&
+ );
+
+ //- Construct from patch, internal field and dictionary
+ pressurePIDControlInletVelocityFvPatchVectorField
+ (
+ const fvPatch&,
+ const DimensionedField<vector, volMesh>&,
+ const dictionary&
+ );
+
+ //- Construct by mapping given
+ // flowRateInletVelocityFvPatchVectorField
+ // onto a new patch
+ pressurePIDControlInletVelocityFvPatchVectorField
+ (
+ const pressurePIDControlInletVelocityFvPatchVectorField&,
+ const fvPatch&,
+ const DimensionedField<vector, volMesh>&,
+ const fvPatchFieldMapper&
+ );
+
+ //- Construct as copy
+ pressurePIDControlInletVelocityFvPatchVectorField
+ (
+ const pressurePIDControlInletVelocityFvPatchVectorField&
+ );
+
+ //- Construct and return a clone
+ virtual tmp<fvPatchVectorField> clone() const
+ {
+ return tmp<fvPatchVectorField>
+ (
+ new pressurePIDControlInletVelocityFvPatchVectorField
+ (
+ *this
+ )
+ );
+ }
+
+ //- Construct as copy setting internal field reference
+ pressurePIDControlInletVelocityFvPatchVectorField
+ (
+ const pressurePIDControlInletVelocityFvPatchVectorField&,
+ 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 pressurePIDControlInletVelocityFvPatchVectorField
+ (
+ *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