flowRateOutletVelocityFvPatchVectorField: Outlet equivalent of flowRateOutletVelocityFvPatchVectorField BC

Velocity outlet boundary condition which corrects the extrapolated velocity to
match the specified flow rate.

src/finiteVolume/Make/files

@@ -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

src/finiteVolume/fields/fvPatchFields/derived/flowRateInletVelocity/flowRateInletVelocityFvPatchVectorField.H

@@ -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
+    Velocity inlet boundary condition either correcting the extrapolated
-    from the flux (volumetric or mass-based), whose direction is assumed
+    velocity or creating a uniform velocity field normal to the patch adjusted
-    to be normal to the patch.
+    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

src/finiteVolume/fields/fvPatchFields/derived/flowRateOutletVelocity/flowRateOutletVelocityFvPatchVectorField.C

@@ -0,0 +1,250 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  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
+   );
+}
+
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/flowRateOutletVelocity/flowRateOutletVelocityFvPatchVectorField.H

@@ -0,0 +1,220 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  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
+
+// ************************************************************************* //