Added a varying aoa boundary condition

src/adjoint/Make/files_Compressible

@@ -91,6 +91,7 @@ DASolver/DATurboFoam/DATurboFoam.C
 
 boundaryConditions/multiFreqVector/multiFreqVectorFvPatchField.C
 boundaryConditions/nutUSpaldingWallFunctionDF/nutUSpaldingWallFunctionFvPatchScalarFieldDF.C
+boundaryConditions/varyingFlowDirection/varyingFlowDirectionFvPatchVectorField.C
 models/dummyTurbulenceModel/makeDummyTurbulenceModelCompressible.C
 models/SpalartAllmarasFv3/makeSpalartAllmarasFv3Compressible.C
 models/SpalartAllmarasFv3FieldInversion/makeSpalartAllmarasFv3FieldInversionCompressible.C

src/adjoint/Make/files_Incompressible

@@ -102,6 +102,7 @@ DASolver/DAPimpleDyMFoam/DAPimpleDyMFoam.C
 
 boundaryConditions/multiFreqVector/multiFreqVectorFvPatchField.C
 boundaryConditions/nutUSpaldingWallFunctionDF/nutUSpaldingWallFunctionFvPatchScalarFieldDF.C
+boundaryConditions/varyingFlowDirection/varyingFlowDirectionFvPatchVectorField.C
 models/dummyTurbulenceModel/makeDummyTurbulenceModelIncompressible.C
 models/SpalartAllmarasFv3/makeSpalartAllmarasFv3Incompressible.C
 models/SpalartAllmarasFv3FieldInversion/makeSpalartAllmarasFv3FieldInversionIncompressible.C

src/adjoint/boundaryConditions/varyingFlowDirection/varyingFlowDirectionFvPatchVectorField.C

@@ -0,0 +1,158 @@
+/*---------------------------------------------------------------------------*\
+
+    DAFoam  : Discrete Adjoint with OpenFOAM
+    Version : v3
+
+    This file is modified from OpenFOAM's source code
+    src/finiteVolume/fields/fvPatchFields/basic/fixedValue/fixedValueFvPatchField.C
+
+    OpenFOAM: The Open Source CFD Toolbox
+
+    Copyright (C): 2011-2016 OpenFOAM Foundation
+
+    OpenFOAM License:
+
+        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 "varyingFlowDirectionFvPatchVectorField.H"
+#include "volFields.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::varyingFlowDirectionFvPatchVectorField::varyingFlowDirectionFvPatchVectorField(
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF)
+    : fixedValueFvPatchVectorField(p, iF),
+      UMag_(0.0),
+      flowDir_("x"),
+      normalDir_("y"),
+      alpha0_(0),
+      rate_(0)
+{
+}
+
+Foam::varyingFlowDirectionFvPatchVectorField::varyingFlowDirectionFvPatchVectorField(
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF,
+    const dictionary& dict)
+    : fixedValueFvPatchVectorField(p, iF),
+      UMag_(dict.lookupOrDefault<scalar>("UMag", 0.0)),
+      flowDir_(dict.lookupOrDefault<word>("flowDir", "x")),
+      normalDir_(dict.lookupOrDefault<word>("normalDir", "y")),
+      alpha0_(dict.lookupOrDefault<scalar>("alpha0", 0.0)),
+      rate_(dict.lookupOrDefault<scalar>("rate", 0.0))
+{
+
+    if (dict.found("value"))
+    {
+        fvPatchVectorField::operator=(
+            vectorField("value", dict, p.size()));
+    }
+    else
+    {
+        this->evaluate();
+    }
+}
+
+Foam::varyingFlowDirectionFvPatchVectorField::varyingFlowDirectionFvPatchVectorField(
+    const varyingFlowDirectionFvPatchVectorField& ptf,
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF,
+    const fvPatchFieldMapper& mapper)
+    : fixedValueFvPatchVectorField(p, iF),
+      UMag_(ptf.UMag_),
+      flowDir_(ptf.flowDir_),
+      normalDir_(ptf.normalDir_),
+      alpha0_(ptf.alpha0_),
+      rate_(ptf.rate_)
+{
+    this->evaluate();
+}
+
+Foam::varyingFlowDirectionFvPatchVectorField::varyingFlowDirectionFvPatchVectorField(
+    const varyingFlowDirectionFvPatchVectorField& wbppsf)
+    : fixedValueFvPatchVectorField(wbppsf),
+      UMag_(wbppsf.UMag_),
+      flowDir_(wbppsf.flowDir_),
+      normalDir_(wbppsf.normalDir_),
+      alpha0_(wbppsf.alpha0_),
+      rate_(wbppsf.rate_)
+{
+    this->evaluate();
+}
+
+Foam::varyingFlowDirectionFvPatchVectorField::varyingFlowDirectionFvPatchVectorField(
+    const varyingFlowDirectionFvPatchVectorField& wbppsf,
+    const DimensionedField<vector, volMesh>& iF)
+    : fixedValueFvPatchVectorField(wbppsf, iF),
+      UMag_(wbppsf.UMag_),
+      flowDir_(wbppsf.flowDir_),
+      normalDir_(wbppsf.normalDir_),
+      alpha0_(wbppsf.alpha0_),
+      rate_(wbppsf.rate_)
+{
+    this->evaluate();
+}
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+void Foam::varyingFlowDirectionFvPatchVectorField::updateCoeffs()
+{
+    // calculate patch values
+    const scalar t = this->db().time().timeOutputValue();
+    scalar alpha = alpha0_ + t * rate_;
+
+    HashTable<label> compTable;
+    compTable.set("x", 0);
+    compTable.set("y", 1);
+    compTable.set("z", 2);
+
+    vectorField& thisPatchRef = *this;
+    vectorField thisPatch = thisPatchRef;
+    forAll(thisPatch, idxI) 
+    {
+        label compFlow = compTable[flowDir_];
+        label compNormal = compTable[normalDir_];
+        thisPatch[idxI][compFlow] = UMag_ * cos(alpha);
+        thisPatch[idxI][compNormal] = UMag_ * sin(alpha);
+    }
+
+    fvPatchVectorField::operator==(thisPatch);
+
+    fixedValueFvPatchVectorField::updateCoeffs();
+}
+
+void Foam::varyingFlowDirectionFvPatchVectorField::write(Ostream& os) const
+{
+    fixedValueFvPatchVectorField::write(os);
+    os.writeEntry("UMag", UMag_);
+    os.writeEntry("flowDir", flowDir_);
+    os.writeEntry("normalDir", normalDir_);
+    os.writeEntry("alpha0", alpha0_);
+    os.writeEntry("rate", rate_);
+    //writeEntry("value", os);
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+makePatchTypeField(
+    fvPatchVectorField,
+    varyingFlowDirectionFvPatchVectorField);
+}
+
+// ************************************************************************* //

src/adjoint/boundaryConditions/varyingFlowDirection/varyingFlowDirectionFvPatchVectorField.H

@@ -0,0 +1,154 @@
+/*---------------------------------------------------------------------------*\
+
+    DAFoam  : Discrete Adjoint with OpenFOAM
+    Version : v3
+
+    This file is modified from OpenFOAM's source code
+    src/finiteVolume/fields/fvPatchFields/basic/fixedValue/fixedValueFvPatchField.H
+
+    OpenFOAM: The Open Source CFD Toolbox
+
+    Copyright (C): 2011-2016 OpenFOAM Foundation
+
+    OpenFOAM License:
+
+        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/>.
+
+    Description:
+
+        This boundary condition provides a varying flow direction at the far field
+
+        U_flowDir = UMag * cos(alpha)
+        U_normalDir = UMag * sin(alpha)
+        alpha = alpha0 + rate * t
+
+        where
+
+        U_flowDir    : velocity component parallel to the flow. Options are: x, y, or z
+        U_normalDir  : velocity component normal to the flow. Options are: x, y, or z
+        UMag         : velocity magnitude [m/s]
+        alpha0       : initial flow angle [rad]
+        rate         : rate of change for the flow angle [rad/s]
+
+        Example of the boundary condition specification:
+        myPatch
+        {
+            type             varyingFlowDirection;
+            UMag             10;
+            flowDir          x;
+            normalDir        y;
+            alpha0           0;
+            rate             0.1;
+        }
+
+        This will change the flow direction with a rate of 0.1 rad/s starting from 0 rad
+        U[0] = cos(0+0.1*t) 
+        U[1] = sin(0+0.1*t) 
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef varyingFlowDirectionFvPatchVectorFields_H
+#define varyingFlowDirectionFvPatchVectorFields_H
+
+#include "fixedValueFvPatchFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+             Class varyingFlowDirectionFvPatchVectorField Declaration
+\*---------------------------------------------------------------------------*/
+
+class varyingFlowDirectionFvPatchVectorField
+    : public fixedValueFvPatchVectorField
+{
+    // Private data
+
+    scalar UMag_;
+    word flowDir_;
+    word normalDir_;
+    scalar alpha0_;
+    scalar rate_;
+
+public:
+    //- Runtime type information
+    TypeName("varyingFlowDirection");
+
+    // Constructors
+
+    //- Construct from patch and internal field
+    varyingFlowDirectionFvPatchVectorField(
+        const fvPatch&,
+        const DimensionedField<vector, volMesh>&);
+
+    //- Construct from patch, internal field and dictionary
+    varyingFlowDirectionFvPatchVectorField(
+        const fvPatch&,
+        const DimensionedField<vector, volMesh>&,
+        const dictionary&);
+
+    //- Construct by mapping given varyingFlowDirectionFvPatchVectorField onto
+    //  a new patch
+    varyingFlowDirectionFvPatchVectorField(
+        const varyingFlowDirectionFvPatchVectorField&,
+        const fvPatch&,
+        const DimensionedField<vector, volMesh>&,
+        const fvPatchFieldMapper&);
+
+    //- Construct as copy
+    varyingFlowDirectionFvPatchVectorField(
+        const varyingFlowDirectionFvPatchVectorField&);
+
+    //- Construct and return a clone
+    virtual tmp<fvPatchVectorField> clone() const
+    {
+        return tmp<fvPatchVectorField>(
+            new varyingFlowDirectionFvPatchVectorField(*this));
+    }
+
+    //- Construct as copy setting internal field reference
+    varyingFlowDirectionFvPatchVectorField(
+        const varyingFlowDirectionFvPatchVectorField&,
+        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 varyingFlowDirectionFvPatchVectorField(*this, iF));
+    }
+
+    // Member functions
+
+    //- Update the patch field
+    virtual void updateCoeffs();
+
+    //- Write
+    virtual void write(Ostream&) const;
+};
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //