From 8165c462cd7fb184ff0d98d559ac1b8fc23d7d71 Mon Sep 17 00:00:00 2001
From: Henry Weller <http://openfoam.org>
Date: Fri, 23 Feb 2018 12:23:06 +0000
Subject: [PATCH] ENH: freestreamPressure, freestreamVelocity: New blended
boundary conditions for the freestream
These BCs blend between typical inflow and outflow conditions based on the
velocity orientation.
airFoil2D tutorial updated to demonstrate these new BCs.
---
src/finiteVolume/Make/files | 1 +
.../freestream/freestreamFvPatchField.H | 4 +-
.../freestreamPressureFvPatchScalarField.C | 95 ++++-----
.../freestreamPressureFvPatchScalarField.H | 40 ++--
.../freestreamVelocityFvPatchVectorField.C | 136 +++++++++++++
.../freestreamVelocityFvPatchVectorField.H | 184 ++++++++++++++++++
.../incompressible/simpleFoam/airFoil2D/0/U | 8 +-
.../incompressible/simpleFoam/airFoil2D/0/p | 2 +
.../simpleFoam/airFoil2D/system/controlDict | 2 +-
.../simpleFoam/airFoil2D/system/fvSolution | 2 -
10 files changed, 388 insertions(+), 86 deletions(-)
create mode 100644 src/finiteVolume/fields/fvPatchFields/derived/freestreamVelocity/freestreamVelocityFvPatchVectorField.C
create mode 100644 src/finiteVolume/fields/fvPatchFields/derived/freestreamVelocity/freestreamVelocityFvPatchVectorField.H
diff --git a/src/finiteVolume/Make/files b/src/finiteVolume/Make/files
index f64ba15fe81..74dd85ebe42 100644
--- a/src/finiteVolume/Make/files
+++ b/src/finiteVolume/Make/files
@@ -154,6 +154,7 @@ $(derivedFvPatchFields)/flowRateInletVelocity/flowRateInletVelocityFvPatchVector
$(derivedFvPatchFields)/flowRateOutletVelocity/flowRateOutletVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/fluxCorrectedVelocity/fluxCorrectedVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/freestream/freestreamFvPatchFields.C
+$(derivedFvPatchFields)/freestreamVelocity/freestreamVelocityFvPatchVectorField.C
$(derivedFvPatchFields)/freestreamPressure/freestreamPressureFvPatchScalarField.C
$(derivedFvPatchFields)/inletOutlet/inletOutletFvPatchFields.C
$(derivedFvPatchFields)/inletOutletTotalTemperature/inletOutletTotalTemperatureFvPatchScalarField.C
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/freestream/freestreamFvPatchField.H b/src/finiteVolume/fields/fvPatchFields/derived/freestream/freestreamFvPatchField.H
index 258c38ceefd..15757c90cf1 100644
--- a/src/finiteVolume/fields/fvPatchFields/derived/freestream/freestreamFvPatchField.H
+++ b/src/finiteVolume/fields/fvPatchFields/derived/freestream/freestreamFvPatchField.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) 2011-2018 OpenFOAM Foundation
\\/ M anipulation |
-------------------------------------------------------------------------------
License
@@ -45,7 +45,7 @@ Usage
<patchName>
{
type freestream;
- phi phi;
+ freestreamValue uniform (300 0 0);
}
\endverbatim
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/freestreamPressure/freestreamPressureFvPatchScalarField.C b/src/finiteVolume/fields/fvPatchFields/derived/freestreamPressure/freestreamPressureFvPatchScalarField.C
index 1986bc40d68..551b4d55e70 100644
--- a/src/finiteVolume/fields/fvPatchFields/derived/freestreamPressure/freestreamPressureFvPatchScalarField.C
+++ b/src/finiteVolume/fields/fvPatchFields/derived/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) 2011-2018 OpenFOAM Foundation
\\/ M anipulation |
-------------------------------------------------------------------------------
License
@@ -24,10 +24,7 @@ License
\*---------------------------------------------------------------------------*/
#include "freestreamPressureFvPatchScalarField.H"
-#include "freestreamFvPatchFields.H"
-#include "fvPatchFieldMapper.H"
#include "volFields.H"
-#include "surfaceFields.H"
#include "addToRunTimeSelectionTable.H"
// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
@@ -39,10 +36,8 @@ freestreamPressureFvPatchScalarField
const DimensionedField<scalar, volMesh>& iF
)
:
- zeroGradientFvPatchScalarField(p, iF),
- UName_("U"),
- phiName_("phi"),
- rhoName_("rho")
+ mixedFvPatchScalarField(p, iF),
+ UName_("U")
{}
@@ -54,11 +49,26 @@ freestreamPressureFvPatchScalarField
const dictionary& dict
)
:
- zeroGradientFvPatchScalarField(p, iF, dict),
- UName_(dict.lookupOrDefault<word>("U", "U")),
- phiName_(dict.lookupOrDefault<word>("phi", "phi")),
- rhoName_(dict.lookupOrDefault<word>("rho", "rho"))
-{}
+ mixedFvPatchScalarField(p, iF),
+ UName_(dict.lookupOrDefault<word>("U", "U"))
+{
+ freestreamValue() = scalarField("freestreamValue", dict, p.size());
+
+ if (dict.found("value"))
+ {
+ fvPatchScalarField::operator=
+ (
+ scalarField("value", dict, p.size())
+ );
+ }
+ else
+ {
+ fvPatchScalarField::operator=(freestreamValue());
+ }
+
+ refGrad() = Zero;
+ valueFraction() = 0;
+}
Foam::freestreamPressureFvPatchScalarField::
@@ -70,10 +80,8 @@ freestreamPressureFvPatchScalarField
const fvPatchFieldMapper& mapper
)
:
- zeroGradientFvPatchScalarField(ptf, p, iF, mapper),
- UName_(ptf.UName_),
- phiName_(ptf.phiName_),
- rhoName_(ptf.rhoName_)
+ mixedFvPatchScalarField(ptf, p, iF, mapper),
+ UName_(ptf.UName_)
{}
@@ -83,10 +91,8 @@ freestreamPressureFvPatchScalarField
const freestreamPressureFvPatchScalarField& wbppsf
)
:
- zeroGradientFvPatchScalarField(wbppsf),
- UName_(wbppsf.UName_),
- phiName_(wbppsf.phiName_),
- rhoName_(wbppsf.rhoName_)
+ mixedFvPatchScalarField(wbppsf),
+ UName_(wbppsf.UName_)
{}
@@ -97,10 +103,8 @@ freestreamPressureFvPatchScalarField
const DimensionedField<scalar, volMesh>& iF
)
:
- zeroGradientFvPatchScalarField(wbppsf, iF),
- UName_(wbppsf.UName_),
- phiName_(wbppsf.phiName_),
- rhoName_(wbppsf.rhoName_)
+ mixedFvPatchScalarField(wbppsf, iF),
+ UName_(wbppsf.UName_)
{}
@@ -113,43 +117,15 @@ void Foam::freestreamPressureFvPatchScalarField::updateCoeffs()
return;
}
- const freestreamFvPatchVectorField& Up =
- refCast<const freestreamFvPatchVectorField>
+ const Field<vector>& Up =
+ patch().template lookupPatchField<volVectorField, vector>
(
- patch().lookupPatchField<volVectorField, vector>(UName_)
+ UName_
);
- const surfaceScalarField& phi =
- db().lookupObject<surfaceScalarField>(phiName_);
-
- fvsPatchField<scalar>& phip =
- const_cast<fvsPatchField<scalar>&>
- (
- patch().patchField<surfaceScalarField, scalar>(phi)
- );
-
- if (phi.dimensions() == dimVelocity*dimArea)
- {
- phip = patch().Sf() & Up.freestreamValue();
- }
- else if (phi.dimensions() == dimDensity*dimVelocity*dimArea)
- {
- const fvPatchField<scalar>& rhop =
- patch().lookupPatchField<volScalarField, scalar>(rhoName_);
-
- phip = rhop*(patch().Sf() & Up.freestreamValue());
- }
- else
- {
- FatalErrorInFunction
- << "dimensions of phi are not correct"
- << "\n on patch " << this->patch().name()
- << " of field " << this->internalField().name()
- << " in file " << this->internalField().objectPath()
- << exit(FatalError);
- }
+ valueFraction() = 0.5 + 0.5*(Up & patch().nf())/mag(Up);
- zeroGradientFvPatchScalarField::updateCoeffs();
+ mixedFvPatchField<scalar>::updateCoeffs();
}
@@ -157,8 +133,7 @@ void Foam::freestreamPressureFvPatchScalarField::write(Ostream& os) const
{
fvPatchScalarField::write(os);
os.writeEntryIfDifferent<word>("U", "U", UName_);
- os.writeEntryIfDifferent<word>("phi", "phi", phiName_);
- os.writeEntryIfDifferent<word>("rho", "rho", rhoName_);
+ freestreamValue().writeEntry("freestreamValue", os);
writeEntry("value", os);
}
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/freestreamPressure/freestreamPressureFvPatchScalarField.H b/src/finiteVolume/fields/fvPatchFields/derived/freestreamPressure/freestreamPressureFvPatchScalarField.H
index be263b1af2a..8486e42805b 100644
--- a/src/finiteVolume/fields/fvPatchFields/derived/freestreamPressure/freestreamPressureFvPatchScalarField.H
+++ b/src/finiteVolume/fields/fvPatchFields/derived/freestreamPressure/freestreamPressureFvPatchScalarField.H
@@ -29,15 +29,16 @@ Group
Description
This boundary condition provides a free-stream condition for pressure.
- It is a zero-gradient condition that constrains the flux across the patch
- based on the free-stream velocity.
+
+ It is an outlet-inlet condition that uses the velocity orientation to
+ continuously blend between zero gradient for normal inlet and fixed value
+ for normal outlet flow.
Usage
\table
- Property | Description | Required | Default value
- U | velocity field name | no | U
- phi | flux field name | no | phi
- rho | density field name | no | none
+ Property | Description | Required | Default value
+ U | velocity field name | no | U
+ freestreamValue | freestream pressure | yes |
\endtable
Example of the boundary condition specification:
@@ -45,14 +46,15 @@ Usage
<patchName>
{
type freestreamPressure;
+ freestreamValue uniform 1e5;
}
\endverbatim
Note
- This condition is designed to operate with a freestream velocity condition
+ This condition is designed to operate with a freestreamVelocity condition
See also
- Foam::zeroGradientFvPatchField
+ Foam::mixedFvPatchField
Foam::freestreamFvPatchField
SourceFiles
@@ -64,7 +66,7 @@ SourceFiles
#define freestreamPressureFvPatchScalarField_H
#include "fvPatchFields.H"
-#include "zeroGradientFvPatchFields.H"
+#include "mixedFvPatchFields.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
@@ -77,20 +79,13 @@ namespace Foam
class freestreamPressureFvPatchScalarField
:
- public zeroGradientFvPatchScalarField
+ public mixedFvPatchScalarField
{
// Private data
//- Name of the velocity field
word UName_;
- //- Name of the flux transporting the field
- word phiName_;
-
- //- Name of the density field used to normalise the mass flux
- //- if necessary
- word rhoName_;
-
public:
@@ -162,6 +157,17 @@ public:
// Member functions
+ const scalarField& freestreamValue() const
+ {
+ return refValue();
+ }
+
+ scalarField& freestreamValue()
+ {
+ return refValue();
+ }
+
+
// Evaluation functions
//- Update the coefficients associated with the patch field
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/freestreamVelocity/freestreamVelocityFvPatchVectorField.C b/src/finiteVolume/fields/fvPatchFields/derived/freestreamVelocity/freestreamVelocityFvPatchVectorField.C
new file mode 100644
index 00000000000..9990cb0c8e7
--- /dev/null
+++ b/src/finiteVolume/fields/fvPatchFields/derived/freestreamVelocity/freestreamVelocityFvPatchVectorField.C
@@ -0,0 +1,136 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2018 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 "freestreamVelocityFvPatchVectorField.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
+
+Foam::freestreamVelocityFvPatchVectorField::freestreamVelocityFvPatchVectorField
+(
+ const fvPatch& p,
+ const DimensionedField<vector, volMesh>& iF
+)
+:
+ mixedFvPatchVectorField(p, iF)
+{}
+
+
+Foam::freestreamVelocityFvPatchVectorField::freestreamVelocityFvPatchVectorField
+(
+ const fvPatch& p,
+ const DimensionedField<vector, volMesh>& iF,
+ const dictionary& dict
+)
+:
+ mixedFvPatchVectorField(p, iF)
+{
+ freestreamValue() = vectorField("freestreamValue", dict, p.size());
+
+ if (dict.found("value"))
+ {
+ fvPatchVectorField::operator=
+ (
+ vectorField("value", dict, p.size())
+ );
+ }
+ else
+ {
+ fvPatchVectorField::operator=(freestreamValue());
+ }
+
+ refGrad() = Zero;
+ valueFraction() = 1;
+}
+
+
+Foam::freestreamVelocityFvPatchVectorField::freestreamVelocityFvPatchVectorField
+(
+ const freestreamVelocityFvPatchVectorField& ptf,
+ const fvPatch& p,
+ const DimensionedField<vector, volMesh>& iF,
+ const fvPatchFieldMapper& mapper
+)
+:
+ mixedFvPatchVectorField(ptf, p, iF, mapper)
+{}
+
+
+Foam::freestreamVelocityFvPatchVectorField::freestreamVelocityFvPatchVectorField
+(
+ const freestreamVelocityFvPatchVectorField& wbppsf
+)
+:
+ mixedFvPatchVectorField(wbppsf)
+{}
+
+
+Foam::freestreamVelocityFvPatchVectorField::freestreamVelocityFvPatchVectorField
+(
+ const freestreamVelocityFvPatchVectorField& wbppsf,
+ const DimensionedField<vector, volMesh>& iF
+)
+:
+ mixedFvPatchVectorField(wbppsf, iF)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
+
+void Foam::freestreamVelocityFvPatchVectorField::updateCoeffs()
+{
+ if (updated())
+ {
+ return;
+ }
+
+ const Field<vector>& Up = *this;
+
+ valueFraction() = 0.5 - 0.5*(Up & patch().nf())/mag(Up);
+
+ mixedFvPatchField<vector>::updateCoeffs();
+}
+
+
+void Foam::freestreamVelocityFvPatchVectorField::write(Ostream& os) const
+{
+ fvPatchVectorField::write(os);
+ freestreamValue().writeEntry("freestreamValue", os);
+ writeEntry("value", os);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+ makePatchTypeField
+ (
+ fvPatchVectorField,
+ freestreamVelocityFvPatchVectorField
+ );
+}
+
+// ************************************************************************* //
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/freestreamVelocity/freestreamVelocityFvPatchVectorField.H b/src/finiteVolume/fields/fvPatchFields/derived/freestreamVelocity/freestreamVelocityFvPatchVectorField.H
new file mode 100644
index 00000000000..9415256e495
--- /dev/null
+++ b/src/finiteVolume/fields/fvPatchFields/derived/freestreamVelocity/freestreamVelocityFvPatchVectorField.H
@@ -0,0 +1,184 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2018 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::freestreamVelocityFvPatchVectorField
+
+Group
+ grpInletBoundaryConditions grpOutletBoundaryConditions
+
+Description
+ This boundary condition provides a free-stream condition for velocity.
+
+ It is an inlet-outlet condition that uses the velocity orientation to
+ continuously blend between fixed value for normal inlet and zero gradient
+ for normal outlet flow.
+
+Usage
+ \table
+ Property | Description | Required | Default value
+ freestreamValue | freestream velocity | yes |
+ \endtable
+
+ Example of the boundary condition specification:
+ \verbatim
+ <patchName>
+ {
+ type freestreamVelocity;
+ freestreamValue uniform (300 0 0);
+ }
+ \endverbatim
+
+Note
+ This condition is designed to operate with the freestreamPressure condition
+
+See also
+ Foam::mixedFvPatchField
+ Foam::freestreamFvPatchField
+
+SourceFiles
+ freestreamVelocityFvPatchVectorField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef freestreamVelocityFvPatchVectorField_H
+#define freestreamVelocityFvPatchVectorField_H
+
+#include "fvPatchFields.H"
+#include "mixedFvPatchFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+ Class freestreamVelocityFvPatchVectorField Declaration
+\*---------------------------------------------------------------------------*/
+
+class freestreamVelocityFvPatchVectorField
+:
+ public mixedFvPatchVectorField
+{
+
+public:
+
+ //- Runtime type information
+ TypeName("freestreamVelocity");
+
+
+ // Constructors
+
+ //- Construct from patch and internal field
+ freestreamVelocityFvPatchVectorField
+ (
+ const fvPatch&,
+ const DimensionedField<vector, volMesh>&
+ );
+
+ //- Construct from patch, internal field and dictionary
+ freestreamVelocityFvPatchVectorField
+ (
+ const fvPatch&,
+ const DimensionedField<vector, volMesh>&,
+ const dictionary&
+ );
+
+ //- Construct by mapping given freestreamVelocityFvPatchVectorField onto
+ // a new patch
+ freestreamVelocityFvPatchVectorField
+ (
+ const freestreamVelocityFvPatchVectorField&,
+ const fvPatch&,
+ const DimensionedField<vector, volMesh>&,
+ const fvPatchFieldMapper&
+ );
+
+ //- Construct as copy
+ freestreamVelocityFvPatchVectorField
+ (
+ const freestreamVelocityFvPatchVectorField&
+ );
+
+ //- Construct and return a clone
+ virtual tmp<fvPatchVectorField> clone() const
+ {
+ return tmp<fvPatchVectorField>
+ (
+ new freestreamVelocityFvPatchVectorField(*this)
+ );
+ }
+
+ //- Construct as copy setting internal field reference
+ freestreamVelocityFvPatchVectorField
+ (
+ const freestreamVelocityFvPatchVectorField&,
+ 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 freestreamVelocityFvPatchVectorField(*this, iF)
+ );
+ }
+
+
+ // Member functions
+
+ const vectorField& freestreamValue() const
+ {
+ return refValue();
+ }
+
+ vectorField& freestreamValue()
+ {
+ return refValue();
+ }
+
+
+ // Evaluation functions
+
+ //- Update the coefficients associated with the patch field
+ virtual void updateCoeffs();
+
+
+ //- Write
+ virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //
diff --git a/tutorials/incompressible/simpleFoam/airFoil2D/0/U b/tutorials/incompressible/simpleFoam/airFoil2D/0/U
index ba119821d39..5121c5c3517 100644
--- a/tutorials/incompressible/simpleFoam/airFoil2D/0/U
+++ b/tutorials/incompressible/simpleFoam/airFoil2D/0/U
@@ -22,14 +22,14 @@ boundaryField
{
inlet
{
- type freestream;
- freestreamValue uniform (25.75 3.62 0);
+ type freestreamVelocity;
+ freestreamValue $internalField;
}
outlet
{
- type freestream;
- freestreamValue uniform (25.75 3.62 0);
+ type freestreamVelocity;
+ freestreamValue $internalField;
}
walls
diff --git a/tutorials/incompressible/simpleFoam/airFoil2D/0/p b/tutorials/incompressible/simpleFoam/airFoil2D/0/p
index 4494ee33c1f..75c231def0b 100644
--- a/tutorials/incompressible/simpleFoam/airFoil2D/0/p
+++ b/tutorials/incompressible/simpleFoam/airFoil2D/0/p
@@ -23,11 +23,13 @@ boundaryField
inlet
{
type freestreamPressure;
+ freestreamValue $internalField;
}
outlet
{
type freestreamPressure;
+ freestreamValue $internalField;
}
walls
diff --git a/tutorials/incompressible/simpleFoam/airFoil2D/system/controlDict b/tutorials/incompressible/simpleFoam/airFoil2D/system/controlDict
index 3e4f6c5e380..6d0c7a03523 100644
--- a/tutorials/incompressible/simpleFoam/airFoil2D/system/controlDict
+++ b/tutorials/incompressible/simpleFoam/airFoil2D/system/controlDict
@@ -17,7 +17,7 @@ FoamFile
application simpleFoam;
-startFrom latestTime;
+startFrom startTime;
startTime 0;
diff --git a/tutorials/incompressible/simpleFoam/airFoil2D/system/fvSolution b/tutorials/incompressible/simpleFoam/airFoil2D/system/fvSolution
index 1d22f18c896..0dc5cf88e4b 100644
--- a/tutorials/incompressible/simpleFoam/airFoil2D/system/fvSolution
+++ b/tutorials/incompressible/simpleFoam/airFoil2D/system/fvSolution
@@ -47,8 +47,6 @@ solvers
SIMPLE
{
nNonOrthogonalCorrectors 0;
- pRefCell 0;
- pRefValue 0;
residualControl
{
--
GitLab