From 0af97856f15b6d5f07f741a1dc95d4c93c8138e9 Mon Sep 17 00:00:00 2001
From: Andrew Heather <a.heather@opencfd.co.uk>
Date: Tue, 12 Dec 2017 08:51:47 +0000
Subject: [PATCH] ENH: Added new nutUBlendedWallFunction
This forms part of what is termed 'automatic wall treatment' in the
reference:
Menter, F., Carregal Ferreira, J., Esch, T., Konno, B. (2003).
The SST Turbulence Model with Improved Wall Treatment
for Heat Transfer Predictions in Gas Turbines.
Proceedings of the International Gas Turbine Congress 2003 Tokyo
Note
The full 'automatic wall treatment' description also requires use of
the Foam::omegaWallFunction with the \c blended flag set to 'on'
---
.../turbulenceModels/Make/files | 1 +
...utUBlendedWallFunctionFvPatchScalarField.C | 225 ++++++++++++++++++
...utUBlendedWallFunctionFvPatchScalarField.H | 206 ++++++++++++++++
3 files changed, 432 insertions(+)
create mode 100644 src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.C
create mode 100644 src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.H
diff --git a/src/TurbulenceModels/turbulenceModels/Make/files b/src/TurbulenceModels/turbulenceModels/Make/files
index 2123e373e88..315ba24226f 100644
--- a/src/TurbulenceModels/turbulenceModels/Make/files
+++ b/src/TurbulenceModels/turbulenceModels/Make/files
@@ -40,6 +40,7 @@ $(nutWallFunctions)/nutkWallFunction/nutkWallFunctionFvPatchScalarField.C
$(nutWallFunctions)/nutkRoughWallFunction/nutkRoughWallFunctionFvPatchScalarField.C
$(nutWallFunctions)/nutkAtmRoughWallFunction/nutkAtmRoughWallFunctionFvPatchScalarField.C
+$(nutWallFunctions)/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.C
$(nutWallFunctions)/nutUWallFunction/nutUWallFunctionFvPatchScalarField.C
$(nutWallFunctions)/nutUSpaldingWallFunction/nutUSpaldingWallFunctionFvPatchScalarField.C
$(nutWallFunctions)/nutUTabulatedWallFunction/nutUTabulatedWallFunctionFvPatchScalarField.C
diff --git a/src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.C b/src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.C
new file mode 100644
index 00000000000..81f1d10a259
--- /dev/null
+++ b/src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.C
@@ -0,0 +1,225 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2016 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 "nutUBlendedWallFunctionFvPatchScalarField.H"
+#include "turbulenceModel.H"
+#include "fvPatchFieldMapper.H"
+#include "volFields.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * Protected Member Functions * * * * * * * * * * * //
+
+Foam::tmp<Foam::scalarField>
+Foam::nutUBlendedWallFunctionFvPatchScalarField::calcNut() const
+{
+ const label patchi = patch().index();
+
+ const turbulenceModel& turbModel = db().lookupObject<turbulenceModel>
+ (
+ IOobject::groupName
+ (
+ turbulenceModel::propertiesName,
+ internalField().group()
+ )
+ );
+ const fvPatchVectorField& Uw = turbModel.U().boundaryField()[patchi];
+ const scalarField magGradU(mag(Uw.snGrad()));
+ const tmp<scalarField> tnuw = turbModel.nu(patchi);
+ const scalarField& nuw = tnuw();
+
+ return max
+ (
+ scalar(0),
+ sqr(calcUTau(magGradU))/(magGradU + ROOTVSMALL) - nuw
+ );
+}
+
+
+Foam::tmp<Foam::scalarField>
+Foam::nutUBlendedWallFunctionFvPatchScalarField::calcUTau
+(
+ const scalarField& magGradU
+) const
+{
+ const label patchi = patch().index();
+
+ const turbulenceModel& turbModel = db().lookupObject<turbulenceModel>
+ (
+ IOobject::groupName
+ (
+ turbulenceModel::propertiesName,
+ internalField().group()
+ )
+ );
+
+ const scalarField& y = turbModel.y()[patchi];
+
+ const tmp<scalarField> tnuw = turbModel.nu(patchi);
+ const scalarField& nuw = tnuw();
+
+ const vectorField n(patch().nf());
+ const fvPatchVectorField& Uw = turbModel.U().boundaryField()[patchi];
+ vectorField Up(Uw.patchInternalField() - Uw);
+ Up -= n*(n & Up);
+ const scalarField magUp(mag(Up));
+
+ tmp<scalarField> tuTaup(new scalarField(patch().size(), 0.0));
+ scalarField& uTaup = tuTaup.ref();
+
+ const scalarField& nutw = *this;
+
+ forAll(uTaup, facei)
+ {
+ scalar ut = sqrt((nutw[facei] + nuw[facei])*magGradU[facei]);
+ scalar error = GREAT;
+ label iter = 0;
+ while (iter++ < 10 && error > 0.001)
+ {
+ scalar yPlus = y[facei]*ut/nuw[facei];
+ scalar uTauVis = magUp[facei]/yPlus;
+ scalar uTauLog = kappa_*magUp[facei]/log(E_*yPlus);
+
+ scalar utNew = pow(pow(uTauVis, n_) + pow(uTauLog, n_), 1.0/n_);
+ error = mag(ut - utNew)/(ut + ROOTVSMALL);
+ ut = 0.5*(ut + utNew);
+ }
+ uTaup[facei] = ut;
+ }
+
+ return tuTaup;
+}
+
+
+// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
+
+Foam::nutUBlendedWallFunctionFvPatchScalarField::
+nutUBlendedWallFunctionFvPatchScalarField
+(
+ const fvPatch& p,
+ const DimensionedField<scalar, volMesh>& iF
+)
+:
+ nutWallFunctionFvPatchScalarField(p, iF),
+ n_(4)
+{}
+
+
+Foam::nutUBlendedWallFunctionFvPatchScalarField::
+nutUBlendedWallFunctionFvPatchScalarField
+(
+ const nutUBlendedWallFunctionFvPatchScalarField& ptf,
+ const fvPatch& p,
+ const DimensionedField<scalar, volMesh>& iF,
+ const fvPatchFieldMapper& mapper
+)
+:
+ nutWallFunctionFvPatchScalarField(ptf, p, iF, mapper),
+ n_(ptf.n_)
+{}
+
+
+Foam::nutUBlendedWallFunctionFvPatchScalarField::
+nutUBlendedWallFunctionFvPatchScalarField
+(
+ const fvPatch& p,
+ const DimensionedField<scalar, volMesh>& iF,
+ const dictionary& dict
+)
+:
+ nutWallFunctionFvPatchScalarField(p, iF, dict),
+ n_(dict.lookupOrDefault<scalar>("n", 4))
+{}
+
+
+Foam::nutUBlendedWallFunctionFvPatchScalarField::
+nutUBlendedWallFunctionFvPatchScalarField
+(
+ const nutUBlendedWallFunctionFvPatchScalarField& wfpsf
+)
+:
+ nutWallFunctionFvPatchScalarField(wfpsf),
+ n_(wfpsf.n_)
+{}
+
+
+Foam::nutUBlendedWallFunctionFvPatchScalarField::
+nutUBlendedWallFunctionFvPatchScalarField
+(
+ const nutUBlendedWallFunctionFvPatchScalarField& wfpsf,
+ const DimensionedField<scalar, volMesh>& iF
+)
+:
+ nutWallFunctionFvPatchScalarField(wfpsf, iF),
+ n_(wfpsf.n_)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
+
+Foam::tmp<Foam::scalarField>
+Foam::nutUBlendedWallFunctionFvPatchScalarField::yPlus() const
+{
+ const label patchi = patch().index();
+
+ const turbulenceModel& turbModel = db().lookupObject<turbulenceModel>
+ (
+ IOobject::groupName
+ (
+ turbulenceModel::propertiesName,
+ internalField().group()
+ )
+ );
+ const scalarField& y = turbModel.y()[patchi];
+ const tmp<scalarField> tnuw = turbModel.nu(patchi);
+ const scalarField& nuw = tnuw();
+ const fvPatchVectorField& Uw = turbModel.U().boundaryField()[patchi];
+ const scalarField magGradU(mag(Uw.snGrad()));
+
+ return y*calcUTau(magGradU)/nuw;
+}
+
+
+void Foam::nutUBlendedWallFunctionFvPatchScalarField::write(Ostream& os) const
+{
+ fvPatchField<scalar>::write(os);
+ writeLocalEntries(os);
+ writeEntry("value", os);
+ os.writeEntry("n", n_);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+ makePatchTypeField
+ (
+ fvPatchScalarField,
+ nutUBlendedWallFunctionFvPatchScalarField
+ );
+}
+
+
+// ************************************************************************* //
diff --git a/src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.H b/src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.H
new file mode 100644
index 00000000000..67db5bf700a
--- /dev/null
+++ b/src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.H
@@ -0,0 +1,206 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2016-2017 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::nutUBlendedWallFunctionFvPatchScalarField
+
+Group
+ grpWallFunctions
+
+Description
+ This boundary condition provides a turbulent kinematic viscosity condition
+ when using wall functions, based on a blending of laminar sub-layer and
+ log region contributions.
+
+ \f[
+ uTau = (uTau_v^n + uTau_l^n)^(1/n)
+ \f]
+
+ where
+ \vartable
+ uTau | friction velocity
+ uTau_v | friction velocity in the viscous region
+ uTau_l | friction velocity in the log region
+ \endvartable
+
+
+Usage
+
+ Example of the boundary condition specification:
+ \verbatim
+ myPatch
+ {
+ type nutUBlendedWallFunction;
+ }
+ \endverbatim
+
+ Reference:
+ See the section that describes 'automatic wall treatment'
+ \verbatim
+ Menter, F., Carregal Ferreira, J., Esch, T., Konno, B. (2003).
+ The SST Turbulence Model with Improved Wall Treatment
+ for Heat Transfer Predictions in Gas Turbines.
+ Proceedings of the International Gas Turbine Congress 2003 Tokyo
+ \endverbatim
+
+Note
+ The full 'automatic wall treatment' description also requires use of the
+ Foam::omegaWallFunction with the \c blended flag set to 'on'
+
+SeeAlso
+ Foam::nutWallFunctionFvPatchScalarField
+ Foam::omegaWallFunctionFvPatchScalarField
+
+SourceFiles
+ nutUBlendedWallFunctionFvPatchScalarField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef nutUBlendedWallFunctionFvPatchScalarField_H
+#define nutUBlendedWallFunctionFvPatchScalarField_H
+
+#include "nutWallFunctionFvPatchScalarField.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+ Class nutUBlendedWallFunctionFvPatchScalarField Declaration
+\*---------------------------------------------------------------------------*/
+
+class nutUBlendedWallFunctionFvPatchScalarField
+:
+ public nutWallFunctionFvPatchScalarField
+{
+protected:
+
+ // Protected data
+
+ //- Model coefficient; default = 4
+ scalar n_;
+
+
+ // Protected Member Functions
+
+ //- Calculate the turbulence viscosity
+ virtual tmp<scalarField> calcNut() const;
+
+ //- Calculate the friction velocity
+ virtual tmp<scalarField> calcUTau(const scalarField& magGradU) const;
+
+
+public:
+
+ //- Runtime type information
+ TypeName("nutUBlendedWallFunction");
+
+
+ // Constructors
+
+ //- Construct from patch and internal field
+ nutUBlendedWallFunctionFvPatchScalarField
+ (
+ const fvPatch&,
+ const DimensionedField<scalar, volMesh>&
+ );
+
+ //- Construct from patch, internal field and dictionary
+ nutUBlendedWallFunctionFvPatchScalarField
+ (
+ const fvPatch&,
+ const DimensionedField<scalar, volMesh>&,
+ const dictionary&
+ );
+
+ //- Construct by mapping given
+ // nutUBlendedWallFunctionFvPatchScalarField
+ // onto a new patch
+ nutUBlendedWallFunctionFvPatchScalarField
+ (
+ const nutUBlendedWallFunctionFvPatchScalarField&,
+ const fvPatch&,
+ const DimensionedField<scalar, volMesh>&,
+ const fvPatchFieldMapper&
+ );
+
+ //- Construct as copy
+ nutUBlendedWallFunctionFvPatchScalarField
+ (
+ const nutUBlendedWallFunctionFvPatchScalarField&
+ );
+
+ //- Construct and return a clone
+ virtual tmp<fvPatchScalarField> clone() const
+ {
+ return tmp<fvPatchScalarField>
+ (
+ new nutUBlendedWallFunctionFvPatchScalarField(*this)
+ );
+ }
+
+ //- Construct as copy setting internal field reference
+ nutUBlendedWallFunctionFvPatchScalarField
+ (
+ const nutUBlendedWallFunctionFvPatchScalarField&,
+ const DimensionedField<scalar, volMesh>&
+ );
+
+ //- Construct and return a clone setting internal field reference
+ virtual tmp<fvPatchScalarField> clone
+ (
+ const DimensionedField<scalar, volMesh>& iF
+ ) const
+ {
+ return tmp<fvPatchScalarField>
+ (
+ new nutUBlendedWallFunctionFvPatchScalarField(*this, iF)
+ );
+ }
+
+
+ // Member functions
+
+ // Evaluation functions
+
+ //- Calculate and return the yPlus at the boundary
+ virtual tmp<scalarField> yPlus() const;
+
+
+ // I-O
+
+ //- Write
+ virtual void write(Ostream& os) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //
--
GitLab