From 11756a06f744718e5c71683cc5469555cf238dc9 Mon Sep 17 00:00:00 2001
From: Henry <Henry>
Date: Fri, 9 Jan 2015 16:12:58 +0000
Subject: [PATCH] advectionDiffusionPatchDistMethod: Calculation of approximate
distance to nearest patch for all cells and boundary by solving the Eikonal
equation in advection form with diffusion smoothing.
---
src/finiteVolume/Make/files | 1 +
.../Poisson/PoissonPatchDistMethod.H | 6 +-
.../advectionDiffusionPatchDistMethod.C | 171 +++++++++++++++
.../advectionDiffusionPatchDistMethod.H | 206 ++++++++++++++++++
4 files changed, 381 insertions(+), 3 deletions(-)
create mode 100644 src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.C
create mode 100644 src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.H
diff --git a/src/finiteVolume/Make/files b/src/finiteVolume/Make/files
index 99acdd281b9..5543c83aee1 100644
--- a/src/finiteVolume/Make/files
+++ b/src/finiteVolume/Make/files
@@ -45,6 +45,7 @@ $(wallDist)/wallDist/wallDist.C
$(wallDist)/patchDistMethods/patchDistMethod/patchDistMethod.C
$(wallDist)/patchDistMethods/meshWave/meshWavePatchDistMethod.C
$(wallDist)/patchDistMethods/Poisson/PoissonPatchDistMethod.C
+$(wallDist)/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.C
fvMeshMapper = fvMesh/fvMeshMapper
diff --git a/src/finiteVolume/fvMesh/wallDist/patchDistMethods/Poisson/PoissonPatchDistMethod.H b/src/finiteVolume/fvMesh/wallDist/patchDistMethods/Poisson/PoissonPatchDistMethod.H
index b87d2d33b66..1e70b3f140f 100644
--- a/src/finiteVolume/fvMesh/wallDist/patchDistMethods/Poisson/PoissonPatchDistMethod.H
+++ b/src/finiteVolume/fvMesh/wallDist/patchDistMethods/Poisson/PoissonPatchDistMethod.H
@@ -30,15 +30,15 @@ Description
References:
\verbatim
- D.B.Spalding,
+ D.B. Spalding,
"Calculation of turbulent heat transfer in cluttered spaces",
Proc. 10th Int. Heat Transfer Conference, Brighton, UK, (1994).
- E.Fares and W.Schroder,
+ E. Fares and W. Schroder,
"Differential Equation for Approximate Wall Distance",
Int.J.Numer.Meth., 39:743-762, (2002).
- P. G. Tucker,
+ P.G. Tucker,
"Differential equation based wall distance computation for DES and
RANS",
J.Comp.Phys., Vol. 190, Issue 1, 1 st September, pp. 229-248 (2003)
diff --git a/src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.C b/src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.C
new file mode 100644
index 00000000000..caf45bdf4b2
--- /dev/null
+++ b/src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.C
@@ -0,0 +1,171 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2015 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 "advectionDiffusionPatchDistMethod.H"
+#include "surfaceInterpolate.H"
+#include "fvcGrad.H"
+#include "fvcDiv.H"
+#include "fvmDiv.H"
+#include "fvmLaplacian.H"
+#include "fvmSup.H"
+#include "addToRunTimeSelectionTable.H"
+
+#include "fixedValueFvPatchFields.H"
+#include "zeroGradientFvPatchFields.H"
+
+// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
+
+namespace Foam
+{
+namespace patchDistMethods
+{
+ defineTypeNameAndDebug(advectionDiffusion, 0);
+ addToRunTimeSelectionTable(patchDistMethod, advectionDiffusion, dictionary);
+}
+}
+
+// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
+
+Foam::patchDistMethods::advectionDiffusion::advectionDiffusion
+(
+ const dictionary& dict,
+ const fvMesh& mesh,
+ const labelHashSet& patchIDs
+)
+:
+ patchDistMethod(mesh, patchIDs),
+ coeffs_(dict.subDict(type() + "Coeffs")),
+ pdmPredictor_
+ (
+ patchDistMethod::New
+ (
+ coeffs_,
+ mesh,
+ patchIDs
+ )
+ ),
+ epsilon_(coeffs_.lookupOrDefault<scalar>("epsilon", 0.1)),
+ maxIter_(coeffs_.lookupOrDefault<int>("maxIter", 10)),
+ tolerance_(coeffs_.lookupOrDefault<scalar>("tolerance", 1e-3))
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
+
+bool Foam::patchDistMethods::advectionDiffusion::correct(volScalarField& y)
+{
+ return correct(y, const_cast<volVectorField&>(volVectorField::null()));
+}
+
+namespace Foam
+{
+template<class Type>
+wordList patchTypes
+(
+ const fvMesh& mesh,
+ const labelHashSet& patchIDs
+)
+{
+ wordList yTypes
+ (
+ mesh.boundary().size(),
+ zeroGradientFvPatchField<Type>::typeName
+ );
+
+ forAllConstIter(labelHashSet, patchIDs, iter)
+ {
+ yTypes[iter.key()] = fixedValueFvPatchField<Type>::typeName;
+ }
+
+ return yTypes;
+}
+}
+
+
+bool Foam::patchDistMethods::advectionDiffusion::correct
+(
+ volScalarField& y,
+ volVectorField& n
+)
+{
+ pdmPredictor_->correct(y);
+
+ int iter = 0;
+ scalar initialResidual = 0;
+
+ do
+ {
+ volVectorField ny
+ (
+ IOobject
+ (
+ "ny",
+ mesh_.time().timeName(),
+ mesh_
+ ),
+ mesh_,
+ dimensionedVector("nWall", dimless, vector::zero),
+ patchTypes<vector>(mesh_, patchIDs_)
+ );
+
+ const fvPatchList& patches = mesh_.boundary();
+
+ forAllConstIter(labelHashSet, patchIDs_, iter)
+ {
+ label patchi = iter.key();
+ ny.boundaryField()[patchi] == -patches[patchi].nf();
+ }
+
+ ny = fvc::grad(y);
+ ny /= (mag(ny) + SMALL);
+ surfaceVectorField nf(fvc::interpolate(ny));
+ nf /= (mag(nf) + SMALL);
+ surfaceScalarField yPhi("yPhi", mesh_.Sf() & nf);
+
+ fvScalarMatrix yEqn
+ (
+ fvm::div(yPhi, y)
+ - fvm::Sp(fvc::div(yPhi), y)
+ - epsilon_*y*fvm::laplacian(y)
+ ==
+ dimensionedScalar("1", dimless, 1.0)
+ );
+
+ yEqn.relax();
+ initialResidual = yEqn.solve().initialResidual();
+
+ // Only calculate n if the field is defined
+ if (notNull(n))
+ {
+ n = -ny;
+ }
+
+ } while (initialResidual > tolerance_ && ++iter < maxIter_);
+
+ return true;
+}
+
+
+// ************************************************************************* //
diff --git a/src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.H b/src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.H
new file mode 100644
index 00000000000..1b710cb7507
--- /dev/null
+++ b/src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.H
@@ -0,0 +1,206 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2015 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::patchDistMethods::advectionDiffusion
+
+Description
+ Calculation of approximate distance to nearest patch for all cells and
+ boundary by solving the Eikonal equation in advection form with diffusion
+ smoothing.
+
+ References:
+ \verbatim
+ P.G. Tucker, C.L. Rumsey, R.E. Bartels, R.T. Biedron,
+ "Transport equation based wall distance computations aimed at flows
+ with time-dependent geometry",
+ NASA/TM-2003-212680, December 2003.
+ \endverbatim
+
+ Example of the wallDist specification in fvSchemes:
+ \verbatim
+ laplacianSchemes
+ {
+ .
+ .
+ laplacian(yPsi) Gauss linear corrected;
+ laplacian(yWall) Gauss linear corrected;
+ .
+ .
+ }
+
+ wallDist
+ {
+ method advectionDiffusion;
+
+ advectionDiffusionCoeffs
+ {
+ method Poisson;
+ epsilon 0.1;
+ tolerance 1e-3;
+ maxIter 10;
+ }
+ }
+ \endverbatim
+ Also the solver specification for yWall is required in fvSolution, e.g.
+ for simple cases:
+ \verbatim
+ yPsi
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-4;
+ relTol 0;
+ }
+
+ yWall
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-4;
+ relTol 0;
+ }
+
+ or for more complex cases:
+
+ yPsi
+ {
+ solver GAMG;
+ smoother GaussSeidel;
+ cacheAgglomeration true;
+ nCellsInCoarsestLevel 10;
+ agglomerator faceAreaPair;
+ mergeLevels 1;
+ tolerance 1e-4;
+ relTol 0;
+ }
+
+ yWall
+ {
+ solver GAMG;
+ smoother symGaussSeidel;
+ cacheAgglomeration true;
+ nCellsInCoarsestLevel 10;
+ agglomerator faceAreaPair;
+ mergeLevels 1;
+ tolerance 1e-4;
+ relTol 0;
+ }
+ \endverbatim
+
+SeeAlso
+ Foam::patchDistMethod::meshWave
+ Foam::wallDist
+
+SourceFiles
+ advectionDiffusionPatchDistMethod.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef advectionDiffusionPatchDistMethod_H
+#define advectionDiffusionPatchDistMethod_H
+
+#include "patchDistMethod.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+namespace patchDistMethods
+{
+
+/*---------------------------------------------------------------------------*\
+ Class advectionDiffusion Declaration
+\*---------------------------------------------------------------------------*/
+
+class advectionDiffusion
+:
+ public patchDistMethod
+{
+ // Private Member Data
+
+ //- Sub-dictionary of coefficients
+ dictionary coeffs_;
+
+ //- Run-time selected method to predict the distance-to-wall field
+ autoPtr<patchDistMethod> pdmPredictor_;
+
+ //- Diffusion coefficient multiplying y*laplacian(y)
+ scalar epsilon_;
+
+ //- Convergence tolerance for the iterations of the advection-diffusion
+ // equation to correct the distance-to-patch and normal-to-patch fields
+ scalar tolerance_;
+
+ //- Maximum number of iterations of the advection-diffusion equation
+ // to correct the distance-to-patch and normal-to-patch fields
+ int maxIter_;
+
+
+ // Private Member Functions
+
+ //- Disallow default bitwise copy construct
+ advectionDiffusion(const advectionDiffusion&);
+
+ //- Disallow default bitwise assignment
+ void operator=(const advectionDiffusion&);
+
+
+public:
+
+ //- Runtime type information
+ TypeName("advectionDiffusion");
+
+
+ // Constructors
+
+ //- Construct from coefficients dictionary, mesh
+ // and fixed-value patch set
+ advectionDiffusion
+ (
+ const dictionary& dict,
+ const fvMesh& mesh,
+ const labelHashSet& patchIDs
+ );
+
+
+ // Member Functions
+
+ //- Correct the given distance-to-patch field
+ virtual bool correct(volScalarField& y);
+
+ //- Correct the given distance-to-patch and normal-to-patch fields
+ virtual bool correct(volScalarField& y, volVectorField& n);
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace patchDistMethods
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //
--
GitLab