From 0f230ba35b973419788bbe5154bf79457fd8dedd Mon Sep 17 00:00:00 2001
From: Gabriel Barajas <gabriel.barajas@unican.es>
Date: Fri, 2 Jun 2017 09:47:31 +0100
Subject: [PATCH] ENH: Added new Grimshaw and McCowan wave models - initial
commit for integration
---
src/waveModels/Make/files | 2 +
.../derived/Grimshaw/GrimshawWaveModel.C | 282 ++++++++++++
.../derived/Grimshaw/GrimshawWaveModel.H | 154 +++++++
.../derived/McCowan/McCowanWaveModel.C | 408 ++++++++++++++++++
.../derived/McCowan/McCowanWaveModel.H | 170 ++++++++
.../waveExampleSolitaryGrimshaw/0.orig/U | 53 +++
.../0.orig/alpha.water | 52 +++
.../waveExampleSolitaryGrimshaw/0.orig/p_rgh | 60 +++
.../waveExampleSolitaryGrimshaw/Allclean | 10 +
.../waveExampleSolitaryGrimshaw/Allrun | 15 +
.../waveExampleSolitaryGrimshaw/constant/g | 22 +
.../constant/transportProperties | 37 ++
.../constant/turbulenceProperties | 20 +
.../constant/waveProperties | 43 ++
.../system/blockMeshDict | 89 ++++
.../system/controlDict | 143 ++++++
.../system/decomposeParDict | 29 ++
.../system/fvSchemes | 54 +++
.../system/fvSolution | 78 ++++
.../system/setFieldsDict | 37 ++
.../waveExampleSolitaryMcCowan/0.orig/U | 53 +++
.../0.orig/alpha.water | 52 +++
.../waveExampleSolitaryMcCowan/0.orig/p_rgh | 60 +++
.../waveExampleSolitaryMcCowan/Allclean | 10 +
.../laminar/waveExampleSolitaryMcCowan/Allrun | 15 +
.../waveExampleSolitaryMcCowan/constant/g | 22 +
.../constant/transportProperties | 37 ++
.../constant/turbulenceProperties | 20 +
.../constant/waveProperties | 43 ++
.../system/blockMeshDict | 89 ++++
.../system/controlDict | 143 ++++++
.../system/decomposeParDict | 29 ++
.../system/fvSchemes | 54 +++
.../system/fvSolution | 78 ++++
.../system/setFieldsDict | 37 ++
35 files changed, 2500 insertions(+)
create mode 100644 src/waveModels/waveGenerationModels/derived/Grimshaw/GrimshawWaveModel.C
create mode 100644 src/waveModels/waveGenerationModels/derived/Grimshaw/GrimshawWaveModel.H
create mode 100644 src/waveModels/waveGenerationModels/derived/McCowan/McCowanWaveModel.C
create mode 100644 src/waveModels/waveGenerationModels/derived/McCowan/McCowanWaveModel.H
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/U
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/alpha.water
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/p_rgh
create mode 100755 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/Allclean
create mode 100755 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/Allrun
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/g
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/transportProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/turbulenceProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/waveProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/blockMeshDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/controlDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/decomposeParDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/fvSchemes
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/fvSolution
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/setFieldsDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/U
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/alpha.water
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/p_rgh
create mode 100755 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/Allclean
create mode 100755 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/Allrun
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/g
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/transportProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/turbulenceProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/waveProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/blockMeshDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/controlDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/decomposeParDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/fvSchemes
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/fvSolution
create mode 100644 tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/setFieldsDict
diff --git a/src/waveModels/Make/files b/src/waveModels/Make/files
index 67333fa8212..44b6ad45c1a 100644
--- a/src/waveModels/Make/files
+++ b/src/waveModels/Make/files
@@ -6,6 +6,8 @@ waveGenerationModels/base/regularWaveModel/regularWaveModel.C
waveGenerationModels/base/solitaryWaveModel/solitaryWaveModel.C
waveGenerationModels/derived/Boussinesq/BoussinesqWaveModel.C
waveGenerationModels/derived/cnoidal/cnoidalWaveModel.C
+waveGenerationModels/derived/Grimshaw/GrimshawWaveModel.C
+waveGenerationModels/derived/McCowan/McCowanWaveModel.C
waveGenerationModels/derived/StokesII/StokesIIWaveModel.C
waveGenerationModels/derived/StokesI/StokesIWaveModel.C
waveGenerationModels/derived/StokesV/StokesVWaveModel.C
diff --git a/src/waveModels/waveGenerationModels/derived/Grimshaw/GrimshawWaveModel.C b/src/waveModels/waveGenerationModels/derived/Grimshaw/GrimshawWaveModel.C
new file mode 100644
index 00000000000..caaf612c16a
--- /dev/null
+++ b/src/waveModels/waveGenerationModels/derived/Grimshaw/GrimshawWaveModel.C
@@ -0,0 +1,282 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2016 OpenCFD Ltd.
+ \\/ M anipulation | Copyright (C) 2015 IH-Cantabria
+-------------------------------------------------------------------------------
+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 "GrimshawWaveModel.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
+
+namespace Foam
+{
+namespace waveModels
+{
+ defineTypeNameAndDebug(Grimshaw, 0);
+ addToRunTimeSelectionTable
+ (
+ waveModel,
+ Grimshaw,
+ patch
+ );
+}
+}
+
+
+// * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * * //
+
+Foam::scalar Foam::waveModels::Grimshaw::alfa
+(
+ const scalar H,
+ const scalar h
+) const
+{
+ scalar eps = H/h;
+ scalar alfa = sqrt(0.75*eps)*(1.0 - (5.0/8.0)*eps + (71.0/128.0)*eps*eps);
+
+ return alfa;
+}
+
+//- Wave height
+Foam::scalar Foam::waveModels::Grimshaw::eta
+(
+ const scalar H,
+ const scalar h,
+ const scalar x,
+ const scalar y,
+ const scalar theta,
+ const scalar t,
+ const scalar X0
+) const
+{
+ scalar eps = H/h;
+ scalar C = sqrt(mag(g_)*h)*sqrt(1.0+eps-(1.0/20.0)*eps*eps-(3.0/70.0)*eps*eps*eps);
+
+ scalar ts = 3.5*h/sqrt(H/h);
+ scalar xa = -C*t + ts - X0 + x*cos(theta) + y*sin(theta);
+
+ scalar alfa = this->alfa(H, h);
+
+ scalar s = (1.0)/(cosh(alfa*(xa/h)));
+ scalar q = tanh(alfa*(xa/h));
+
+ return h*(eps*s*s - 0.75*eps*eps*s*s*q*q + eps*eps*eps*((5.0/8.0)*s*s*q*q - (101.0/80.0)*s*s*s*s*q*q));
+}
+
+//- Wave velocity
+Foam::vector Foam::waveModels::Grimshaw::U
+(
+ const scalar H,
+ const scalar h,
+ const scalar x,
+ const scalar y,
+ const scalar theta,
+ const scalar t,
+ const scalar X0,
+ const scalar z
+) const
+{
+ scalar eps = H/h;
+ scalar C = sqrt(mag(g_)*h)*sqrt(1.0+eps-(1.0/20.0)*eps*eps-(3.0/70.0)*eps*eps*eps);
+ scalar ts = 3.5*h/sqrt(H/h);
+ scalar xa = -C*t + ts - X0 + x*cos(theta) + y*sin(theta);
+ scalar alfa = this->alfa(H, h);
+
+ scalar s = (1.0)/(cosh(alfa*(xa/h)));
+
+ scalar outa = eps*s*s - eps*eps*(-(1.0/4.0)*s*s + s*s*s*s + ((z/h)*(z/h))*((3.0/2.0)*s*s - (9.0/4.0)*s*s*s*s));
+ scalar outb = (19.0/40.0)*s*s + (1.0/5.0)*s*s*s*s - (6.0/5.0)*s*s*s*s*s*s;
+ scalar outc = ((z/h)*(z/h)) * ( -(3.0/2.0)*s*s - (15.0/4.0)*s*s*s*s + (15.0/2.0)*s*s*s*s*s*s);
+ scalar outd = ((z/h)*(z/h)*(z/h)*(z/h)) * ((-3.0/8.0)*s*s + (45.0/16.0)*s*s*s*s - (45.0/16.0)*s*s*s*s*s*s);
+
+ scalar u = sqrt(mag(g_)*h)*(outa - eps*eps*eps*(outb+outc+outd));
+
+ outa = eps*s*s - eps*eps*((3.0/8.0)*s*s + 2.0*s*s*s*s + ((z/h)*(z/h))*(0.5*s*s - (3.0/2.0)*s*s*s*s));
+ outb = (49.0/640.0)*s*s - (17.0/20.0)*s*s*s*s - (18.0/5.0)*s*s*s*s*s*s;
+ outc = ((z/h)*(z/h)) * ((-13.0/16.0)*s*s -(25.0/16.0)*s*s*s*s + (15.0/2.0)*s*s*s*s*s*s);
+ outd = ((z/h)*(z/h)*(z/h)*(z/h)) * ((-3.0/40.0)*s*s -(9.0/8.0)*s*s*s*s - (27.0/16.0)*s*s*s*s*s*s);
+
+ scalar w = sqrt(mag(g_)*h)*(outa - eps*eps*eps*(outb+outc+outd));
+
+ scalar v = u*sin(waveAngle_);
+ u *= cos(waveAngle_);
+
+ return vector(u, v, w);
+}
+
+void Foam::waveModels::Grimshaw::setLevel
+(
+ const scalar t,
+ const scalar tCoeff,
+ scalarField& level
+) const
+{
+ forAll(level, paddlei)
+ {
+ const scalar eta =
+ this->eta
+ (
+ waveHeight_,
+ waterDepthRef_,
+ xPaddle_[paddlei],
+ yPaddle_[paddlei],
+ waveAngle_,
+ t,
+ x0_
+ );
+
+ level[paddlei] = waterDepthRef_ + tCoeff*eta;
+ }
+}
+
+
+// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
+
+Foam::waveModels::Grimshaw::Grimshaw
+(
+ const dictionary& dict,
+ const fvMesh& mesh,
+ const polyPatch& patch,
+ const bool readFields
+)
+:
+ solitaryWaveModel(dict, mesh, patch, false)
+{
+ if (readFields)
+ {
+ read(dict);
+ }
+}
+
+
+// * * * * * * * * * * * * * * * * Destructor * * * * * * * * * * * * * * * //
+
+Foam::waveModels::Grimshaw::~Grimshaw()
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
+
+bool Foam::waveModels::Grimshaw::read(const dictionary& overrideDict)
+{
+ if (solitaryWaveModel::read(overrideDict))
+ {
+ return true;
+ }
+
+ return false;
+}
+
+void Foam::waveModels::Grimshaw::setVelocity
+(
+ const scalar t,
+ const scalar tCoeff,
+ const scalarField& level,
+ const scalar tg
+)
+{
+ forAll(U_, facei)
+ {
+ // Fraction of geometry represented by paddle - to be set
+ scalar fraction = 1;
+
+ // Height - to be set
+ scalar z = 0;
+
+ setPaddlePropeties(level, facei, fraction, z);
+
+ if (fraction > 0)
+ {
+
+ if ( (tg<0) || (t >= tg) )
+ {
+ const label paddlei = faceToPaddle_[facei];
+
+ const vector Uf = U
+ (
+ waveHeight_,
+ waterDepthRef_,
+ xPaddle_[paddlei],
+ yPaddle_[paddlei],
+ waveAngle_,
+ t,
+ x0_,
+ z
+ );
+
+ U_[facei] = fraction*Uf*tCoeff + fraction*UCurrent_;
+
+ }
+ else if ( tg>=t )
+ {
+ U_[facei] = fraction*UCurrent_;
+ }
+ }
+ }
+}
+
+void Foam::waveModels::Grimshaw::setVelocityAbsorption
+(
+ const scalarField& calculatedLevel,
+ const scalarField& activeLevel
+)
+{
+
+ forAll(U_, facei)
+ {
+ const label paddlei = faceToPaddle_[facei];
+
+ scalar activeLevelMBL=activeLevel[paddlei];
+
+ scalar zMin = zMin_[facei];
+
+//------ not needed anymore in new release
+ if (fabs(zMinGb_)>1.0e-3)
+ {
+ zMin = zMin - zMinGb_;
+ }
+//------
+
+ if (zMin < activeLevelMBL)
+
+ {
+ scalar UCorr =
+ (calculatedLevel[paddlei] - activeLevel[paddlei])
+ *sqrt(mag(g_)/activeLevel[paddlei]);
+
+ U_[facei].x() += UCorr;
+ }
+ else
+ {
+ U_[facei].x() = 0;
+ }
+ }
+}
+
+void Foam::waveModels::Grimshaw::info(Ostream& os) const
+{
+ solitaryWaveModel::info(os);
+}
+
+
+// ************************************************************************* //
diff --git a/src/waveModels/waveGenerationModels/derived/Grimshaw/GrimshawWaveModel.H b/src/waveModels/waveGenerationModels/derived/Grimshaw/GrimshawWaveModel.H
new file mode 100644
index 00000000000..cca90683d09
--- /dev/null
+++ b/src/waveModels/waveGenerationModels/derived/Grimshaw/GrimshawWaveModel.H
@@ -0,0 +1,154 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2016 OpenCFD Ltd.
+ \\/ M anipulation | Copyright (C) 2015 IH-Cantabria
+-------------------------------------------------------------------------------
+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::waveModels::Grimshaw
+
+Description
+ Grimshaw wave model
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef waveModels_Grimshaw_H
+#define waveModels_Grimshaw_H
+
+#include "solitaryWaveModel.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+namespace waveModels
+{
+
+/*---------------------------------------------------------------------------*\
+ Class Grimshaw Declaration
+\*---------------------------------------------------------------------------*/
+
+class Grimshaw
+:
+ public solitaryWaveModel
+{
+protected:
+
+ // Protected Member Functions
+
+ //- Wave height
+ virtual scalar eta
+ (
+ const scalar H,
+ const scalar h,
+ const scalar x,
+ const scalar y,
+ const scalar theta,
+ const scalar t,
+ const scalar X0
+ ) const;
+
+ //-
+ virtual scalar alfa
+ (
+ const scalar H,
+ const scalar h
+ ) const;
+
+ //- Wave velocity
+ virtual vector U
+ (
+ const scalar H,
+ const scalar h,
+ const scalar x,
+ const scalar y,
+ const scalar theta,
+ const scalar t,
+ const scalar X0,
+ const scalar z
+ ) const;
+
+ //- Set the water level
+ virtual void setLevel
+ (
+ const scalar t,
+ const scalar tCoeff,
+ scalarField& level
+ ) const;
+
+ //- Calculate the wave model velocity
+ virtual void setVelocity
+ (
+ const scalar t,
+ const scalar tCoeff,
+ const scalarField& level,
+ const scalar tg
+ );
+
+ // Add current absorption to velocity
+ virtual void setCurrent
+ (
+ const scalarField& levelMBO
+ );
+
+ //- Calculate the wave model velocity absorption
+ virtual void setVelocityAbsorption
+ (
+ const scalarField& calculatedLevel,
+ const scalarField& activeLevel
+ );
+
+public:
+
+ //- Runtime type information
+ TypeName("Grimshaw");
+
+ //- Constructor
+ Grimshaw
+ (
+ const dictionary& dict,
+ const fvMesh& mesh,
+ const polyPatch& patch,
+ const bool readFields = true
+ );
+
+ //- Destructor
+ virtual ~Grimshaw();
+
+
+ // Public Member Functions
+
+ //- Read from dictionary
+ virtual bool read(const dictionary& overrideDict);
+
+ //- Info
+ virtual void info(Ostream& os) const;
+};
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace waveModels
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //
diff --git a/src/waveModels/waveGenerationModels/derived/McCowan/McCowanWaveModel.C b/src/waveModels/waveGenerationModels/derived/McCowan/McCowanWaveModel.C
new file mode 100644
index 00000000000..b818d11e44b
--- /dev/null
+++ b/src/waveModels/waveGenerationModels/derived/McCowan/McCowanWaveModel.C
@@ -0,0 +1,408 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2016 OpenCFD Ltd.
+ \\/ M anipulation | Copyright (C) 2015 IH-Cantabria
+-------------------------------------------------------------------------------
+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 "McCowanWaveModel.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
+
+namespace Foam
+{
+namespace waveModels
+{
+ defineTypeNameAndDebug(McCowan, 0);
+ addToRunTimeSelectionTable
+ (
+ waveModel,
+ McCowan,
+ patch
+ );
+}
+}
+
+
+// * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * * //
+
+Foam::scalar Foam::waveModels::McCowan::eta
+(
+ const scalar H,
+ const scalar h,
+ const scalar x,
+ const scalar y,
+ const scalar theta,
+ const scalar t,
+ const scalar X0
+) const
+{
+ vector vec = this->mn(H,h);
+ scalar mm = vec[0];
+ scalar nn = vec[1];
+
+ scalar C = sqrt(((mag(g_)*h)/mm)*tan(mm));
+ scalar ts = 3.5*h/sqrt(H/h);
+ scalar Xa = -C*t + ts - X0 + x*cos(theta) + y*sin(theta);
+
+ scalar xin = 0.5*H;
+ scalar etas = newtonRapsonF2(xin,H,h,Xa,mm,nn);
+ return etas;
+}
+
+Foam::vector Foam::waveModels::McCowan::mn
+(
+ const scalar H,
+ const scalar h
+) const
+{
+ //m
+ scalar xin = 1.0;
+ scalar m = newtonRapsonF1(xin,H,h);
+
+ //n
+ scalar c1=sin(m+(1.0+((2.0*H)/(3.0*h))));
+ scalar n = (2.0/3.0)*pow(c1,2);
+
+ scalar aux=n;
+
+ return vector(m, n, aux);
+}
+
+Foam::scalar Foam::waveModels::McCowan::newtonRapsonF1
+(
+ const scalar x0,
+ const scalar H,
+ const scalar h
+) const
+{
+ scalar N=10000;
+ scalar eps=1.e-5;
+ scalar maxval = 10000.0;
+
+ scalar xn=0;
+ scalar x=0;
+ scalar c1=0;
+ scalar c2=0;
+ scalar c3=0;
+ scalar fx=0;
+ scalar fprime=0;
+ scalar fxn=0;
+ scalar fxx=0;
+
+ //define value for divergence
+ scalar xx=x0;
+ while (N>0)
+ {
+ //f
+ c1=sin(xx+(1.0+((2.0*H)/(3.0*h))));
+ fx = (2.0/3.0)*pow(c1,2) - (xx*H)/(h*tan(0.5*xx*(1.0+(H/h))));
+
+ //fprime
+ c2=1/tan(0.5*xx*(h/H + 1.0));
+ c3=1/sin(0.5*xx*(H/h + 1.0));
+ fprime=(4.0/3.0)*sin((2.0*H)/(3.0*h) + xx + 1.0)*cos((2.0*H)/(3.0*h) + xx + 1.0)-(h*c2)/H - (0.5*h*xx*(H/h + 1.0)*pow(c3,2))/h;
+ xn = xx-fx/fprime;
+
+ c1=sin(xn+(1.0+((2.0*H)/(3.0*h))));
+ fxn = (2.0/3.0)*pow(c1,2) - (xn*H)/(h*tan(0.5*xn*(1.0+(H/h))));
+ if (fabs(fxn)<eps)
+ {
+ x=xn;
+ return x;
+ }
+
+ c1=sin(xx+(1.0+((2.0*H)/(3.0*h))));
+ fxx = (2.0/3.0)*pow(c1,2) - (xx*H)/(h*tan(0.5*xx*(1.0+(H/h))));
+ if (fabs(fxx)>maxval)
+ {
+ FatalIOErrorInFunction(*this)
+ << "fxx > maxval !!!"
+ << exit(FatalIOError);
+ }
+
+ N = N - 1;
+ xx = xn;
+ }
+
+ return x;
+}
+
+Foam::scalar Foam::waveModels::McCowan::newtonRapsonF2
+(
+ const scalar x0,
+ const scalar H,
+ const scalar h,
+ const scalar xa,
+ const scalar m,
+ const scalar n
+) const
+{
+ scalar N=10000;
+ scalar eps=1.e-5;
+ scalar maxval = 10000.0;
+
+ scalar xn=0;
+ scalar x=0;
+ scalar c2=0;
+ scalar c3=0;
+ scalar fx=0;
+ scalar fprime=0;
+ scalar fxn=0;
+ scalar fxx=0;
+
+ //define value for divergence
+ scalar xx=x0;
+ while (N>0)
+ {
+ //f
+ fx = xx-(h*(n/m)*((sin(m*(1.0+(xx/h))))/(cos(m*(1.0+(xx/h)))+cosh(m*(xa/h)))));
+
+ //fprime
+ c2=sin((m*(h + x))/h);
+ c3=cosh((xa*m)/h) + cos((m*(h + x))/h);
+ fprime = 1 - (n*cos((m*(h + x))/h))/(cosh((xa*m)/h) + cos((m*(h + x))/h)) - (n*pow(c2,2))/(pow(c3,2));
+
+ xn = xx-fx/fprime;
+
+ fxn = xn-(h*(n/m)*((sin(m*(1.0+(xn/h))))/(cos(m*(1.0+(xn/h)))+cosh(m*(xa/h)))));
+ if (fabs(fxn)<eps)
+ {
+ x=xn;
+ return x;
+ }
+
+ fxx = xx-(h*(n/m)*((sin(m*(1.0+(xx/h))))/(cos(m*(1.0+(xx/h)))+cosh(m*(xa/h)))));
+ if (fabs(fxx)>maxval)
+ {
+ FatalIOErrorInFunction(*this)
+ << "fxx > maxval !!!"
+ << exit(FatalIOError);
+ }
+
+ N = N - 1;
+ xx = xn;
+ }
+
+ return x;
+}
+
+Foam::vector Foam::waveModels::McCowan::U
+(
+ const scalar H,
+ const scalar h,
+ const scalar x,
+ const scalar y,
+ const scalar theta,
+ const scalar t,
+ const scalar X0,
+ const scalar z
+) const
+{
+ vector vec = this->mn(H,h);
+ scalar mm = vec[0];
+ scalar nn = vec[1];
+
+ scalar C = sqrt(((mag(g_)*h)/mm)*tan(mm));
+ scalar ts = 3.5*h/sqrt(H/h);
+ scalar Xa = -C*t + ts - X0 + x*cos(theta) + y*sin(theta);
+
+ scalar outa = C*nn*(1.0+cos(mm*(z/h))*cosh(mm*(Xa/h)));
+ scalar outb = (cos(mm*(z/h))+cosh(mm*(Xa/h))) * (cos(mm*(z/h))+cosh(mm*(Xa/h)));
+
+ scalar u = outa/outb;
+
+ outa = C*nn*(sin(mm*(z/h))*sinh(mm*(Xa/h)));
+ outb = (cos(mm*(z/h))+cosh(mm*(Xa/h))) * (cos(mm*(z/h))+cosh(mm*(Xa/h)));
+
+ scalar w = outa/outb;
+
+ scalar v = u*sin(waveAngle_);
+ u *= cos(waveAngle_);
+
+ return vector(u, v, w);
+}
+
+
+void Foam::waveModels::McCowan::setLevel
+(
+ const scalar t,
+ const scalar tCoeff,
+ scalarField& level
+) const
+{
+ forAll(level, paddlei)
+ {
+ const scalar eta =
+ this->eta
+ (
+ waveHeight_,
+ waterDepthRef_,
+ xPaddle_[paddlei],
+ yPaddle_[paddlei],
+ waveAngle_,
+ t,
+ x0_
+ );
+
+ level[paddlei] = waterDepthRef_ + tCoeff*eta;
+ }
+}
+
+
+// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
+
+Foam::waveModels::McCowan::McCowan
+(
+ const dictionary& dict,
+ const fvMesh& mesh,
+ const polyPatch& patch,
+ const bool readFields
+)
+:
+ solitaryWaveModel(dict, mesh, patch, false)
+{
+ if (readFields)
+ {
+ read(dict);
+ }
+}
+
+
+// * * * * * * * * * * * * * * * * Destructor * * * * * * * * * * * * * * * //
+
+Foam::waveModels::McCowan::~McCowan()
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
+
+bool Foam::waveModels::McCowan::read(const dictionary& overrideDict)
+{
+ if (solitaryWaveModel::read(overrideDict))
+ {
+ return true;
+ }
+
+ return false;
+}
+
+void Foam::waveModels::McCowan::setVelocity
+(
+ const scalar t,
+ const scalar tCoeff,
+ const scalarField& level,
+ const scalar tg
+)
+{
+ forAll(U_, facei)
+ {
+ // Fraction of geometry represented by paddle - to be set
+ scalar fraction = 1;
+
+ // Height - to be set
+ scalar z = 0;
+
+ setPaddlePropeties(level, facei, fraction, z);
+
+ if (fraction > 0)
+ {
+
+ if ( (tg<0) || (t >= tg) )
+ {
+ const label paddlei = faceToPaddle_[facei];
+
+ const vector Uf = U
+ (
+ waveHeight_,
+ waterDepthRef_,
+ xPaddle_[paddlei],
+ yPaddle_[paddlei],
+ waveAngle_,
+ t,
+ x0_,
+ z
+ );
+
+ U_[facei] = fraction*Uf*tCoeff + fraction*UCurrent_;
+
+ }
+ else if ( tg>=t )
+ {
+ U_[facei] = fraction*UCurrent_;
+ }
+ }
+ }
+}
+
+void Foam::waveModels::McCowan::setVelocityAbsorption
+(
+ const scalarField& calculatedLevel,
+ const scalarField& activeLevel
+)
+{
+
+ forAll(U_, facei)
+ {
+ const label paddlei = faceToPaddle_[facei];
+
+ scalar activeLevelMBL=activeLevel[paddlei];
+
+ scalar zMin = zMin_[facei];
+
+//------ not needed anymore in new release
+ if (fabs(zMinGb_)>1.0e-3)
+ {
+ zMin = zMin - zMinGb_;
+ }
+//------
+
+ if (zMin < activeLevelMBL)
+ {
+ scalar UCorr =
+ (calculatedLevel[paddlei] - activeLevel[paddlei])
+ *sqrt(mag(g_)/activeLevel[paddlei]);
+
+ U_[facei].x() += UCorr;
+ }
+ else
+ {
+ U_[facei].x() = 0;
+ }
+ }
+}
+
+void Foam::waveModels::McCowan::setCurrent
+(
+ const scalarField& levelMBO
+)
+{
+ //No needed for generation
+}
+
+void Foam::waveModels::McCowan::info(Ostream& os) const
+{
+ solitaryWaveModel::info(os);
+}
+
+
+// ************************************************************************* //
diff --git a/src/waveModels/waveGenerationModels/derived/McCowan/McCowanWaveModel.H b/src/waveModels/waveGenerationModels/derived/McCowan/McCowanWaveModel.H
new file mode 100644
index 00000000000..880684b0438
--- /dev/null
+++ b/src/waveModels/waveGenerationModels/derived/McCowan/McCowanWaveModel.H
@@ -0,0 +1,170 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2016 OpenCFD Ltd.
+ \\/ M anipulation | Copyright (C) 2015 IH-Cantabria
+-------------------------------------------------------------------------------
+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::waveModels::McCowan
+
+Description
+ McCowan wave model
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef waveModels_McCowan_H
+#define waveModels_McCowan_H
+
+#include "solitaryWaveModel.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+namespace waveModels
+{
+
+/*---------------------------------------------------------------------------*\
+ Class McCowan Declaration
+\*---------------------------------------------------------------------------*/
+
+class McCowan
+:
+ public solitaryWaveModel
+{
+protected:
+
+ // Protected Member Functions
+
+ //- Wave height
+ virtual scalar eta
+ (
+ const scalar H,
+ const scalar h,
+ const scalar x,
+ const scalar y,
+ const scalar theta,
+ const scalar t,
+ const scalar X0
+ ) const;
+
+ virtual vector mn
+ (
+ const scalar H,
+ const scalar h
+ ) const;
+
+ virtual scalar newtonRapsonF1
+ (
+ const scalar x0,
+ const scalar H,
+ const scalar h
+ ) const;
+
+ virtual scalar newtonRapsonF2
+ (
+ const scalar x0,
+ const scalar H,
+ const scalar h,
+ const scalar xa,
+ const scalar m,
+ const scalar n
+ ) const;
+
+ //- Wave velocity
+ virtual vector U
+ (
+ const scalar H,
+ const scalar h,
+ const scalar x,
+ const scalar y,
+ const scalar theta,
+ const scalar t,
+ const scalar X0,
+ const scalar z
+ ) const;
+
+ //- Set the water level
+ virtual void setLevel
+ (
+ const scalar t,
+ const scalar tCoeff,
+ scalarField& level
+ ) const;
+
+ //- Calculate the wave model velocity
+ virtual void setVelocity
+ (
+ const scalar t,
+ const scalar tCoeff,
+ const scalarField& level,
+ const scalar tg
+ );
+
+ // Add current absorption to velocity
+ virtual void setCurrent
+ (
+ const scalarField& levelMBO
+ );
+
+ //- Calculate the wave model velocity absorption
+ virtual void setVelocityAbsorption
+ (
+ const scalarField& calculatedLevel,
+ const scalarField& activeLevel
+ );
+
+public:
+
+ //- Runtime type information
+ TypeName("McCowan");
+
+ //- Constructor
+ McCowan
+ (
+ const dictionary& dict,
+ const fvMesh& mesh,
+ const polyPatch& patch,
+ const bool readFields = true
+ );
+
+ //- Destructor
+ virtual ~McCowan();
+
+
+ // Public Member Functions
+
+ //- Read from dictionary
+ virtual bool read(const dictionary& overrideDict);
+
+ //- Info
+ virtual void info(Ostream& os) const;
+};
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace waveModels
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/U b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/U
new file mode 100644
index 00000000000..e0c42a3ef50
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/U
@@ -0,0 +1,53 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.7.x |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volVectorField;
+ location "0";
+ object U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -1 0 0 0 0];
+
+internalField uniform (0 0 0);
+
+boundaryField
+{
+ left
+ {
+ type waveVelocity;
+ value uniform (0 0 0);
+ }
+
+ right
+ {
+ type waveVelocity;
+ value uniform (0 0 0);
+ }
+
+ sides
+ {
+ type slip;
+ }
+
+ ground
+ {
+ type noSlip;
+ }
+
+ top
+ {
+ type pressureInletOutletVelocity;
+ value uniform (0 0 0);
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/alpha.water b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/alpha.water
new file mode 100644
index 00000000000..3562fc0b2f8
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/alpha.water
@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.5-dev |
+| \\ / A nd | Web: http://www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object alpha.water;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 0 0 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ left
+ {
+ type waveAlpha;
+ value uniform 0;
+ }
+
+ right
+ {
+ type zeroGradient;
+ }
+
+ ground
+ {
+ type zeroGradient;
+ }
+
+ sides
+ {
+ type zeroGradient;
+ }
+
+ top
+ {
+ type inletOutlet;
+ inletValue uniform 0;
+ value uniform 0;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/p_rgh b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/p_rgh
new file mode 100644
index 00000000000..a19dce973ee
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/0.orig/p_rgh
@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.5-dev |
+| \\ / A nd | Web: http://www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -2 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ left
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ right
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ ground
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ sides
+ {
+ type slip;
+ }
+
+ top
+ {
+ type totalPressure;
+ U U;
+ phi rhoPhi;
+ rho rho;
+ psi none;
+ gamma 1;
+ p0 uniform 0;
+ value uniform 0;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/Allclean b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/Allclean
new file mode 100755
index 00000000000..705f91474c4
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/Allclean
@@ -0,0 +1,10 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+rm -rf 0
+
+cleanCase
+
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/Allrun b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/Allrun
new file mode 100755
index 00000000000..9f0c668029a
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/Allrun
@@ -0,0 +1,15 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+restore0Dir
+
+runApplication blockMesh
+
+runApplication decomposePar
+
+runParallel setFields
+
+runParallel $(getApplication)
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/g b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/g
new file mode 100644
index 00000000000..317bdd50def
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/g
@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.6 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class uniformDimensionedVectorField;
+ location "constant";
+ object g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -2 0 0 0 0];
+value ( 0 0 -9.81 );
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/transportProperties b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/transportProperties
new file mode 100644
index 00000000000..3633e43efb9
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/transportProperties
@@ -0,0 +1,37 @@
+/*---------------------------------------------------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.3 |
+| \\ / A nd | Web: http://www.openfoam.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phases (water air);
+
+water
+{
+ transportModel Newtonian;
+ nu [0 2 -1 0 0 0 0] 1e-06;
+ rho [1 -3 0 0 0 0 0] 1000;
+}
+
+air
+{
+ transportModel Newtonian;
+ nu [0 2 -1 0 0 0 0] 1.48e-05;
+ rho [1 -3 0 0 0 0 0] 1;
+}
+
+sigma [1 0 -2 0 0 0 0] 0.07;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/turbulenceProperties b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/turbulenceProperties
new file mode 100644
index 00000000000..22f11ecab7a
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/turbulenceProperties
@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.6 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType laminar;
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/waveProperties b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/waveProperties
new file mode 100644
index 00000000000..7247a17696e
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/constant/waveProperties
@@ -0,0 +1,43 @@
+/*---------------------------------------------------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: http://www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object wavesProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+left
+{
+ alpha alpha.water;
+
+ waveModel Grimshaw;
+
+ nPaddle 1;
+
+ waveHeight 0.05;
+
+ waveAngle 0.0;
+
+ activeAbsorption no;
+}
+
+right
+{
+ alpha alpha.water;
+
+ waveModel shallowWaterAbsorption;
+
+ nPaddle 1;
+}
+
+// ************************************************************************* //
+
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/blockMeshDict b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/blockMeshDict
new file mode 100644
index 00000000000..f7d292e0231
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/blockMeshDict
@@ -0,0 +1,89 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+ ( 0.0 0.0 0.0)
+ ( 7.0 0.0 0.0)
+ ( 7.0 0.55 0.0)
+ ( 0.0 0.55 0.0)
+ ( 0.0 0.0 0.5)
+ ( 7.0 0.0 0.5)
+ ( 7.0 0.55 0.5)
+ ( 0.0 0.55 0.5)
+
+);
+
+blocks
+(
+ hex (0 1 2 3 4 5 6 7) (350 28 42) simpleGrading (1 1 1)
+);
+edges
+(
+);
+
+boundary
+(
+ left
+ {
+ type patch;
+ faces
+ (
+ (0 4 7 3)
+ );
+ }
+ right
+ {
+ type patch;
+ faces
+ (
+ (1 5 6 2)
+ );
+ }
+ ground
+ {
+ type wall;
+ faces
+ (
+ (0 1 2 3)
+ );
+ }
+ top
+ {
+ type patch;
+ faces
+ (
+ (4 5 6 7)
+ );
+ }
+ sides
+ {
+ type patch;
+ faces
+ (
+ (0 1 5 4)
+ (3 2 6 7)
+ );
+ }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/controlDict b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/controlDict
new file mode 100644
index 00000000000..5e5bd614380
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/controlDict
@@ -0,0 +1,143 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application interFoam;
+
+startFrom latestTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 7.0;
+
+deltaT 0.1;
+
+writeControl adjustableRunTime;
+
+writeInterval 0.1;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 6;
+
+writeCompression uncompressed;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable yes;
+
+adjustTimeStep on;
+
+maxCo 0.4;
+maxAlphaCo 0.4;
+
+maxDeltaT 0.01;
+
+functions
+{
+ //Sensores VOF
+ line
+ {
+ type sets;
+ functionObjectLibs ("libsampling.so");
+ enabled true;
+ outputControl writeTime;
+ outputInterval 1;
+
+ interpolationScheme cellPoint;
+ setFormat raw;
+ sets
+ (
+ s1
+ {
+
+ type uniform;
+ axis distance;
+ start ( 0.865 0.275 0.0 );
+ end ( 0.865 0.275 0.5 );
+ nPoints 101;
+ }
+ s2
+ {
+
+ type uniform;
+ axis distance;
+ start ( 1.065 0.275 0.0 );
+ end ( 1.065 0.275 0.5 );
+ nPoints 101;
+ }
+ s3
+ {
+
+ type uniform;
+ axis distance;
+ start ( 4.1 0.275 0.0 );
+ end ( 4.1 0.275 0.5 );
+ nPoints 101;
+ }
+ s4
+ {
+
+ type uniform;
+ axis distance;
+ start ( 4.645 0.275 0.0 );
+ end ( 4.645 0.275 0.5 );
+ nPoints 101;
+ }
+ s5
+ {
+
+ type uniform;
+ axis distance;
+ start ( 5.2 0.275 0.0 );
+ end ( 5.2 0.275 0.5 );
+ nPoints 101;
+ }
+ s6
+ {
+
+ type uniform;
+ axis distance;
+ start ( 5.85 0.275 0.0 );
+ end ( 5.85 0.275 0.5 );
+ nPoints 101;
+ }
+ s7
+ {
+
+ type uniform;
+ axis distance;
+ start ( 6.15 0.275 0.0 );
+ end ( 6.15 0.275 0.5 );
+ nPoints 101;
+ }
+ );
+ fixedLocations false;
+ fields
+ (
+ alpha.water
+ );
+ }
+
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/decomposeParDict b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/decomposeParDict
new file mode 100644
index 00000000000..a4e660116ce
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/decomposeParDict
@@ -0,0 +1,29 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 2;
+
+method hierarchical;
+
+hierarchicalCoeffs
+{
+ n (2 1 1);
+ delta 0.001;
+ order xyz;
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/fvSchemes b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/fvSchemes
new file mode 100644
index 00000000000..eeff89271fb
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/fvSchemes
@@ -0,0 +1,54 @@
+
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default Euler;
+}
+
+gradSchemes
+{
+ default Gauss linear;
+}
+
+divSchemes
+{
+ div(rhoPhi,U) Gauss linearUpwind grad(U);
+ div(phi,alpha) Gauss vanLeer;
+ div(phirb,alpha) Gauss linear;
+ div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear orthogonal;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default orthogonal;
+}
+
+
+// ************************************************************************* //
+
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/fvSolution b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/fvSolution
new file mode 100644
index 00000000000..859308b6fab
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/fvSolution
@@ -0,0 +1,78 @@
+
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ "alpha.water.*"
+ {
+ nAlphaCorr 1;
+ nAlphaSubCycles 3;
+ cAlpha 1;
+ }
+
+ pcorr
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-6;
+ relTol 0;
+ }
+
+ p_rgh
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-6;
+ relTol 0.1;
+ }
+
+ p_rghFinal
+ {
+ solver GAMG;
+ smoother DIC;
+ tolerance 1e-7;
+ relTol 0;
+ }
+
+ U
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-6;
+ relTol 0.1;
+ }
+
+ UFinal
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-6;
+ relTol 0;
+ }
+}
+
+PIMPLE
+{
+ momentumPredictor no;
+ nCorrectors 2;
+ nNonOrthogonalCorrectors 0;
+}
+
+
+// ************************************************************************* //
+
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/setFieldsDict b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/setFieldsDict
new file mode 100644
index 00000000000..5873ea0e3d1
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryGrimshaw/system/setFieldsDict
@@ -0,0 +1,37 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+defaultFieldValues
+(
+ volScalarFieldValue alpha.water 0
+ volVectorFieldValue U (0 0 0)
+);
+
+regions
+(
+ boxToCell
+ {
+ box (-10 -10 -10) (100 100 0.15);
+ fieldValues
+ (
+ volScalarFieldValue alpha.water 1
+ );
+ }
+);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/U b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/U
new file mode 100644
index 00000000000..e0c42a3ef50
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/U
@@ -0,0 +1,53 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.7.x |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volVectorField;
+ location "0";
+ object U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -1 0 0 0 0];
+
+internalField uniform (0 0 0);
+
+boundaryField
+{
+ left
+ {
+ type waveVelocity;
+ value uniform (0 0 0);
+ }
+
+ right
+ {
+ type waveVelocity;
+ value uniform (0 0 0);
+ }
+
+ sides
+ {
+ type slip;
+ }
+
+ ground
+ {
+ type noSlip;
+ }
+
+ top
+ {
+ type pressureInletOutletVelocity;
+ value uniform (0 0 0);
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/alpha.water b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/alpha.water
new file mode 100644
index 00000000000..3562fc0b2f8
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/alpha.water
@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.5-dev |
+| \\ / A nd | Web: http://www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object alpha.water;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 0 0 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ left
+ {
+ type waveAlpha;
+ value uniform 0;
+ }
+
+ right
+ {
+ type zeroGradient;
+ }
+
+ ground
+ {
+ type zeroGradient;
+ }
+
+ sides
+ {
+ type zeroGradient;
+ }
+
+ top
+ {
+ type inletOutlet;
+ inletValue uniform 0;
+ value uniform 0;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/p_rgh b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/p_rgh
new file mode 100644
index 00000000000..a19dce973ee
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/0.orig/p_rgh
@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.5-dev |
+| \\ / A nd | Web: http://www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -2 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ left
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ right
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ ground
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ sides
+ {
+ type slip;
+ }
+
+ top
+ {
+ type totalPressure;
+ U U;
+ phi rhoPhi;
+ rho rho;
+ psi none;
+ gamma 1;
+ p0 uniform 0;
+ value uniform 0;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/Allclean b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/Allclean
new file mode 100755
index 00000000000..705f91474c4
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/Allclean
@@ -0,0 +1,10 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+rm -rf 0
+
+cleanCase
+
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/Allrun b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/Allrun
new file mode 100755
index 00000000000..9f0c668029a
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/Allrun
@@ -0,0 +1,15 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+restore0Dir
+
+runApplication blockMesh
+
+runApplication decomposePar
+
+runParallel setFields
+
+runParallel $(getApplication)
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/g b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/g
new file mode 100644
index 00000000000..317bdd50def
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/g
@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.6 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class uniformDimensionedVectorField;
+ location "constant";
+ object g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -2 0 0 0 0];
+value ( 0 0 -9.81 );
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/transportProperties b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/transportProperties
new file mode 100644
index 00000000000..3633e43efb9
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/transportProperties
@@ -0,0 +1,37 @@
+/*---------------------------------------------------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.3 |
+| \\ / A nd | Web: http://www.openfoam.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phases (water air);
+
+water
+{
+ transportModel Newtonian;
+ nu [0 2 -1 0 0 0 0] 1e-06;
+ rho [1 -3 0 0 0 0 0] 1000;
+}
+
+air
+{
+ transportModel Newtonian;
+ nu [0 2 -1 0 0 0 0] 1.48e-05;
+ rho [1 -3 0 0 0 0 0] 1;
+}
+
+sigma [1 0 -2 0 0 0 0] 0.07;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/turbulenceProperties b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/turbulenceProperties
new file mode 100644
index 00000000000..22f11ecab7a
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/turbulenceProperties
@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.6 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType laminar;
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/waveProperties b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/waveProperties
new file mode 100644
index 00000000000..3ec89ee67e8
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/constant/waveProperties
@@ -0,0 +1,43 @@
+/*---------------------------------------------------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: http://www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object wavesProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+left
+{
+ alpha alpha.water;
+
+ waveModel McCowan;
+
+ nPaddle 1;
+
+ waveHeight 0.05;
+
+ waveAngle 0.0;
+
+ activeAbsorption yes;
+}
+
+right
+{
+ alpha alpha.water;
+
+ waveModel shallowWaterAbsorption;
+
+ nPaddle 1;
+}
+
+// ************************************************************************* //
+
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/blockMeshDict b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/blockMeshDict
new file mode 100644
index 00000000000..f7d292e0231
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/blockMeshDict
@@ -0,0 +1,89 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+ ( 0.0 0.0 0.0)
+ ( 7.0 0.0 0.0)
+ ( 7.0 0.55 0.0)
+ ( 0.0 0.55 0.0)
+ ( 0.0 0.0 0.5)
+ ( 7.0 0.0 0.5)
+ ( 7.0 0.55 0.5)
+ ( 0.0 0.55 0.5)
+
+);
+
+blocks
+(
+ hex (0 1 2 3 4 5 6 7) (350 28 42) simpleGrading (1 1 1)
+);
+edges
+(
+);
+
+boundary
+(
+ left
+ {
+ type patch;
+ faces
+ (
+ (0 4 7 3)
+ );
+ }
+ right
+ {
+ type patch;
+ faces
+ (
+ (1 5 6 2)
+ );
+ }
+ ground
+ {
+ type wall;
+ faces
+ (
+ (0 1 2 3)
+ );
+ }
+ top
+ {
+ type patch;
+ faces
+ (
+ (4 5 6 7)
+ );
+ }
+ sides
+ {
+ type patch;
+ faces
+ (
+ (0 1 5 4)
+ (3 2 6 7)
+ );
+ }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/controlDict b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/controlDict
new file mode 100644
index 00000000000..5e5bd614380
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/controlDict
@@ -0,0 +1,143 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application interFoam;
+
+startFrom latestTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 7.0;
+
+deltaT 0.1;
+
+writeControl adjustableRunTime;
+
+writeInterval 0.1;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 6;
+
+writeCompression uncompressed;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable yes;
+
+adjustTimeStep on;
+
+maxCo 0.4;
+maxAlphaCo 0.4;
+
+maxDeltaT 0.01;
+
+functions
+{
+ //Sensores VOF
+ line
+ {
+ type sets;
+ functionObjectLibs ("libsampling.so");
+ enabled true;
+ outputControl writeTime;
+ outputInterval 1;
+
+ interpolationScheme cellPoint;
+ setFormat raw;
+ sets
+ (
+ s1
+ {
+
+ type uniform;
+ axis distance;
+ start ( 0.865 0.275 0.0 );
+ end ( 0.865 0.275 0.5 );
+ nPoints 101;
+ }
+ s2
+ {
+
+ type uniform;
+ axis distance;
+ start ( 1.065 0.275 0.0 );
+ end ( 1.065 0.275 0.5 );
+ nPoints 101;
+ }
+ s3
+ {
+
+ type uniform;
+ axis distance;
+ start ( 4.1 0.275 0.0 );
+ end ( 4.1 0.275 0.5 );
+ nPoints 101;
+ }
+ s4
+ {
+
+ type uniform;
+ axis distance;
+ start ( 4.645 0.275 0.0 );
+ end ( 4.645 0.275 0.5 );
+ nPoints 101;
+ }
+ s5
+ {
+
+ type uniform;
+ axis distance;
+ start ( 5.2 0.275 0.0 );
+ end ( 5.2 0.275 0.5 );
+ nPoints 101;
+ }
+ s6
+ {
+
+ type uniform;
+ axis distance;
+ start ( 5.85 0.275 0.0 );
+ end ( 5.85 0.275 0.5 );
+ nPoints 101;
+ }
+ s7
+ {
+
+ type uniform;
+ axis distance;
+ start ( 6.15 0.275 0.0 );
+ end ( 6.15 0.275 0.5 );
+ nPoints 101;
+ }
+ );
+ fixedLocations false;
+ fields
+ (
+ alpha.water
+ );
+ }
+
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/decomposeParDict b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/decomposeParDict
new file mode 100644
index 00000000000..a4e660116ce
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/decomposeParDict
@@ -0,0 +1,29 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 2;
+
+method hierarchical;
+
+hierarchicalCoeffs
+{
+ n (2 1 1);
+ delta 0.001;
+ order xyz;
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/fvSchemes b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/fvSchemes
new file mode 100644
index 00000000000..eeff89271fb
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/fvSchemes
@@ -0,0 +1,54 @@
+
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default Euler;
+}
+
+gradSchemes
+{
+ default Gauss linear;
+}
+
+divSchemes
+{
+ div(rhoPhi,U) Gauss linearUpwind grad(U);
+ div(phi,alpha) Gauss vanLeer;
+ div(phirb,alpha) Gauss linear;
+ div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear orthogonal;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default orthogonal;
+}
+
+
+// ************************************************************************* //
+
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/fvSolution b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/fvSolution
new file mode 100644
index 00000000000..859308b6fab
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/fvSolution
@@ -0,0 +1,78 @@
+
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ "alpha.water.*"
+ {
+ nAlphaCorr 1;
+ nAlphaSubCycles 3;
+ cAlpha 1;
+ }
+
+ pcorr
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-6;
+ relTol 0;
+ }
+
+ p_rgh
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-6;
+ relTol 0.1;
+ }
+
+ p_rghFinal
+ {
+ solver GAMG;
+ smoother DIC;
+ tolerance 1e-7;
+ relTol 0;
+ }
+
+ U
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-6;
+ relTol 0.1;
+ }
+
+ UFinal
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-6;
+ relTol 0;
+ }
+}
+
+PIMPLE
+{
+ momentumPredictor no;
+ nCorrectors 2;
+ nNonOrthogonalCorrectors 0;
+}
+
+
+// ************************************************************************* //
+
diff --git a/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/setFieldsDict b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/setFieldsDict
new file mode 100644
index 00000000000..5873ea0e3d1
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveExampleSolitaryMcCowan/system/setFieldsDict
@@ -0,0 +1,37 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+defaultFieldValues
+(
+ volScalarFieldValue alpha.water 0
+ volVectorFieldValue U (0 0 0)
+);
+
+regions
+(
+ boxToCell
+ {
+ box (-10 -10 -10) (100 100 0.15);
+ fieldValues
+ (
+ volScalarFieldValue alpha.water 1
+ );
+ }
+);
+
+
+// ************************************************************************* //
--
GitLab