From 6e1e854cbccba8b22f8721273572e000b7b98638 Mon Sep 17 00:00:00 2001
From: Gabriel Barajas <gabriel.barajas@unican.es>
Date: Thu, 15 Nov 2018 08:29:54 +0000
Subject: [PATCH] INT: Initial commit of new wave-maker BCs based on mesh
motion
waveMakerFlap: creates waves using a flapping motion
waveMakerPiston: creates waves using a piston motion
---
.../waveMakerFlapPointPatchVectorField.C | 250 ++++++++++++++++++
.../waveMakerFlapPointPatchVectorField.H | 179 +++++++++++++
.../waveMakerPistonPointPatchVectorField.C | 238 +++++++++++++++++
.../waveMakerPistonPointPatchVectorField.H | 179 +++++++++++++
.../interFoam/laminar/waveMakerFlap/0.org/U | 59 +++++
.../laminar/waveMakerFlap/0.org/alpha.water | 55 ++++
.../laminar/waveMakerFlap/0.org/p_rgh | 65 +++++
.../waveMakerFlap/0.org/pointDisplacement | 72 +++++
.../waveMakerFlap/constant/dynamicMeshDict | 29 ++
.../laminar/waveMakerFlap/constant/g | 22 ++
.../constant/transportProperties | 37 +++
.../constant/turbulenceProperties | 20 ++
.../waveMakerFlap/constant/waveProperties | 28 ++
.../waveMakerFlap/system/blockMeshDict | 111 ++++++++
.../laminar/waveMakerFlap/system/controlDict | 139 ++++++++++
.../laminar/waveMakerFlap/system/fvSchemes | 64 +++++
.../laminar/waveMakerFlap/system/fvSolution | 98 +++++++
.../waveMakerFlap/system/setFieldsDict | 33 +++
.../interFoam/laminar/waveMakerPiston/0.org/U | 59 +++++
.../laminar/waveMakerPiston/0.org/alpha.water | 55 ++++
.../laminar/waveMakerPiston/0.org/p_rgh | 65 +++++
.../waveMakerPiston/0.org/pointDisplacement | 72 +++++
.../waveMakerPiston/constant/dynamicMeshDict | 29 ++
.../laminar/waveMakerPiston/constant/g | 22 ++
.../constant/transportProperties | 37 +++
.../constant/turbulenceProperties | 20 ++
.../waveMakerPiston/constant/waveProperties | 28 ++
.../waveMakerPiston/system/blockMeshDict | 111 ++++++++
.../waveMakerPiston/system/controlDict | 139 ++++++++++
.../laminar/waveMakerPiston/system/fvSchemes | 64 +++++
.../laminar/waveMakerPiston/system/fvSolution | 97 +++++++
.../waveMakerPiston/system/setFieldsDict | 33 +++
32 files changed, 2509 insertions(+)
create mode 100644 src/waveModels/derivedFvPatchFields/waveMakerFlap/waveMakerFlapPointPatchVectorField.C
create mode 100644 src/waveModels/derivedFvPatchFields/waveMakerFlap/waveMakerFlapPointPatchVectorField.H
create mode 100644 src/waveModels/derivedFvPatchFields/waveMakerPiston/waveMakerPistonPointPatchVectorField.C
create mode 100644 src/waveModels/derivedFvPatchFields/waveMakerPiston/waveMakerPistonPointPatchVectorField.H
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/U
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/alpha.water
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/p_rgh
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/pointDisplacement
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/dynamicMeshDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/g
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/transportProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/turbulenceProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/waveProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/blockMeshDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/controlDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/fvSchemes
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/fvSolution
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/setFieldsDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/U
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/alpha.water
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/p_rgh
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/pointDisplacement
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/dynamicMeshDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/g
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/transportProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/turbulenceProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/waveProperties
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/blockMeshDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/controlDict
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/fvSchemes
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/fvSolution
create mode 100644 tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/setFieldsDict
diff --git a/src/waveModels/derivedFvPatchFields/waveMakerFlap/waveMakerFlapPointPatchVectorField.C b/src/waveModels/derivedFvPatchFields/waveMakerFlap/waveMakerFlapPointPatchVectorField.C
new file mode 100644
index 00000000000..71e1c6806ad
--- /dev/null
+++ b/src/waveModels/derivedFvPatchFields/waveMakerFlap/waveMakerFlapPointPatchVectorField.C
@@ -0,0 +1,250 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2011-2016 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 "waveMakerFlapPointPatchVectorField.H"
+#include "mathematicalConstants.H"
+#include "pointPatchFields.H"
+#include "addToRunTimeSelectionTable.H"
+#include "Time.H"
+#include "polyMesh.H"
+
+// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
+
+Foam::waveMakerFlapPointPatchVectorField::
+waveMakerFlapPointPatchVectorField
+(
+ const pointPatch& p,
+ const DimensionedField<vector, pointMesh>& iF
+)
+:
+ fixedValuePointPatchField<vector>(p, iF),
+ initialDepth_(0.0),
+ wavePeriod_(0.0),
+ waveHeigth_(0.0),
+ waveLength_(0.0),
+ wavePhase_(0.0),
+ waveNumber_(0.0),
+ rampTime_(0.0),
+ g_(Zero),
+ secondOrder_(false)
+{}
+
+
+Foam::waveMakerFlapPointPatchVectorField::
+waveMakerFlapPointPatchVectorField
+(
+ const pointPatch& p,
+ const DimensionedField<vector, pointMesh>& iF,
+ const dictionary& dict
+)
+:
+ fixedValuePointPatchField<vector>(p, iF, dict),
+ initialDepth_(readScalar(dict.lookup("initialDepth"))),
+ wavePeriod_(readScalar(dict.lookup("wavePeriod"))),
+ waveHeigth_(readScalar(dict.lookup("waveHeigth"))),
+ waveLength_(readScalar(dict.lookup("waveLength"))),
+ wavePhase_(readScalar(dict.lookup("wavePhase"))),
+ waveNumber_(readScalar(dict.lookup("waveNumber"))),
+ rampTime_(readScalar(dict.lookup("rampTime"))),
+ g_(dict.lookup("g")),
+ secondOrder_(dict.lookupOrDefault<bool>("secondOrder",false))
+{
+ if (!dict.found("value"))
+ {
+ updateCoeffs();
+ }
+}
+
+
+Foam::waveMakerFlapPointPatchVectorField::
+waveMakerFlapPointPatchVectorField
+(
+ const waveMakerFlapPointPatchVectorField& ptf,
+ const pointPatch& p,
+ const DimensionedField<vector, pointMesh>& iF,
+ const pointPatchFieldMapper& mapper
+)
+:
+ fixedValuePointPatchField<vector>(ptf, p, iF, mapper),
+ initialDepth_(ptf.initialDepth_),
+ wavePeriod_(ptf.wavePeriod_),
+ waveHeigth_(ptf.waveHeigth_),
+ waveLength_(ptf.waveLength_),
+ wavePhase_(ptf.wavePhase_),
+ waveNumber_(ptf.waveNumber_),
+ rampTime_(ptf.rampTime_),
+ g_(ptf.g_),
+ secondOrder_(ptf.secondOrder_)
+{}
+
+
+Foam::waveMakerFlapPointPatchVectorField::
+waveMakerFlapPointPatchVectorField
+(
+ const waveMakerFlapPointPatchVectorField& ptf,
+ const DimensionedField<vector, pointMesh>& iF
+)
+:
+ fixedValuePointPatchField<vector>(ptf, iF),
+ initialDepth_(ptf.initialDepth_),
+ wavePeriod_(ptf.wavePeriod_),
+ waveHeigth_(ptf.waveHeigth_),
+ waveLength_(ptf.waveLength_),
+ wavePhase_(ptf.wavePhase_),
+ waveNumber_(ptf.waveNumber_),
+ rampTime_(ptf.rampTime_),
+ g_(ptf.g_),
+ secondOrder_(ptf.secondOrder_)
+{}
+
+// * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * * //
+
+Foam::scalar Foam::waveMakerFlapPointPatchVectorField::waveLength
+(
+ const scalar h,
+ const scalar T
+)
+{
+ const scalar L0 = mag(g_)*T*T/(constant::mathematical::twoPi);
+ scalar L = L0;
+
+ for(int i=1; i<=100; i++)
+ {
+ L = L0*tanh(constant::mathematical::twoPi*h/L);
+ }
+ return L;
+}
+
+Foam::scalar Foam::waveMakerFlapPointPatchVectorField::timeCoeff
+(
+ const scalar t
+) const
+{
+ return max(0, min(t/rampTime_, 1));
+}
+
+
+// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
+
+void Foam::waveMakerFlapPointPatchVectorField::updateCoeffs()
+{
+ if (this->updated())
+ {
+ return;
+ }
+
+ const polyMesh& mesh = this->internalField().mesh()();
+ const Time& t = mesh.time();
+
+ // Time ramp weight
+ const scalar tCoeff = timeCoeff(t.value());
+
+ vectorField localPoints_ = this->patch().localPoints();
+ vectorField waveBoardMotion_ = 0.0*localPoints_;
+
+ waveLength_ = waveLength (initialDepth_, wavePeriod_);
+
+ const scalar waveK = constant::mathematical::twoPi/waveLength_;
+ const scalar sigma_ = (2.0*constant::mathematical::pi) / wavePeriod_;
+
+ //First order
+ if (secondOrder_== false)
+ {
+ forAll (localPoints_, labelP)
+ {
+ scalar waveBoardStroke_ = (sinh(2.0*waveK*initialDepth_)
+ + 2.0*waveK*initialDepth_)
+ / (4.0*sinh(waveK*initialDepth_))
+ * (1.0 / ( sinh(waveK*initialDepth_)
+ + (1.0-cosh(waveK*initialDepth_))
+ / (waveK*initialDepth_) ) ) * waveHeigth_;
+
+ waveBoardMotion_[labelP].component(0) = tCoeff
+ * (1.0+(localPoints_[labelP].component(2)-initialDepth_)
+ / (initialDepth_))*(waveBoardStroke_/2.0)*sin(sigma_*t.value());
+ }
+
+ Field<vector>::operator=
+ (
+ waveBoardMotion_
+ );
+ }
+ else if ( secondOrder_ == true)
+ {
+ scalar m1_;
+ forAll (localPoints_, labelP)
+ {
+ m1_ = ((4.0*sinh(waveK*initialDepth_))
+ / (sinh(2.0*waveK*initialDepth_)+2.0*waveK*initialDepth_))
+ * ( sinh(waveK*initialDepth_) + 1.0/(waveK*initialDepth_)
+ * (1.0-cosh(waveK*initialDepth_)));
+
+ waveBoardMotion_[labelP].component(0) = waveHeigth_/(2.0*m1_)*sin(sigma_*t.value())
+ + pow(waveHeigth_,2)/(16.0*initialDepth_)*(3.0*cosh(waveK*initialDepth_)
+ / pow(sinh(waveK*initialDepth_),3) -2.0/m1_)*sin(2.0*sigma_*t.value());
+
+ waveBoardMotion_[labelP].component(0) = tCoeff
+ * (1.0+(localPoints_[labelP].component(2)-initialDepth_)
+ / (initialDepth_)) * waveBoardMotion_[labelP].component(0);
+ }
+
+ Field<vector>::operator=
+ (
+ waveBoardMotion_
+ );
+ }
+
+ fixedValuePointPatchField<vector>::updateCoeffs();
+}
+
+
+void Foam::waveMakerFlapPointPatchVectorField::write(Ostream& os) const
+{
+ pointPatchField<vector>::write(os);
+ os.writeEntry("initialDepth", initialDepth_);
+ os.writeEntry("wavePeriod", wavePeriod_);
+ os.writeEntry("waveHeigth", waveHeigth_);
+ os.writeEntry("waveLength", waveLength_);
+ os.writeEntry("wavePhase", wavePhase_);
+ os.writeEntry("waveNumber", waveNumber_);
+ os.writeEntry("rampTime", rampTime_);
+ os.writeEntry("g", g_);
+ os.writeEntry("secondOrder", secondOrder_);
+ writeEntry("value", os);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+ makePointPatchTypeField
+ (
+ pointPatchVectorField,
+ waveMakerFlapPointPatchVectorField
+ );
+}
+
+// ************************************************************************* //
diff --git a/src/waveModels/derivedFvPatchFields/waveMakerFlap/waveMakerFlapPointPatchVectorField.H b/src/waveModels/derivedFvPatchFields/waveMakerFlap/waveMakerFlapPointPatchVectorField.H
new file mode 100644
index 00000000000..689048d10ac
--- /dev/null
+++ b/src/waveModels/derivedFvPatchFields/waveMakerFlap/waveMakerFlapPointPatchVectorField.H
@@ -0,0 +1,179 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2011-2016 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::waveMakerFlapPointPatchVectorField
+
+Description
+ Foam::waveMakerFlapPointPatchVectorField
+
+SourceFiles
+ waveMakerFlapPointPatchVectorField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef waveMakerFlapPointPatchVectorField_H
+#define waveMakerFlapPointPatchVectorField_H
+
+#include "fixedValuePointPatchField.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+ Class waveMakerFlapPointPatchVectorField Declaration
+\*---------------------------------------------------------------------------*/
+
+class waveMakerFlapPointPatchVectorField
+:
+ public fixedValuePointPatchField<vector>
+{
+ // Private data
+
+ //inital water depth
+ scalar initialDepth_;
+
+ //wave period
+ scalar wavePeriod_;
+
+ //wave heigth
+ scalar waveHeigth_;
+
+ //wavelength
+ scalar waveLength_;
+
+ //wave phase
+ scalar wavePhase_;
+
+ //wave number
+ scalar waveNumber_;
+
+ //ramp time
+ scalar rampTime_;
+
+ // gravity vector
+ vector g_;
+
+ //on/off second order generation
+ scalar secondOrder_;
+
+ // Protected Member Functions
+
+ // Dispersion equation
+ virtual scalar waveLength(const scalar h, const scalar T);
+
+ //- Return the time scaling coefficient
+ virtual scalar timeCoeff(const scalar t) const;
+
+public:
+
+ //- Runtime type information
+ TypeName("waveMakerFlap");
+
+
+ // Constructors
+
+ //- Construct from patch and internal field
+ waveMakerFlapPointPatchVectorField
+ (
+ const pointPatch&,
+ const DimensionedField<vector, pointMesh>&
+ );
+
+ //- Construct from patch, internal field and dictionary
+ waveMakerFlapPointPatchVectorField
+ (
+ const pointPatch&,
+ const DimensionedField<vector, pointMesh>&,
+ const dictionary&
+ );
+
+ //- Construct by mapping given patchField<vector> onto a new patch
+ waveMakerFlapPointPatchVectorField
+ (
+ const waveMakerFlapPointPatchVectorField&,
+ const pointPatch&,
+ const DimensionedField<vector, pointMesh>&,
+ const pointPatchFieldMapper&
+ );
+
+ //- Construct and return a clone
+ virtual autoPtr<pointPatchField<vector>> clone() const
+ {
+ return autoPtr<pointPatchField<vector>>
+ (
+ new waveMakerFlapPointPatchVectorField
+ (
+ *this
+ )
+ );
+ }
+
+ //- Construct as copy setting internal field reference
+ waveMakerFlapPointPatchVectorField
+ (
+ const waveMakerFlapPointPatchVectorField&,
+ const DimensionedField<vector, pointMesh>&
+ );
+
+ //- Construct and return a clone setting internal field reference
+ virtual autoPtr<pointPatchField<vector>> clone
+ (
+ const DimensionedField<vector, pointMesh>& iF
+ ) const
+ {
+ return autoPtr<pointPatchField<vector>>
+ (
+ new waveMakerFlapPointPatchVectorField
+ (
+ *this,
+ iF
+ )
+ );
+ }
+
+
+ // Member functions
+
+ // Evaluation functions
+
+ //- Update the coefficients associated with the patch field
+ virtual void updateCoeffs();
+
+
+ //- Write
+ virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //
diff --git a/src/waveModels/derivedFvPatchFields/waveMakerPiston/waveMakerPistonPointPatchVectorField.C b/src/waveModels/derivedFvPatchFields/waveMakerPiston/waveMakerPistonPointPatchVectorField.C
new file mode 100644
index 00000000000..7eb2346fe4e
--- /dev/null
+++ b/src/waveModels/derivedFvPatchFields/waveMakerPiston/waveMakerPistonPointPatchVectorField.C
@@ -0,0 +1,238 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2011-2016 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 "waveMakerPistonPointPatchVectorField.H"
+#include "mathematicalConstants.H"
+#include "pointPatchFields.H"
+#include "addToRunTimeSelectionTable.H"
+#include "Time.H"
+#include "polyMesh.H"
+
+// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
+
+Foam::waveMakerPistonPointPatchVectorField::
+waveMakerPistonPointPatchVectorField
+(
+ const pointPatch& p,
+ const DimensionedField<vector, pointMesh>& iF
+)
+:
+ fixedValuePointPatchField<vector>(p, iF),
+ initialDepth_(0.0),
+ wavePeriod_(0.0),
+ waveHeigth_(0.0),
+ waveLength_(0.0),
+ wavePhase_(0.0),
+ waveNumber_(0.0),
+ rampTime_(0.0),
+ g_(Zero),
+ secondOrder_(false)
+{}
+
+
+Foam::waveMakerPistonPointPatchVectorField::
+waveMakerPistonPointPatchVectorField
+(
+ const pointPatch& p,
+ const DimensionedField<vector, pointMesh>& iF,
+ const dictionary& dict
+)
+:
+ fixedValuePointPatchField<vector>(p, iF, dict),
+ initialDepth_(readScalar(dict.lookup("initialDepth"))),
+ wavePeriod_(readScalar(dict.lookup("wavePeriod"))),
+ waveHeigth_(readScalar(dict.lookup("waveHeigth"))),
+ waveLength_(readScalar(dict.lookup("waveLength"))),
+ wavePhase_(readScalar(dict.lookup("wavePhase"))),
+ waveNumber_(readScalar(dict.lookup("waveNumber"))),
+ rampTime_(readScalar(dict.lookup("rampTime"))),
+ g_(dict.lookup("g")),
+ secondOrder_(dict.lookupOrDefault<bool>("secondOrder",false))
+{
+ if (!dict.found("value"))
+ {
+ updateCoeffs();
+ }
+}
+
+
+Foam::waveMakerPistonPointPatchVectorField::
+waveMakerPistonPointPatchVectorField
+(
+ const waveMakerPistonPointPatchVectorField& ptf,
+ const pointPatch& p,
+ const DimensionedField<vector, pointMesh>& iF,
+ const pointPatchFieldMapper& mapper
+)
+:
+ fixedValuePointPatchField<vector>(ptf, p, iF, mapper),
+ initialDepth_(ptf.initialDepth_),
+ wavePeriod_(ptf.wavePeriod_),
+ waveHeigth_(ptf.waveHeigth_),
+ waveLength_(ptf.waveLength_),
+ wavePhase_(ptf.wavePhase_),
+ waveNumber_(ptf.waveNumber_),
+ rampTime_(ptf.rampTime_),
+ g_(ptf.g_),
+ secondOrder_(ptf.secondOrder_)
+{}
+
+
+Foam::waveMakerPistonPointPatchVectorField::
+waveMakerPistonPointPatchVectorField
+(
+ const waveMakerPistonPointPatchVectorField& ptf,
+ const DimensionedField<vector, pointMesh>& iF
+)
+:
+ fixedValuePointPatchField<vector>(ptf, iF),
+ initialDepth_(ptf.initialDepth_),
+ wavePeriod_(ptf.wavePeriod_),
+ waveHeigth_(ptf.waveHeigth_),
+ waveLength_(ptf.waveLength_),
+ wavePhase_(ptf.wavePhase_),
+ waveNumber_(ptf.waveNumber_),
+ rampTime_(ptf.rampTime_),
+ g_(ptf.g_),
+ secondOrder_(ptf.secondOrder_)
+{}
+
+// * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * * //
+
+Foam::scalar Foam::waveMakerPistonPointPatchVectorField::waveLength
+(
+ const scalar h,
+ const scalar T
+)
+{
+ const scalar L0 = mag(g_)*T*T/(constant::mathematical::twoPi);
+ scalar L = L0;
+
+ for(int i=1; i<=100; i++)
+ {
+ L = L0*tanh(constant::mathematical::twoPi*h/L);
+ }
+ return L;
+}
+
+Foam::scalar Foam::waveMakerPistonPointPatchVectorField::timeCoeff
+(
+ const scalar t
+) const
+{
+ return max(0, min(t/rampTime_, 1));
+}
+
+
+// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
+
+void Foam::waveMakerPistonPointPatchVectorField::updateCoeffs()
+{
+ if (this->updated())
+ {
+ return;
+ }
+
+ const polyMesh& mesh = this->internalField().mesh()();
+ const Time& t = mesh.time();
+
+ // Time ramp weight
+ const scalar tCoeff = timeCoeff(t.value());
+
+ vectorField localPoints_ = this->patch().localPoints();
+ vectorField auxPoints = 0.0*localPoints_;
+
+ waveLength_ = waveLength (initialDepth_, wavePeriod_);
+
+ const scalar waveK = constant::mathematical::twoPi/waveLength_;
+
+ vector waveBoardMotion_(0,0,0);
+ const scalar sigma_ = (2.0*constant::mathematical::pi) / wavePeriod_;
+
+ //first order
+ if ( secondOrder_ == false)
+ {
+ scalar waveBoardStroke_ = (sinh(2.0*waveK*initialDepth_)
+ + 2.0*waveK*initialDepth_)
+ / (2.0*(cosh(2.0*waveK*initialDepth_)
+ - 1.0)) * waveHeigth_;
+ waveBoardMotion_.component(0)= tCoeff*(waveBoardStroke_/2.0)
+ * sin(sigma_*t.value());
+
+ Field<vector>::operator=
+ (
+ waveBoardMotion_
+ );
+ }
+ //second order
+ else if ( secondOrder_ == true)
+ {
+ scalar m1_ = (2.0*(cosh(2.0*waveK*initialDepth_)-1.0))
+ / (sinh(2.0*waveK*initialDepth_)
+ + 2.0*waveK*initialDepth_);
+ waveBoardMotion_.component(0) = tCoeff * (waveHeigth_/(2.0*m1_)
+ * sin(sigma_*t.value()) + pow(waveHeigth_,2)
+ / (32.0*initialDepth_)*(3.0*cosh(waveK*initialDepth_)
+ / pow(sinh(waveK*initialDepth_),3)-2.0/m1_)
+ * sin(2.0*sigma_*t.value()));
+
+ Field<vector>::operator=
+ (
+ waveBoardMotion_
+ );
+ }
+
+ fixedValuePointPatchField<vector>::updateCoeffs();
+}
+
+
+void Foam::waveMakerPistonPointPatchVectorField::write(Ostream& os) const
+{
+ pointPatchField<vector>::write(os);
+ os.writeEntry("initialDepth", initialDepth_);
+ os.writeEntry("wavePeriod", wavePeriod_);
+ os.writeEntry("waveHeigth", waveHeigth_);
+ os.writeEntry("waveLength", waveLength_);
+ os.writeEntry("wavePhase", wavePhase_);
+ os.writeEntry("waveNumber", waveNumber_);
+ os.writeEntry("rampTime", rampTime_);
+ os.writeEntry("g", g_);
+ os.writeEntry("secondOrder", secondOrder_);
+ writeEntry("value", os);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+ makePointPatchTypeField
+ (
+ pointPatchVectorField,
+ waveMakerPistonPointPatchVectorField
+ );
+}
+
+// ************************************************************************* //
diff --git a/src/waveModels/derivedFvPatchFields/waveMakerPiston/waveMakerPistonPointPatchVectorField.H b/src/waveModels/derivedFvPatchFields/waveMakerPiston/waveMakerPistonPointPatchVectorField.H
new file mode 100644
index 00000000000..1929821fb7f
--- /dev/null
+++ b/src/waveModels/derivedFvPatchFields/waveMakerPiston/waveMakerPistonPointPatchVectorField.H
@@ -0,0 +1,179 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2011-2016 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::waveMakerPistonPointPatchVectorField
+
+Description
+ Foam::waveMakerPistonPointPatchVectorField
+
+SourceFiles
+ waveMakerPistonPointPatchVectorField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef waveMakerPistonPointPatchVectorField_H
+#define waveMakerPistonPointPatchVectorField_H
+
+#include "fixedValuePointPatchField.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+ Class waveMakerPistonPointPatchVectorField Declaration
+\*---------------------------------------------------------------------------*/
+
+class waveMakerPistonPointPatchVectorField
+:
+ public fixedValuePointPatchField<vector>
+{
+ // Private data
+
+ //inital water depth
+ scalar initialDepth_;
+
+ //wave period
+ scalar wavePeriod_;
+
+ //wave heigth
+ scalar waveHeigth_;
+
+ //wavelength
+ scalar waveLength_;
+
+ //wave phase
+ scalar wavePhase_;
+
+ //wave number
+ scalar waveNumber_;
+
+ //ramp time
+ scalar rampTime_;
+
+ // gravity vector
+ vector g_;
+
+ //on/off second order generation
+ scalar secondOrder_;
+
+ // Protected Member Functions
+
+ // Dispersion equation
+ virtual scalar waveLength(const scalar h, const scalar T);
+
+ //- Return the time scaling coefficient
+ virtual scalar timeCoeff(const scalar t) const;
+
+public:
+
+ //- Runtime type information
+ TypeName("waveMakerPiston");
+
+
+ // Constructors
+
+ //- Construct from patch and internal field
+ waveMakerPistonPointPatchVectorField
+ (
+ const pointPatch&,
+ const DimensionedField<vector, pointMesh>&
+ );
+
+ //- Construct from patch, internal field and dictionary
+ waveMakerPistonPointPatchVectorField
+ (
+ const pointPatch&,
+ const DimensionedField<vector, pointMesh>&,
+ const dictionary&
+ );
+
+ //- Construct by mapping given patchField<vector> onto a new patch
+ waveMakerPistonPointPatchVectorField
+ (
+ const waveMakerPistonPointPatchVectorField&,
+ const pointPatch&,
+ const DimensionedField<vector, pointMesh>&,
+ const pointPatchFieldMapper&
+ );
+
+ //- Construct and return a clone
+ virtual autoPtr<pointPatchField<vector>> clone() const
+ {
+ return autoPtr<pointPatchField<vector>>
+ (
+ new waveMakerPistonPointPatchVectorField
+ (
+ *this
+ )
+ );
+ }
+
+ //- Construct as copy setting internal field reference
+ waveMakerPistonPointPatchVectorField
+ (
+ const waveMakerPistonPointPatchVectorField&,
+ const DimensionedField<vector, pointMesh>&
+ );
+
+ //- Construct and return a clone setting internal field reference
+ virtual autoPtr<pointPatchField<vector>> clone
+ (
+ const DimensionedField<vector, pointMesh>& iF
+ ) const
+ {
+ return autoPtr<pointPatchField<vector>>
+ (
+ new waveMakerPistonPointPatchVectorField
+ (
+ *this,
+ iF
+ )
+ );
+ }
+
+
+ // Member functions
+
+ // Evaluation functions
+
+ //- Update the coefficients associated with the patch field
+ virtual void updateCoeffs();
+
+
+ //- Write
+ virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/U b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/U
new file mode 100644
index 00000000000..1130305105b
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/U
@@ -0,0 +1,59 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.1 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ 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
+{
+ bottom1
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+ bottom2
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+ leftwall
+ {
+ type movingWallVelocity;
+ value uniform (0 0 0);
+ }
+ back
+ {
+ type empty;
+ }
+ front
+ {
+ type empty;
+ }
+ rightwall
+ {
+ type waveVelocity;
+ value uniform (0 0 0);
+ }
+ top
+ {
+ type pressureInletOutletVelocity;
+ value uniform (0 0 0);
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/alpha.water b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/alpha.water
new file mode 100644
index 00000000000..0d6c1ef5e63
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/alpha.water
@@ -0,0 +1,55 @@
+/*--------------------------------*- 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
+{
+ bottom1
+ {
+ type zeroGradient;
+ }
+ bottom2
+ {
+ type zeroGradient;
+ }
+ front
+ {
+ type empty;
+ }
+ back
+ {
+ type empty;
+ }
+ leftwall
+ {
+ type zeroGradient;
+ }
+ rightwall
+ {
+ type zeroGradient;
+ }
+ top
+ {
+ type inletOutlet;
+ inletValue uniform 0;
+ value uniform 0;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/p_rgh b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/p_rgh
new file mode 100644
index 00000000000..69f34699f7c
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/p_rgh
@@ -0,0 +1,65 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.1 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -2 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ bottom1
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+ bottom2
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+ front
+ {
+ type empty;
+ }
+ back
+ {
+ type empty;
+ }
+ leftwall
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+ rightwall
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+ top
+ {
+ type totalPressure;
+ U U;
+ phi phi;
+ rho rho;
+ psi none;
+ gamma 1;
+ p0 uniform 0;
+ value uniform 0;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/pointDisplacement b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/pointDisplacement
new file mode 100644
index 00000000000..820a34f33d6
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/0.org/pointDisplacement
@@ -0,0 +1,72 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.3.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class pointVectorField;
+ object pointDisplacement;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 0 0 0 0 0];
+
+internalField uniform (0 0 0);
+
+boundaryField
+{
+ bottom1
+ {
+ type zeroGradient;
+ }
+ bottom2
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+ leftwall
+ {
+ type waveMakerFlap;
+ value uniform (0 0 0);
+
+ waveBoardStroke 0.0;
+ waveHeigth 0.06;
+ g (0 0 -9.81);
+ initialDepth 0.25;
+ wavePeriod 2.0;
+
+ rampTime 2.0;
+ waveLength 0;
+ wavePhase 0;
+
+ waveNumber 0.0;
+ secondOrder false;
+
+
+ }
+ back
+ {
+ type empty;
+ }
+ front
+ {
+ type empty;
+ }
+ rightwall
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+ top
+ {
+ type zeroGradient;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/dynamicMeshDict b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/dynamicMeshDict
new file mode 100644
index 00000000000..221b2e62629
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/dynamicMeshDict
@@ -0,0 +1,29 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.0.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object dynamicMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dynamicFvMesh dynamicMotionSolverFvMesh;
+motionSolverLibs ("libfvMotionSolvers.so");
+
+solver displacementLaplacian;
+
+displacementLaplacianCoeffs
+{
+ diffusivity inverseDistance (leftwall);
+}
+
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/g b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/g
new file mode 100644
index 00000000000..d6dea987563
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/g
@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.1 |
+| \\ / 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/waveMakerFlap/constant/transportProperties b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/transportProperties
new file mode 100644
index 00000000000..43a98e9c59e
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/transportProperties
@@ -0,0 +1,37 @@
+/*---------------------------------------------------------------------------*\
+| ========= | |
+| \\ / 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 "constant";
+ object transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phases (water air);
+
+water
+{
+ transportModel Newtonian;
+ nu 1e-06;
+ rho 1000;
+}
+
+air
+{
+ transportModel Newtonian;
+ nu 1.48e-05;
+ rho 1;
+}
+
+sigma 0.07;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/turbulenceProperties b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/turbulenceProperties
new file mode 100644
index 00000000000..115a9830c11
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/turbulenceProperties
@@ -0,0 +1,20 @@
+/*--------------------------------*- 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 "constant";
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType laminar;
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/waveProperties b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/waveProperties
new file mode 100644
index 00000000000..2e959d65523
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/constant/waveProperties
@@ -0,0 +1,28 @@
+/*---------------------------------------------------------------------------*\
+| ========= | |
+| \\ / 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 "constant";
+ object wavesProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+rightwall
+{
+ alpha alpha.water;
+
+ waveModel shallowWaterAbsorption;
+
+ nPaddle 1;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/blockMeshDict b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/blockMeshDict
new file mode 100644
index 00000000000..ab6ee28211e
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/blockMeshDict
@@ -0,0 +1,111 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.7.1 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+vertices
+(
+ (0 0 0)
+ (2 0 0)
+ (2 0 0.7)
+ (0 0 0.7)
+ (0 0.01 0)
+ (2 0.01 0)
+ (2 0.01 0.7)
+ (0 0.01 0.7)
+ (4 0 0)
+ (4 0 0.7)
+ (4 0.01 0.7)
+ (4 0.01 0)
+);
+
+blocks
+(
+ hex (0 1 5 4 3 2 6 7) (200 1 140) simpleGrading (1 1 1)
+ hex (1 8 11 5 2 9 10 6) (200 1 140) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+ bottom1
+ {
+ type wall;
+ faces
+ (
+ (0 1 5 4)
+ );
+ }
+ bottom2
+ {
+ type wall;
+ faces
+ (
+ (1 8 11 5)
+ );
+ }
+ front
+ {
+ type empty;
+ faces
+ (
+ (0 1 2 3)
+ (1 8 9 2)
+ );
+ }
+ back
+ {
+ type empty;
+ faces
+ (
+ (4 5 6 7)
+ (5 11 10 6)
+ );
+ }
+ leftwall
+ {
+ type patch;
+ faces
+ (
+ (0 4 7 3)
+ );
+ }
+ rightwall
+ {
+ type patch;
+ faces
+ (
+ (8 11 10 9)
+ );
+ }
+ top
+ {
+ type wall;
+ faces
+ (
+ (3 2 6 7)
+ (2 9 10 6)
+ );
+ }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/controlDict b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/controlDict
new file mode 100644
index 00000000000..c6345fb7632
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/controlDict
@@ -0,0 +1,139 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.3.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application interDyMFoam;
+
+startFrom startTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 40;
+
+deltaT 0.005;
+
+writeControl adjustableRunTime;
+
+writeInterval 0.1;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 6;
+
+writeCompression uncompressed;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable yes;
+
+adjustTimeStep yes;
+
+maxCo 0.65;
+maxAlphaCo 0.65;
+maxDeltaT 0.05;
+
+functions
+{
+ line
+ {
+ type sets;
+ libs ("libsampling.so");
+ enabled true;
+ writeControl writeTime;
+
+ interpolationScheme cellPoint;
+ setFormat raw;
+
+ sets
+ (
+ s1
+ {
+ type uniform;
+ axis distance;
+ start ( 0.5 0.005 0.0 );
+ end ( 0.5 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s2
+ {
+ type uniform;
+ axis distance;
+ start ( 1.0 0.005 0.0 );
+ end ( 1.0 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s3
+ {
+ type uniform;
+ axis distance;
+ start ( 1.5 0.005 0.0 );
+ end ( 1.5 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s4
+ {
+ type uniform;
+ axis distance;
+ start ( 2.0 0.005 0.0 );
+ end ( 2.0 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s5
+ {
+ type uniform;
+ axis distance;
+ start ( 2.5 0.005 0.0 );
+ end ( 2.5 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s6
+ {
+ type uniform;
+ axis distance;
+ start ( 3.0 0.005 0.0 );
+ end ( 3.0 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s7
+ {
+ type uniform;
+ axis distance;
+ start ( 4.0 0.005 0.0 );
+ end ( 4.0 0.005 0.7 );
+ nPoints 1001;
+ }
+ );
+
+ fixedLocations false;
+
+ fields (alpha.water);
+ }
+}
+
+
+// ************************************************************************* /
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/fvSchemes b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/fvSchemes
new file mode 100644
index 00000000000..bfd3a817e58
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/fvSchemes
@@ -0,0 +1,64 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.1 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ 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 interfaceCompression;
+ div(phi,R) Gauss upwind;
+ div(R) Gauss linear;
+ div(phi,nuTilda) Gauss upwind;
+ div((muEff*dev(T(grad(U))))) Gauss linear;
+ div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default corrected;
+}
+
+fluxRequired
+{
+ default no;
+ p_rgh;
+ pcorr;
+ alpha;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/fvSolution b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/fvSolution
new file mode 100644
index 00000000000..56004f9d3e9
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/fvSolution
@@ -0,0 +1,98 @@
+/*--------------------------------*- 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 "system";
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ "(cellDisplacement|cellDisplacementFinal)"
+ {
+ solver GAMG;
+ tolerance 1e-5;
+ relTol 0;
+ smoother GaussSeidel;
+ cacheAgglomeration false;
+ nCellsInCoarsestLevel 10;
+ agglomerator faceAreaPair;
+ mergeLevels 1;
+ }
+
+ "alpha.water.*"
+ {
+ nAlphaCorr 1;
+ nAlphaSubCycles 3;
+ cAlpha 1;
+ }
+
+ "(pcorr|pcorrFinal)"
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-10;
+ relTol 0;
+ }
+
+ p_rgh
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-07;
+ relTol 0.05;
+ }
+
+ p_rghFinal
+ {
+ $p_rgh;
+ tolerance 1e-07;
+ relTol 0;
+ }
+
+ U
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-06;
+ relTol 0;
+ }
+
+ R
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-08;
+ relTol 0;
+ }
+
+ nuTilda
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-03;
+ relTol 0;
+ }
+}
+
+PIMPLE
+{
+ momentumPredictor no;
+ nCorrectors 3;
+ nNonOrthogonalCorrectors 0;
+ nAlphaCorr 1;
+ nAlphaSubCycles 2;
+ cAlpha 1;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/setFieldsDict b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/setFieldsDict
new file mode 100644
index 00000000000..fbf256400fe
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerFlap/system/setFieldsDict
@@ -0,0 +1,33 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.3.0 |
+| \\ / 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
+);
+
+regions
+(
+ boxToCell
+ {
+ box ( -100 -100 -1 ) ( 100.0 100.0 0.25 );
+ fieldValues ( volScalarFieldValue alpha.water 1 );
+ }
+);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/U b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/U
new file mode 100644
index 00000000000..1130305105b
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/U
@@ -0,0 +1,59 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.1 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ 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
+{
+ bottom1
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+ bottom2
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+ leftwall
+ {
+ type movingWallVelocity;
+ value uniform (0 0 0);
+ }
+ back
+ {
+ type empty;
+ }
+ front
+ {
+ type empty;
+ }
+ rightwall
+ {
+ type waveVelocity;
+ value uniform (0 0 0);
+ }
+ top
+ {
+ type pressureInletOutletVelocity;
+ value uniform (0 0 0);
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/alpha.water b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/alpha.water
new file mode 100644
index 00000000000..0d6c1ef5e63
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/alpha.water
@@ -0,0 +1,55 @@
+/*--------------------------------*- 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
+{
+ bottom1
+ {
+ type zeroGradient;
+ }
+ bottom2
+ {
+ type zeroGradient;
+ }
+ front
+ {
+ type empty;
+ }
+ back
+ {
+ type empty;
+ }
+ leftwall
+ {
+ type zeroGradient;
+ }
+ rightwall
+ {
+ type zeroGradient;
+ }
+ top
+ {
+ type inletOutlet;
+ inletValue uniform 0;
+ value uniform 0;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/p_rgh b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/p_rgh
new file mode 100644
index 00000000000..69f34699f7c
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/p_rgh
@@ -0,0 +1,65 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.1 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -2 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ bottom1
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+ bottom2
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+ front
+ {
+ type empty;
+ }
+ back
+ {
+ type empty;
+ }
+ leftwall
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+ rightwall
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+ top
+ {
+ type totalPressure;
+ U U;
+ phi phi;
+ rho rho;
+ psi none;
+ gamma 1;
+ p0 uniform 0;
+ value uniform 0;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/pointDisplacement b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/pointDisplacement
new file mode 100644
index 00000000000..f3eb7ddba3a
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/0.org/pointDisplacement
@@ -0,0 +1,72 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.3.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class pointVectorField;
+ object pointDisplacement;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 0 0 0 0 0];
+
+internalField uniform (0 0 0);
+
+boundaryField
+{
+ bottom1
+ {
+ type zeroGradient;
+ }
+ bottom2
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+ leftwall
+ {
+ type waveMakerPiston;
+ value uniform (0 0 0);
+
+ waveBoardStroke 0;
+ waveHeigth 0.06;
+ g (0 0 -9.81);
+ waterDepthRef 0.25;
+ initialDepth 0.25;
+
+ wavePeriod 2.0;
+
+ rampTime 2.0;
+ waveLength 0;
+ wavePhase 0;
+
+ waveNumber 0.0;
+ secondOrder false;
+ }
+ back
+ {
+ type empty;
+ }
+ front
+ {
+ type empty;
+ }
+ rightwall
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+ top
+ {
+ type zeroGradient;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/dynamicMeshDict b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/dynamicMeshDict
new file mode 100644
index 00000000000..221b2e62629
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/dynamicMeshDict
@@ -0,0 +1,29 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.0.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object dynamicMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dynamicFvMesh dynamicMotionSolverFvMesh;
+motionSolverLibs ("libfvMotionSolvers.so");
+
+solver displacementLaplacian;
+
+displacementLaplacianCoeffs
+{
+ diffusivity inverseDistance (leftwall);
+}
+
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/g b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/g
new file mode 100644
index 00000000000..d6dea987563
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/g
@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.1 |
+| \\ / 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/waveMakerPiston/constant/transportProperties b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/transportProperties
new file mode 100644
index 00000000000..43a98e9c59e
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/transportProperties
@@ -0,0 +1,37 @@
+/*---------------------------------------------------------------------------*\
+| ========= | |
+| \\ / 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 "constant";
+ object transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phases (water air);
+
+water
+{
+ transportModel Newtonian;
+ nu 1e-06;
+ rho 1000;
+}
+
+air
+{
+ transportModel Newtonian;
+ nu 1.48e-05;
+ rho 1;
+}
+
+sigma 0.07;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/turbulenceProperties b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/turbulenceProperties
new file mode 100644
index 00000000000..115a9830c11
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/turbulenceProperties
@@ -0,0 +1,20 @@
+/*--------------------------------*- 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 "constant";
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType laminar;
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/waveProperties b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/waveProperties
new file mode 100644
index 00000000000..2e959d65523
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/constant/waveProperties
@@ -0,0 +1,28 @@
+/*---------------------------------------------------------------------------*\
+| ========= | |
+| \\ / 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 "constant";
+ object wavesProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+rightwall
+{
+ alpha alpha.water;
+
+ waveModel shallowWaterAbsorption;
+
+ nPaddle 1;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/blockMeshDict b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/blockMeshDict
new file mode 100644
index 00000000000..f4fdd4a279c
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/blockMeshDict
@@ -0,0 +1,111 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.7.1 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+vertices
+(
+ (0 0 0)
+ (2 0 0)
+ (2 0 0.7)
+ (0 0 0.7)
+ (0 0.01 0)
+ (2 0.01 0)
+ (2 0.01 0.7)
+ (0 0.01 0.7)
+ (4 0 0)
+ (4 0 0.7)
+ (4 0.01 0.7)
+ (4 0.01 0)
+);
+
+blocks
+(
+ hex (0 1 5 4 3 2 6 7) (100 1 140) simpleGrading (1 1 1)
+ hex (1 8 11 5 2 9 10 6) (300 1 140) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+ bottom1
+ {
+ type wall;
+ faces
+ (
+ (0 1 5 4)
+ );
+ }
+ bottom2
+ {
+ type wall;
+ faces
+ (
+ (1 8 11 5)
+ );
+ }
+ front
+ {
+ type empty;
+ faces
+ (
+ (0 1 2 3)
+ (1 8 9 2)
+ );
+ }
+ back
+ {
+ type empty;
+ faces
+ (
+ (4 5 6 7)
+ (5 11 10 6)
+ );
+ }
+ leftwall
+ {
+ type patch;
+ faces
+ (
+ (0 4 7 3)
+ );
+ }
+ rightwall
+ {
+ type patch;
+ faces
+ (
+ (8 11 10 9)
+ );
+ }
+ top
+ {
+ type wall;
+ faces
+ (
+ (3 2 6 7)
+ (2 9 10 6)
+ );
+ }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/controlDict b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/controlDict
new file mode 100644
index 00000000000..c6345fb7632
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/controlDict
@@ -0,0 +1,139 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.3.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application interDyMFoam;
+
+startFrom startTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 40;
+
+deltaT 0.005;
+
+writeControl adjustableRunTime;
+
+writeInterval 0.1;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 6;
+
+writeCompression uncompressed;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable yes;
+
+adjustTimeStep yes;
+
+maxCo 0.65;
+maxAlphaCo 0.65;
+maxDeltaT 0.05;
+
+functions
+{
+ line
+ {
+ type sets;
+ libs ("libsampling.so");
+ enabled true;
+ writeControl writeTime;
+
+ interpolationScheme cellPoint;
+ setFormat raw;
+
+ sets
+ (
+ s1
+ {
+ type uniform;
+ axis distance;
+ start ( 0.5 0.005 0.0 );
+ end ( 0.5 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s2
+ {
+ type uniform;
+ axis distance;
+ start ( 1.0 0.005 0.0 );
+ end ( 1.0 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s3
+ {
+ type uniform;
+ axis distance;
+ start ( 1.5 0.005 0.0 );
+ end ( 1.5 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s4
+ {
+ type uniform;
+ axis distance;
+ start ( 2.0 0.005 0.0 );
+ end ( 2.0 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s5
+ {
+ type uniform;
+ axis distance;
+ start ( 2.5 0.005 0.0 );
+ end ( 2.5 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s6
+ {
+ type uniform;
+ axis distance;
+ start ( 3.0 0.005 0.0 );
+ end ( 3.0 0.005 0.7 );
+ nPoints 1001;
+ }
+
+ s7
+ {
+ type uniform;
+ axis distance;
+ start ( 4.0 0.005 0.0 );
+ end ( 4.0 0.005 0.7 );
+ nPoints 1001;
+ }
+ );
+
+ fixedLocations false;
+
+ fields (alpha.water);
+ }
+}
+
+
+// ************************************************************************* /
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/fvSchemes b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/fvSchemes
new file mode 100644
index 00000000000..bfd3a817e58
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/fvSchemes
@@ -0,0 +1,64 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.1.1 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ 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 interfaceCompression;
+ div(phi,R) Gauss upwind;
+ div(R) Gauss linear;
+ div(phi,nuTilda) Gauss upwind;
+ div((muEff*dev(T(grad(U))))) Gauss linear;
+ div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default corrected;
+}
+
+fluxRequired
+{
+ default no;
+ p_rgh;
+ pcorr;
+ alpha;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/fvSolution b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/fvSolution
new file mode 100644
index 00000000000..c25fef42d7d
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/fvSolution
@@ -0,0 +1,97 @@
+/*--------------------------------*- 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 "system";
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ "(cellDisplacement|cellDisplacementFinal)"
+ {
+ solver GAMG;
+ tolerance 1e-5;
+ relTol 0;
+ smoother GaussSeidel;
+ cacheAgglomeration false;
+ nCellsInCoarsestLevel 10;
+ agglomerator faceAreaPair;
+ mergeLevels 1;
+ }
+
+ "alpha.water.*"
+ {
+ nAlphaCorr 1;
+ nAlphaSubCycles 3;
+ cAlpha 1;
+ }
+
+ "(pcorr|pcorrFinal)"
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-10;
+ relTol 0;
+ }
+
+ p_rgh
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-07;
+ relTol 0.05;
+ }
+
+ p_rghFinal
+ {
+ $p_rgh;
+ tolerance 1e-07;
+ relTol 0;
+ }
+
+ U
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-06;
+ relTol 0;
+ }
+ R
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-08;
+ relTol 0;
+ }
+
+ nuTilda
+ {
+ solver PBiCG;
+ preconditioner DILU;
+ tolerance 1e-03;
+ relTol 0;
+ }
+}
+
+PIMPLE
+{
+ momentumPredictor no;
+ nCorrectors 3;
+ nNonOrthogonalCorrectors 0;
+ nAlphaCorr 1;
+ nAlphaSubCycles 2;
+ cAlpha 1;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/setFieldsDict b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/setFieldsDict
new file mode 100644
index 00000000000..fbf256400fe
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/waveMakerPiston/system/setFieldsDict
@@ -0,0 +1,33 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.3.0 |
+| \\ / 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
+);
+
+regions
+(
+ boxToCell
+ {
+ box ( -100 -100 -1 ) ( 100.0 100.0 0.25 );
+ fieldValues ( volScalarFieldValue alpha.water 1 );
+ }
+);
+
+
+// ************************************************************************* //
--
GitLab