From 2aa78c6db34f30f9277d3d0a687b093079b7f0cc Mon Sep 17 00:00:00 2001 From: Will Bainbridge Date: Tue, 30 May 2017 09:58:42 +0100 Subject: [PATCH] tutorials: interFoam: Added 2D wave propagation case --- .../multiphase/interFoam/laminar/wave/0.org/U | 63 ++++++++++++ .../interFoam/laminar/wave/0.org/alpha.water | 45 +++++++++ .../interFoam/laminar/wave/0.org/p_rgh | 38 ++++++++ .../interFoam/laminar/wave/Allclean | 7 ++ .../multiphase/interFoam/laminar/wave/Allrun | 33 +++++++ .../interFoam/laminar/wave/constant/fvOptions | 32 +++++++ .../interFoam/laminar/wave/constant/g | 22 +++++ .../laminar/wave/constant/transportProperties | 37 ++++++++ .../wave/constant/turbulenceProperties | 21 ++++ .../laminar/wave/system/blockMeshDict | 88 +++++++++++++++++ .../interFoam/laminar/wave/system/controlDict | 72 ++++++++++++++ .../laminar/wave/system/decomposeParDict | 29 ++++++ .../laminar/wave/system/extrudeMeshDict | 40 ++++++++ .../interFoam/laminar/wave/system/fvSchemes | 58 +++++++++++ .../interFoam/laminar/wave/system/fvSolution | 95 +++++++++++++++++++ .../laminar/wave/system/refineMeshDictX | 40 ++++++++ .../laminar/wave/system/refineMeshDictY | 40 ++++++++ .../interFoam/laminar/wave/system/topoSetDict | 42 ++++++++ .../laminar/wave/system/topoSetDict1 | 32 +++++++ .../laminar/wave/system/topoSetDict2 | 32 +++++++ .../laminar/wave/system/topoSetDict3 | 32 +++++++ .../laminar/wave/system/topoSetDict4 | 32 +++++++ .../laminar/wave/system/topoSetDict5 | 32 +++++++ .../laminar/wave/system/topoSetDict6 | 32 +++++++ 24 files changed, 994 insertions(+) create mode 100644 tutorials/multiphase/interFoam/laminar/wave/0.org/U create mode 100644 tutorials/multiphase/interFoam/laminar/wave/0.org/alpha.water create mode 100644 tutorials/multiphase/interFoam/laminar/wave/0.org/p_rgh create mode 100755 tutorials/multiphase/interFoam/laminar/wave/Allclean create mode 100755 tutorials/multiphase/interFoam/laminar/wave/Allrun create mode 100644 tutorials/multiphase/interFoam/laminar/wave/constant/fvOptions create mode 100644 tutorials/multiphase/interFoam/laminar/wave/constant/g create mode 100644 tutorials/multiphase/interFoam/laminar/wave/constant/transportProperties create mode 100644 tutorials/multiphase/interFoam/laminar/wave/constant/turbulenceProperties create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/blockMeshDict create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/controlDict create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/decomposeParDict create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/extrudeMeshDict create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/fvSchemes create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/fvSolution create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/refineMeshDictX create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/refineMeshDictY create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict1 create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict2 create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict3 create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict4 create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict5 create mode 100644 tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict6 diff --git a/tutorials/multiphase/interFoam/laminar/wave/0.org/U b/tutorials/multiphase/interFoam/laminar/wave/0.org/U new file mode 100644 index 000000000..b94a6a5ae --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/0.org/U @@ -0,0 +1,63 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / 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 +{ + #includeEtc "caseDicts/setConstraintTypes" + + left + { + type waveVelocity; + origin (0 0 0); + direction (1 0 0); + speed 2; + waves + ( + Airy + { + length 300; + amplitude 2.5; + phase 0; + angle 0; + } + ); + scale table ((1200 1) (1800 0)); + crossScale constant 1; + } + right + { + type outletPhaseMeanVelocity; + Umean 2; + alpha alpha.water; + } + top + { + type pressureInletOutletVelocity; + value uniform (0 0 0); + } + bottom + { + type noSlip; + } +} + + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/0.org/alpha.water b/tutorials/multiphase/interFoam/laminar/wave/0.org/alpha.water new file mode 100644 index 000000000..3f80f4670 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/0.org/alpha.water @@ -0,0 +1,45 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class volScalarField; + location "0"; + object alpha.water; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +dimensions [0 0 0 0 0 0 0]; + +internalField uniform 0; + +boundaryField +{ + #includeEtc "caseDicts/setConstraintTypes" + + "(right|bottom)" + { + type zeroGradient; + } + left + { + type waveAlpha; + U U; + inletOutlet true; + } + top + { + type inletOutlet; + inletValue uniform 0; + value uniform 0; + } +} + + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/0.org/p_rgh b/tutorials/multiphase/interFoam/laminar/wave/0.org/p_rgh new file mode 100644 index 000000000..f134851a4 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/0.org/p_rgh @@ -0,0 +1,38 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / 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 +{ + #includeEtc "caseDicts/setConstraintTypes" + + "(left|right|bottom)" + { + type fixedFluxPressure; + value uniform 0; + } + top + { + type totalPressure; + p0 uniform 0; + } +} + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/Allclean b/tutorials/multiphase/interFoam/laminar/wave/Allclean new file mode 100755 index 000000000..7dde89aec --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/Allclean @@ -0,0 +1,7 @@ +#!/bin/sh + +cd ${0%/*} || exit 1 + +. $WM_PROJECT_DIR/bin/tools/CleanFunctions + +cleanCase && rm -rf 0 diff --git a/tutorials/multiphase/interFoam/laminar/wave/Allrun b/tutorials/multiphase/interFoam/laminar/wave/Allrun new file mode 100755 index 000000000..3ee7e4898 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/Allrun @@ -0,0 +1,33 @@ +#!/bin/sh + +cd ${0%/*} || exit 1 + +. $WM_PROJECT_DIR/bin/tools/RunFunctions + +runApplication blockMesh + +cp -r 0.org 0 + +runApplication extrudeMesh + +for i in 1 2 +do + runApplication -s $i topoSet -dict system/topoSetDict$i + runApplication -s $i refineMesh -dict system/refineMeshDictX -overwrite +done + +for i in 3 4 5 6 +do + runApplication -s $i topoSet -dict system/topoSetDict$i + runApplication -s $i refineMesh -dict system/refineMeshDictY -overwrite +done + +runApplication topoSet + +runApplication setWaves -alpha alpha.water + +runApplication decomposePar + +runParallel $(getApplication) + +runApplication reconstructPar diff --git a/tutorials/multiphase/interFoam/laminar/wave/constant/fvOptions b/tutorials/multiphase/interFoam/laminar/wave/constant/fvOptions new file mode 100644 index 000000000..a2691bbb9 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/constant/fvOptions @@ -0,0 +1,32 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "constant"; + object fvOptions; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +option1 +{ + type verticalDamping; + + selectionMode cellZone; + cellZone right; + + lambda 0.1; + + timeStart 0; + duration 1e6; +} + + +//************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/constant/g b/tutorials/multiphase/interFoam/laminar/wave/constant/g new file mode 100644 index 000000000..0cc222ca3 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/constant/g @@ -0,0 +1,22 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / 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 -9.81 0); + + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/constant/transportProperties b/tutorials/multiphase/interFoam/laminar/wave/constant/transportProperties new file mode 100644 index 000000000..10b127326 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/constant/transportProperties @@ -0,0 +1,37 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ 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; + + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/constant/turbulenceProperties b/tutorials/multiphase/interFoam/laminar/wave/constant/turbulenceProperties new file mode 100644 index 000000000..c2c3b28a1 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/constant/turbulenceProperties @@ -0,0 +1,21 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / 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/wave/system/blockMeshDict b/tutorials/multiphase/interFoam/laminar/wave/system/blockMeshDict new file mode 100644 index 000000000..b35cc50a6 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/blockMeshDict @@ -0,0 +1,88 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object blockMeshDict; +} + +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +convertToMeters 1; + +vertices +( + (0 -300 -10) + (1200 -300 -10) + (1200 300 -10) + (0 300 -10) + (0 -300 10) + (1200 -300 10) + (1200 300 10) + (0 300 10) +); + +blocks +( + hex (0 1 2 3 4 5 6 7) (67 40 1) simpleGrading (1 1 1) +); + +edges +( +); + +defaultPatch +{ + name frontAndBack; + type empty; +} + +boundary +( + left + { + type patch; + faces + ( + (0 4 7 3) + ); + } + right + { + type patch; + faces + ( + (2 6 5 1) + ); + } + bottom + { + type patch; + faces + ( + (0 1 5 4) + ); + } + top + { + type patch; + faces + ( + (2 3 7 6) + ); + } +); + +mergePatchPairs +( +); + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/controlDict b/tutorials/multiphase/interFoam/laminar/wave/system/controlDict new file mode 100644 index 000000000..2e359aee6 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/controlDict @@ -0,0 +1,72 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object controlDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +application interFoam; + +startFrom startTime; + +startTime 0; + +stopAt endTime; + +endTime 200; + +deltaT 0.05; + +writeControl adjustableRunTime; + +writeInterval 1; + +purgeWrite 0; + +writeFormat binary; + +writePrecision 6; + +writeCompression uncompressed; + +timeFormat general; + +timePrecision 6; + +runTimeModifiable yes; + +adjustTimeStep no; + +maxCo 1; + +maxAlphaCo 1; + +maxDeltaT 1; + +libs +( + "libwaves.so" +); + +functions +{ + interfaceHeight1 + { + type interfaceHeight; + libs ("libfieldFunctionObjects.so"); + locations ((300 0 0) (450 0 0) (600 0 0)); + alpha alpha.water; + } +} + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/decomposeParDict b/tutorials/multiphase/interFoam/laminar/wave/system/decomposeParDict new file mode 100644 index 000000000..96da5c639 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/decomposeParDict @@ -0,0 +1,29 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object decomposeParDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +numberOfSubdomains 6; + +method simple; + +simpleCoeffs +{ + n (3 2 1); + delta 0.001; +} + + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/extrudeMeshDict b/tutorials/multiphase/interFoam/laminar/wave/system/extrudeMeshDict new file mode 100644 index 000000000..c1db784c5 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/extrudeMeshDict @@ -0,0 +1,40 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object extrudeMeshDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +constructFrom mesh; + +sourceCase "."; + +sourcePatches (right); + +flipNormals false; + +nLayers 25; + +expansionRatio 1.09; + +extrudeModel linearNormal; + +linearNormalCoeffs +{ + thickness 1500; +} + +mergeFaces false; + + +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/fvSchemes b/tutorials/multiphase/interFoam/laminar/wave/system/fvSchemes new file mode 100644 index 000000000..9d964c453 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/fvSchemes @@ -0,0 +1,58 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object fvSchemes; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +ddtSchemes +{ + default CrankNicolson ocCoeff + { + type scale; + scale linearRamp; + duration 1.0; + value 0.9; + }; +} + +gradSchemes +{ + default Gauss linear; +} + +divSchemes +{ + div(rhoPhi,U) Gauss linearUpwindV 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 corrected; +} + +interpolationSchemes +{ + default linear; +} + +snGradSchemes +{ + default corrected; +} + + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/fvSolution b/tutorials/multiphase/interFoam/laminar/wave/system/fvSolution new file mode 100644 index 000000000..96037e94f --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/fvSolution @@ -0,0 +1,95 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object fvSolution; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +solvers +{ + "alpha.water.*" + { + nAlphaCorr 3; + nAlphaSubCycles 1; + cAlpha 1; + icAlpha 0; + + alphaOuterCorrectors yes; + + MULESCorr yes; + nLimiterIter 25; + alphaApplyPrevCorr yes; + + solver smoothSolver; + smoother symGaussSeidel; + tolerance 1e-8; + relTol 0; + minIter 1; + } + + pcorr + { + solver GAMG; + smoother DIC; + tolerance 1e-4; + relTol 0.01; + } + + pcorrFinal + { + $pcorr; + relTol 0; + }; + + + p_rgh + { + solver GAMG; + smoother DIC; + tolerance 1e-7; + relTol 0.001; + } + + p_rghFinal + { + $p_rgh; + relTol 0; + } + + "U.*" + { + solver smoothSolver; + smoother symGaussSeidel; + tolerance 1e-7; + relTol 0; + } +} + +PIMPLE +{ + momentumPredictor yes; + nOuterCorrectors 1; + nCorrectors 3; + nNonOrthogonalCorrectors 0; +} + +relaxationFactors +{ + equations + { + ".*" 1; + } +} + + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/refineMeshDictX b/tutorials/multiphase/interFoam/laminar/wave/system/refineMeshDictX new file mode 100644 index 000000000..4b8c5e898 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/refineMeshDictX @@ -0,0 +1,40 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object refineMeshDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +set box; + +coordinateSystem global; + +globalCoeffs +{ + tan1 (1 0 0); + tan2 (0 1 0); +} + +directions +( + tan1 +); + +useHexTopology true; + +geometricCut false; + +writeMesh false; + + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/refineMeshDictY b/tutorials/multiphase/interFoam/laminar/wave/system/refineMeshDictY new file mode 100644 index 000000000..5a1c6c408 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/refineMeshDictY @@ -0,0 +1,40 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object refineMeshDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +set box; + +coordinateSystem global; + +globalCoeffs +{ + tan1 (1 0 0); + tan2 (0 1 0); +} + +directions +( + tan2 +); + +useHexTopology true; + +geometricCut false; + +writeMesh false; + + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict new file mode 100644 index 000000000..d9f4d4ef8 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict @@ -0,0 +1,42 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object topoSetDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +actions +( + { + name right; + type cellSet; + action new; + source boxToCell; + sourceInfo + { + box (1800 -1e6 -1e6) (1e6 1e6 1e6); + } + } + { + name right; + type cellZoneSet; + action new; + source setToCellZone; + sourceInfo + { + set right; + } + } +); + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict1 b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict1 new file mode 100644 index 000000000..85870f330 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict1 @@ -0,0 +1,32 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object topoSetDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +actions +( + { + name box; + type cellSet; + action new; + source boxToCell; + sourceInfo + { + box (-1e6 -40 -1e6) (1300 40 1e6); + } + } +); + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict2 b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict2 new file mode 100644 index 000000000..a03ca2a2c --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict2 @@ -0,0 +1,32 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object topoSetDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +actions +( + { + name box; + type cellSet; + action new; + source boxToCell; + sourceInfo + { + box (-1e6 -30 -1e6) (1200 30 1e6); + } + } +); + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict3 b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict3 new file mode 100644 index 000000000..b3ab81126 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict3 @@ -0,0 +1,32 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object topoSetDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +actions +( + { + name box; + type cellSet; + action new; + source boxToCell; + sourceInfo + { + box (-1e6 -40 -1e6) (1e6 40 1e6); + } + } +); + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict4 b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict4 new file mode 100644 index 000000000..dc8928996 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict4 @@ -0,0 +1,32 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object topoSetDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +actions +( + { + name box; + type cellSet; + action new; + source boxToCell; + sourceInfo + { + box (-1e6 -30 -1e6) (1e6 30 1e6); + } + } +); + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict5 b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict5 new file mode 100644 index 000000000..07120acc4 --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict5 @@ -0,0 +1,32 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object topoSetDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +actions +( + { + name box; + type cellSet; + action new; + source boxToCell; + sourceInfo + { + box (-1e6 -20 -1e6) (1e6 20 1e6); + } + } +); + +// ************************************************************************* // diff --git a/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict6 b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict6 new file mode 100644 index 000000000..226b0a5fb --- /dev/null +++ b/tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict6 @@ -0,0 +1,32 @@ +/*--------------------------------*- C++ -*----------------------------------*\ +| ========= | | +| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | +| \\ / O peration | Version: dev | +| \\ / A nd | Web: www.OpenFOAM.org | +| \\/ M anipulation | | +\*---------------------------------------------------------------------------*/ +FoamFile +{ + version 2.0; + format ascii; + class dictionary; + location "system"; + object topoSetDict; +} +// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // + +actions +( + { + name box; + type cellSet; + action new; + source boxToCell; + sourceInfo + { + box (-1e6 -10 -1e6) (1e6 10 1e6); + } + } +); + +// ************************************************************************* //