Commit 775194be authored by Sergio Ferraris's avatar Sergio Ferraris Committed by Kutalmis Bercin
Browse files

TUT: new multiphase tutorial: damBreakPermeable

parent 3f7c0577
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
leftWall
{
type noSlip;
}
rightWall
{
type permeableAlphaPressureInletOutletVelocity;
alpha alpha.water;
alphaMin 0.01;
value uniform (0 0 0);
}
lowerWall
{
type noSlip;
}
atmosphere
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
defaultFaces
{
type empty;
}
}
// ************************************************************************* //
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ 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
{
leftWall
{
type zeroGradient;
}
rightWall
{
type zeroGradient;
}
lowerWall
{
type zeroGradient;
}
atmosphere
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
defaultFaces
{
type empty;
}
}
// ************************************************************************* //
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -3 0 0 0 0];
internalField uniform 0.1;
boundaryField
{
leftWall
{
type epsilonWallFunction;
value uniform 0.1;
}
rightWall
{
type epsilonWallFunction;
value uniform 0.1;
}
lowerWall
{
type epsilonWallFunction;
value uniform 0.1;
}
atmosphere
{
type inletOutlet;
inletValue uniform 0.1;
value uniform 0.1;
}
defaultFaces
{
type empty;
}
}
// ************************************************************************* //
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0.1;
boundaryField
{
leftWall
{
type kqRWallFunction;
value uniform 0.1;
}
rightWall
{
type kqRWallFunction;
value uniform 0.1;
}
lowerWall
{
type kqRWallFunction;
value uniform 0.1;
}
atmosphere
{
type inletOutlet;
inletValue uniform 0.1;
value uniform 0.1;
}
defaultFaces
{
type empty;
}
}
// ************************************************************************* //
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
leftWall
{
type nutkWallFunction;
value uniform 0;
}
rightWall
{
type nutkWallFunction;
value uniform 0;
}
lowerWall
{
type nutkWallFunction;
value uniform 0;
}
atmosphere
{
type calculated;
value uniform 0;
}
defaultFaces
{
type empty;
}
}
// ************************************************************************* //
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
leftWall
{
type fixedFluxPressure;
value uniform 0;
}
rightWall
{
type prghPermeableAlphaTotalPressure;
alpha alpha.water;
alphaMin 0.01;
p uniform 0;
value uniform 0;
}
lowerWall
{
type fixedFluxPressure;
value uniform 0;
}
atmosphere
{
type totalPressure;
p0 uniform 0;
}
defaultFaces
{
type empty;
}
}
// ************************************************************************* //
#!/bin/sh
cd "${0%/*}" || exit # Run from this directory
. ${WM_PROJECT_DIR:?}/bin/tools/CleanFunctions # Tutorial clean functions
#------------------------------------------------------------------------------
cleanCase0
#------------------------------------------------------------------------------
#!/bin/sh
cd "${0%/*}" || exit # Run from this directory
. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions # Tutorial run functions
#------------------------------------------------------------------------------
restore0Dir
runApplication blockMesh
runApplication setFields
runApplication decomposePar
runParallel $(getApplication)
runParallel redistributePar -reconstruct -overwrite
#------------------------------------------------------------------------------
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class uniformDimensionedVectorField;
object g;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -2 0 0 0 0];
value (0 -9.81 0);
// ************************************************************************* //
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
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;
// ************************************************************************* //
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RAS;
density variable;
RAS
{
RASModel kEpsilon;
turbulence on;
printCoeffs on;
}
// ************************************************************************* //
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
scale 0.146;
vertices
(
(0 0 0)
(2 0 0)
(2.16438 0 0)
(4 0 0)
(0 0.32876 0)
(2 0.32876 0)
(2.16438 0.32876 0)
(4 0.32876 0)
(0 4 0)
(2 4 0)
(2.16438 4 0)
(4 4 0)
(0 0 0.1)
(2 0 0.1)
(2.16438 0 0.1)
(4 0 0.1)
(0 0.32876 0.1)
(2 0.32876 0.1)
(2.16438 0.32876 0.1)
(4 0.32876 0.1)
(0 4 0.1)
(2 4 0.1)
(2.16438 4 0.1)
(4 4 0.1)
);
blocks
(
hex (0 1 5 4 12 13 17 16) (23 8 1) simpleGrading (1 1 1)
hex (2 3 7 6 14 15 19 18) (19 8 1) simpleGrading (1 1 1)
hex (4 5 9 8 16 17 21 20) (23 42 1) simpleGrading (1 1 1)
hex (5 6 10 9 17 18 22 21) (4 42 1) simpleGrading (1 1 1)
hex (6 7 11 10 18 19 23 22) (19 42 1) simpleGrading (1 1 1)
);
edges
(
);
boundary
(
leftWall
{
type wall;
faces
(
(0 12 16 4)
(4 16 20 8)
);
}
rightWall
{
type wall;
faces
(
(7 19 15 3)
(11 23 19 7)
);
}
lowerWall
{
type wall;
faces
(
(0 1 13 12)
(1 5 17 13)
(5 6 18 17)
(2 14 18 6)
(2 3 15 14)
);
}
atmosphere
{
type patch;
faces
(
(8 20 21 9)
(9 21 22 10)
(10 22 23 11)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application interFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 1;
deltaT 0.001;
writeControl adjustable;
writeInterval 0.05;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;