songtianlun/openfoam
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity

TUT: interFoam: new tutorial for electrostatic deposition

Browse Source
This commit is contained in:
Kutalmis Bercin 2021-09-29 08:31:25 +01:00 committed by Andrew Heather
parent 19f7825a04
commit 27f4cee78d
27 changed files with 1131 additions and 0 deletions
Show Stats Download Patch File Download Diff File Expand all files Collapse all files

37
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/U Normal file
View File

@ -0,0 +1,37 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / 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
{
metalSheet
{
type movingWallVelocity;
value uniform (0 0 0);
}
"side-.*"
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
}
// ************************************************************************* //

45
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/alpha.water Normal file
View File

@ -0,0 +1,45 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / 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
{
metalSheet
{
type zeroGradient;
}
"(side-01|side-06|side-03|side-04|side-05)"
{
type variableHeightFlowRate;
lowerBound 0;
upperBound 1;
value uniform 0;
}
side-02
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
}
// ************************************************************************* //

68
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/electricPotential:V Normal file
View File

@ -0,0 +1,68 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object electricPotential:V;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 2 -3 0 0 -1 0];
internalField uniform 0;
boundaryField
{
metalSheet
{
// Mandatory entries
type electrostaticDeposition;
h uniform 0;
CoulombicEfficiency uniform 2.14e-08;
resistivity uniform 3.00e+06;
// Conditional mandatory entries
phases
{
alpha.air
{
sigma 1e-10;
}
alpha.water
{
sigma 0.14;
}
}
// Optional entries
jMin 0;
qMin 0;
Rbody 0.1;
Vi 0;
qCumulative uniform 0;
// Inherited entries
value uniform 0;
}
"side-05"
{
type fixedValue;
value uniform 100;
}
"(side-01|side-02|side-03|side-04|side-06)"
{
type zeroGradient;
}
}
// ************************************************************************* //

38
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/k Normal file
View File

@ -0,0 +1,38 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / 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 1e-3;
boundaryField
{
metalSheet
{
type kqRWallFunction;
value $internalField;
}
"side-.*"
{
type inletOutlet;
inletValue uniform 1e-3;
value uniform 1e-3;
}
}
// ************************************************************************* //

37
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/nut Normal file
View File

@ -0,0 +1,37 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / 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 1e-05;
boundaryField
{
metalSheet
{
type nutkWallFunction;
value $internalField;
}
"side-.*"
{
type calculated;
value $internalField;
}
}
// ************************************************************************* //

38
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/omega Normal file
View File

@ -0,0 +1,38 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 -1 0 0 0 0];
internalField uniform 0.22;
boundaryField
{
metalSheet
{
type omegaWallFunction;
value $internalField;
}
"side-.*"
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
}
// ************************************************************************* //

37
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/p_rgh Normal file
View File

@ -0,0 +1,37 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / 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
{
metalSheet
{
type fixedFluxPressure;
value $internalField;
}
"side-.*"
{
type totalPressure;
p0 uniform 0;
}
}
// ************************************************************************* //

8
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allclean Executable file
View File

@ -0,0 +1,8 @@
#!/bin/sh
cd "${0%/*}" || exit # Run from this directory
. ${WM_PROJECT_DIR:?}/bin/tools/CleanFunctions # Tutorial clean functions
#------------------------------------------------------------------------------
cleanCase0
#------------------------------------------------------------------------------

10
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun Executable file
View File

@ -0,0 +1,10 @@
#!/bin/sh
cd "${0%/*}" || exit # Run from this directory
. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions # Tutorial run functions
#------------------------------------------------------------------------------
./Allrun.pre
runApplication $(getApplication)
#------------------------------------------------------------------------------

29
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun-parallel Executable file
View File

@ -0,0 +1,29 @@
#!/bin/sh
cd "${0%/*}" || exit # Run from this directory
. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions # Tutorial run functions
#------------------------------------------------------------------------------
./Allrun.pre
runApplication decomposePar
runParallel -s 1 $(getApplication)
runApplication reconstructPar
# restart
latestTime=$(foamListTimes -latestTime)
mv -f "$latestTime" "$latestTime".bak
rm -rf processor*
runParallel -s decompose redistributePar -decompose -latestTime
runParallel -s 2 $(getApplication)
runParallel -s reconstruct redistributePar -reconstruct -latestTime
#------------------------------------------------------------------------------

20
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun.pre Executable file
View File

@ -0,0 +1,20 @@
#!/bin/sh
cd "${0%/*}" || exit # Run from this directory
. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions # Tutorial run functions
#------------------------------------------------------------------------------
runApplication blockMesh
runApplication snappyHexMesh -overwrite
rm -rf 0/
restore0Dir
runApplication setFields
runApplication transformPoints -rollPitchYaw "(0 -90 0)"
runApplication checkMesh -allGeometry -allTopology
#------------------------------------------------------------------------------

28
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/dynamicMeshDict Normal file
View File

@ -0,0 +1,28 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dynamicFvMesh dynamicMotionSolverFvMesh;
motionSolver solidBody;
solidBodyMotionFunction tabulated6DoFMotion;
timeDataFileName "<constant>/meshMotion.dat";
CofG (0 0 0);
// ************************************************************************* //

21
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/g Normal file
View File

@ -0,0 +1,21 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / 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 0 -9.81);
// ************************************************************************* //

21
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/hRef Normal file
View File

@ -0,0 +1,21 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class uniformDimensionedScalarField;
object hRef;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 0 0 0 0 0];
value -0.3;
// ************************************************************************* //

9
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/meshMotion.dat Normal file
View File

@ -0,0 +1,9 @@
4
(
// Time Linear (xyz) Rotation (xyz)
(0 ((0 0 0) (0 0 0)))
(10 ((0 0 -0.80) (0 0 0)))
(11 ((0 0 -0.80) (0 0 0)))
(21 ((0 0 0) (0 0 0)))
)

36
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/transportProperties Normal file
View File

@ -0,0 +1,36 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
phases (water air);
water
{
transportModel Newtonian;
rho 997.561;
nu 8.90883e-07;
}
air
{
transportModel Newtonian;
rho 1.1765;
nu 1.58e-05;
}
sigma 0.072;
// ************************************************************************* //

BIN
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/triSurface/metalSheet.stl.gz Normal file
View File

Binary file not shown.

25
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/turbulenceProperties Normal file
View File

@ -0,0 +1,25 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RAS;
RAS
{
RASModel kOmegaSST;
}
// ************************************************************************* //

52
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/FOelectricPotential Normal file
View File

@ -0,0 +1,52 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2107 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object FOelectricPotential;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
electricPotential
{
// Mandatory entries
type electricPotential;
libs (solverFunctionObjects);
phases
{
alpha.air
{
epsilonr 1.12940906737;
sigma 1e-10;
}
alpha.water
{
epsilonr 3.38822720212;
sigma 0.14;
}
}
// Optional entries
nCorr 1;
writeDerivedFields true;
// Inherited entries
region region0;
enabled true;
log true;
timeStart 0;
timeEnd 100;
executeControl timeStep;
executeInterval 1;
writeControl outputTime;
writeInterval -1;
}
// ************************************************************************* //

93
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/blockMeshDict Normal file
View File

@ -0,0 +1,93 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
scale 0.001;
vertices
(
( -1000 -500 -500 )
( 1000 -500 -500 )
( 1000 500 -500 )
( -1000 500 -500 )
( -1000 -500 500 )
( 1000 -500 500 )
( 1000 500 500 )
( -1000 500 500 )
);
blocks
(
hex (0 1 2 3 4 5 6 7) ( 40 15 15 ) simpleGrading ( 1 1 1 )
);
edges
(
);
boundary
(
side-01
{
type patch;
faces
(
(0 4 7 3)
);
}
side-02
{
type patch;
faces
(
(1 2 6 5)
);
}
side-03
{
type patch;
faces
(
(0 1 5 4)
);
}
side-04
{
type patch;
faces
(
(3 7 6 2)
);
}
side-05
{
type patch;
faces
(
(0 3 2 1)
);
}
side-06
{
type patch;
faces
(
(4 5 6 7)
);
}
);
// ************************************************************************* //

68
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/controlDict Normal file
View File

@ -0,0 +1,68 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application interFoam;
startFrom latestTime;
startTime 0;
stopAt endTime;
endTime 20;
deltaT 0.001;
writeControl adjustableRunTime;
writeInterval 0.5;
purgeWrite 0;
writeFormat ascii;
writePrecision 12;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
adjustTimeStep yes;
maxCo 10;
maxAlphaCo 20;
maxDeltaT 0.05;
functions
{
#include "FOelectricPotential"
fieldMinMax1
{
type fieldMinMax;
libs (fieldFunctionObjects);
fields ("electricPotential:V");
}
}
// ************************************************************************* //

27
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/decomposeParDict Normal file
View File

@ -0,0 +1,27 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 4;
method hierarchical;
coeffs
{
n (4 1 1);
}
// ************************************************************************* //

60
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/fvSchemes Normal file
View File

@ -0,0 +1,60 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default cellLimited leastSquares 1;
}
divSchemes
{
default Gauss linear;
div(rhoPhi,U) Gauss upwind;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss linear;
div(phi,k) Gauss upwind;
div(phi,omega) Gauss upwind;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear orthogonal;
laplacian(electricPotential:sigma,electricPotential:V) Gauss linear orthogonal;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
wallDist
{
method meshWave;
}
// ************************************************************************* //

118
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/fvSolution Normal file
View File

@ -0,0 +1,118 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"alpha.water.*"
{
nAlphaCorr 2;
nAlphaSubCycles 2;
cAlpha 0.8;
icAlpha 0;
MULESCorr yes;
nLimiterIter 15;
alphaApplyPrevCorr no;
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-10;
relTol 0;
minIter 1;
}
"pcorr.*"
{
solver GAMG;
smoother DIC;
tolerance 1e-3;
relTol 0;
};
p_rgh
{
solver GAMG;
smoother DIC;
tolerance 5e-8;
relTol 0.01;
};
p_rghFinal
{
$p_rgh;
relTol 0;
}
"(U|k|omega)"
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 1;
tolerance 1e-7;
relTol 0.1;
minIter 1;
};
"(U|k|omega)Final"
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 1;
tolerance 1e-7;
relTol 0;
minIter 1;
};
"electricPotential:V"
{
solver PBiCGStab;
preconditioner DIC;
tolerance 1e-12;
relTol 0;
}
}
PIMPLE
{
momentumPredictor no;
nOuterCorrectors 1;
nCorrectors 3;
nNonOrthogonalCorrectors 1;
correctPhi no;
moveMeshOuterCorrectors no;
turbOnFinalIterOnly yes;
pRefCell 0;
pRefValue 0;
}
relaxationFactors
{
equations
{
".*" 1;
"electricPotential:V" 0.5;
}
}
cache
{
grad(U);
}
// ************************************************************************* //

21
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/meshQualityDict Normal file
View File

@ -0,0 +1,21 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object meshQualityDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Include defaults parameters from master dictionary
#includeEtc "caseDicts/meshQualityDict"
// ************************************************************************* //

35
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/setFieldsDict Normal file
View File

@ -0,0 +1,35 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
defaultFieldValues
(
volScalarFieldValue alpha.water 0
);
regions
(
boxToCell
{
box (-1 -1 -1) (-0.3 1 1);
fieldValues
(
volScalarFieldValue alpha.water 1
);
}
);
// ************************************************************************* //

150
tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/snappyHexMeshDict Normal file
View File

@ -0,0 +1,150 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2106 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object snappyHexMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
castellatedMesh true;
snap true;
addLayers false;
geometry
{
metalSheet.stl
{
type triSurfaceMesh;
name metalSheet;
}
};
castellatedMeshControls
{
maxLocalCells 200000000;
maxGlobalCells 300000000;
minRefinementCells 0;
nCellsBetweenLevels 5;
maxLoadUnbalance 0.2;
allowFreeStandingZoneFaces false;
resolveFeatureAngle 1;
features
(
);
refinementSurfaces
{
metalSheet
{
level (3 3);
}
}
refinementRegions
{
metalSheet
{
mode distance;
levels ((0.05 3) (0.1 2));
}
}
locationInMesh ( 0.8 0 0 ) ;
}
snapControls
{
tolerance 1;
implicitFeatureSnap true;
explicitFeatureSnap false;
multiRegionFeatureSnap false;
detectNearSurfacesSnap true;
nSmoothPatch 3;
nSolveIter 30;
nRelaxIter 5;
nFeatureSnapIter 5;
strictRegionSnap true;
}
addLayersControls
{
layers
{
}
relativeSizes true ;
expansionRatio 1.2 ;
firstLayerThickness 0.1 ;
featureAngle 85;
slipFeatureAngle 30;
nGrow 0;
nBufferCellsNoExtrude 0;
minMedianAxisAngle 90;
maxFaceThicknessRatio 0.2;
maxThicknessToMedialRatio 0.3;
minThickness 1e-06;
nLayerIter 50;
nRelaxIter 5;
nSmoothSurfaceNormals 10;
nSmoothNormals 3;
nSmoothThickness 10;
nRelaxedIter 10;
nMedialAxisIter 10;
}
meshQualityControls
{
minVol 1e-13;
minTetQuality 1e-13;
minArea 1e-13;
minTwist 0.05;
minDeterminant 1e-06;
minFaceWeight 0.02;
minVolRatio 0.01;
minTriangleTwist 0.01;
minFlatness 0.5;
maxNonOrtho 60;
maxBoundarySkewness 20;
maxInternalSkewness 4;
maxConcave 80;
nSmoothScale 4;
errorReduction 0.75;
relaxed
{
minVol 1e-15;
minTetQuality 1e-15;
minArea 1e-15;
minTwist 0.001;
minDeterminant 1e-06;
minFaceWeight 1e-06;
minVolRatio 0.01;
minTriangleTwist 0.01;
minFlatness 0.5;
maxNonOrtho 65;
maxBoundarySkewness 20;
maxInternalSkewness 4;
maxConcave 80;
nSmoothScale 4;
errorReduction 0.75;
}
}
mergeTolerance 1e-08;
debug 0;
writeFlags
(
scalarLevels
);
// ************************************************************************* //