zhyang-dev/OpenFOAM-12
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity

plateFilm: New compressibleInterFoam tutorial to demonstrate the VoFSurfaceFilm fvModel

Browse Source 
The film is left to drain down a vertical plate after the liquid drains out.
This commit is contained in:
Henry Weller
2021-03-10 14:24:58 +00:00
parent 252b71f3c6
commit b0a57397a4
26 changed files with 1208 additions and 0 deletions
Download Patch File Download Diff File Expand all files Collapse all files

42
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/0/T Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 300;
boundaryField
{
region0_to_plateRegion_plateFaces
{
type zeroGradient;
}
bottom
{
type zeroGradient;
}
atmosphere
{
type inletOutlet;
inletValue $internalField;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

46
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/0/U Normal file
View File

@ -0,0 +1,46 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ 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
{
region0_to_plateRegion_plateFaces
{
type noSlip;
}
bottom
{
type flowRateOutletVelocity;
volumetricFlowRate 2e-6;
value $internalField;
}
atmosphere
{
type pressureInletOutletVelocity;
value $internalField;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

42
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/0/alpha.liquid.orig Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object alpha.liquid;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
region0_to_plateRegion_plateFaces
{
type zeroGradient;
}
bottom
{
type zeroGradient;
}
atmosphere
{
type inletOutlet;
inletValue $internalField;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

44
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/0/p Normal file
View File

@ -0,0 +1,44 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 1e5;
boundaryField
{
region0_to_plateRegion_plateFaces
{
type calculated;
value $internalField;
}
bottom
{
type calculated;
value $internalField;
}
atmosphere
{
type calculated;
value $internalField;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

45
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/0/p_rgh Normal file
View File

@ -0,0 +1,45 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 1e5;
boundaryField
{
region0_to_plateRegion_plateFaces
{
type fixedFluxPressure;
value $internalField;
}
bottom
{
type fixedFluxPressure;
value $internalField;
}
atmosphere
{
type totalPressure;
p0 $internalField;
rho thermo:rho;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

50
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/0/plateRegion/T.orig Normal file
View File

@ -0,0 +1,50 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0/movingWallRegion";
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 300;
boundaryField
{
plateFaces_top
{
type zeroGradient;
}
bottom
{
type inletOutlet;
inletValue $internalField;
}
atmosphere
{
type inletOutlet;
inletValue $internalField;
}
region0_to_plateRegion_plateFaces
{
type zeroGradient;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

49
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/0/plateRegion/U.orig Normal file
View File

@ -0,0 +1,49 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
location "0/movingWallRegion";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
plateFaces_top
{
type slip;
}
bottom
{
type zeroGradient;
}
atmosphere
{
type fixedValue;
value $internalField;
}
region0_to_plateRegion_plateFaces
{
type noSlip;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

50
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/0/plateRegion/delta.orig Normal file
View File

@ -0,0 +1,50 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0/plateRegion";
object delta;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
plateFaces_top
{
type zeroGradient;
}
bottom
{
type inletOutlet;
inletValue $internalField;
}
atmosphere
{
type inletOutlet;
inletValue $internalField;
}
region0_to_plateRegion_plateFaces
{
type zeroGradient;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

11
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/Allclean Executable file
View File

@ -0,0 +1,11 @@
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial clean functions
. $WM_PROJECT_DIR/bin/tools/CleanFunctions
cleanCase
rm -rf 0/T.*
rm -rf constant/plateRegion
#------------------------------------------------------------------------------

18
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/Allrun Executable file
View File

@ -0,0 +1,18 @@
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
# Get application name
application=$(getApplication)
runApplication blockMesh
runApplication topoSet
runApplication extrudeToRegionMesh -overwrite
runApplication setFields
runApplication $application
#------------------------------------------------------------------------------

25
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/constant/fvModels Normal file
View File

@ -0,0 +1,25 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object fvModels;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
VoFSurfaceFilm
{
type VoFSurfaceFilm;
phase liquid;
}
// ************************************************************************* //

22
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/constant/g Normal file
View File

@ -0,0 +1,22 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ 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);
// ************************************************************************* //

21
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/constant/momentumTransport Normal file
View File

@ -0,0 +1,21 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object momentumTransport;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType laminar;
// ************************************************************************* //

81
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/constant/surfaceFilmProperties Normal file
View File

@ -0,0 +1,81 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object SurfaceFilmProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
surfaceFilmModel thermoSingleLayer;
regionName plateRegion;
thermophysicalProperties
{
type liquid;
liquid liquid;
useReferenceValues yes;
pRef 1e5;
TRef 300;
}
viscosity
{
model liquid;
}
deltaWet 1e-12;
hydrophilic no;
transfer
{
VoFPatchTransfer
{
deltaFactorToVoF 1.5;
alphaToVoF 0.9;
deltaFactorToFilm 0.9;
alphaToFilm 0.86;
transferRateCoeff 0.1;
}
}
momentumTransport
{
model laminar;
Cf 0.001;
}
upperSurfaceModels
{
heatTransfer
{
model constant;
c0 1;
}
}
lowerSurfaceModels
{
heatTransfer
{
model constant;
c0 1;
}
}
// ************************************************************************* //

24
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/constant/thermophysicalProperties Normal file
View File

@ -0,0 +1,24 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
phases (liquid air);
pMin 10000;
sigma 0.0309;
// ************************************************************************* //

52
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/constant/thermophysicalProperties.air Normal file
View File

@ -0,0 +1,52 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type heRhoThermo;
mixture pureMixture;
transport const;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleInternalEnergy;
}
mixture
{
specie
{
molWeight 28.9;
}
equationOfState
{
rho 1.2;
}
thermodynamics
{
Cp 1007;
Hf 0;
}
transport
{
mu 1.84e-05;
Pr 0.7;
}
}
// ************************************************************************* //

59
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/constant/thermophysicalProperties.liquid Normal file
View File

@ -0,0 +1,59 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type heRhoThermo;
mixture pureMixture;
properties liquid;
energy sensibleInternalEnergy;
}
"(mixture|liquids)"
{
liquid
{
type H2O;
// Set Cp constant and the corresponding linear function for h
// for compatibility with the current hard-coded thermodynamics model
// in surfaceFilm
Cp
{
a 4200;
b 0;
c 0;
d 0;
e 0;
f 0;
}
h
{
a -1252230; // -Cp*TRef where TRef = 298.15
b 4200;
c 0;
d 0;
e 0;
f 0;
}
}
}
// ************************************************************************* //

110
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/system/blockMeshDict Normal file
View File

@ -0,0 +1,110 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.001;
w 50;
h 100;
wCells 80;
hCells 80;
wGrading
(
(0.1 1 1)
(0.9 2.25 10)
);
vertices
(
(0 0 -1)
($w 0 -1)
(0 $h -1)
($w $h -1)
(0 0 0)
($w 0 0)
(0 $h 0)
($w $h 0)
);
blocks
(
hex (0 1 3 2 4 5 7 6)
($wCells $hCells 1)
simpleGrading ($wGrading 1 1)
);
boundary
(
plate
{
type wall;
faces
(
(0 2 6 4)
);
}
vessel
{
type symmetryPlane;
faces
(
(1 3 7 5)
);
}
bottom
{
type patch;
faces
(
(0 1 5 4)
);
}
atmosphere
{
type patch;
faces
(
(2 3 7 6)
);
}
back
{
type empty;
faces
(
(0 2 3 1)
);
}
front
{
type empty;
faces
(
(4 5 7 6)
);
}
);
// ************************************************************************* //

56
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/system/controlDict Normal file
View File

@ -0,0 +1,56 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application compressibleInterFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 5;
deltaT 1e-3;
writeControl adjustableRunTime;
writeInterval 0.1;
purgeWrite 0;
writeFormat ascii;
writePrecision 10;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
adjustTimeStep no;
maxCo 1;
maxAlphaCo 1;
maxDeltaT 1;
// ************************************************************************* //

39
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/system/extrudeToRegionMeshDict Normal file
View File

@ -0,0 +1,39 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object extrudeToRegionMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
region plateRegion;
faceZones (plateFaces);
oneD false;
sampleMode nearestPatchFace;
extrudeModel linearNormal;
nLayers 1;
expansionRatio 1;
adaptMesh yes;
linearNormalCoeffs
{
thickness 0.001;
}
// ************************************************************************* //

57
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/system/fvSchemes Normal file
View File

@ -0,0 +1,57 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ 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 linearUpwindV grad(U);
div(rhoPhi,T) Gauss linearUpwind grad(T);
div(phi,alpha) Gauss interfaceCompression vanLeer 1;
div(phi,p) Gauss upwind;
div(rhoPhi,K) Gauss upwind;
div(((thermo:rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
// ************************************************************************* //

90
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/system/fvSolution Normal file
View File

@ -0,0 +1,90 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"alpha.liquid.*"
{
nAlphaCorr 2;
nAlphaSubCycles 1;
MULESCorr yes;
nLimiterIter 5;
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-8;
relTol 0;
}
"pcorr.*"
{
solver PCG;
preconditioner DIC;
tolerance 1e-5;
relTol 0;
}
p_rgh
{
solver PCG;
preconditioner DIC;
tolerance 1e-9;
relTol 0.05;
}
p_rghFinal
{
$p_rgh;
relTol 0;
}
"U.*"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-6;
relTol 0;
}
"(T|k|B|nuTilda|sigma).*"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-8;
relTol 0;
}
}
PIMPLE
{
momentumPredictor no;
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
}
relaxationFactors
{
equations
{
".*" 1;
}
}
// ************************************************************************* //

49
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/system/plateRegion/fvSchemes Normal file
View File

@ -0,0 +1,49 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system/plateRegion";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
default none;
div(phid,alpha) Gauss upwind;
div(phi,U) Gauss upwind;
div(phi,h) Gauss upwind;
}
laplacianSchemes
{
default Gauss linear uncorrected;
}
snGradSchemes
{
default uncorrected;
}
// ************************************************************************* //

46
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/system/plateRegion/fvSolution Normal file
View File

@ -0,0 +1,46 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system/wallFilmRegion";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"(U|h|alpha).*"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-10;
relTol 0;
}
}
PIMPLE
{
momentumPredictor yes;
nOuterCorrectors 2;
nCorrectors 1;
nNonOrthogonalCorrectors 0;
}
relaxationFactors
{
equations
{
".*" 1;
}
}
// ************************************************************************* //

36
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/system/setFieldsDict Normal file
View File

@ -0,0 +1,36 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
defaultFieldValues
(
volScalarFieldValue alpha.liquid 0
);
regions
(
boxToCell
{
box (0 0 -1) (1 0.08 1);
fieldValues
(
volScalarFieldValue alpha.liquid 1
);
}
);
// ************************************************************************* //

44
tutorials/multiphase/compressibleInterFoam/laminar/plateFilm/system/topoSetDict Normal file
View File

@ -0,0 +1,44 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name plateFaceSet;
type faceSet;
action new;
source patchToFace;
sourceInfo
{
name plate;
}
}
{
name plateFaces;
type faceZoneSet;
action new;
source setToFaceZone;
sourceInfo
{
faceSet plateFaceSet;
}
}
);
// ************************************************************************* //