Skip to content
Snippets Groups Projects
Commit 7f2907f6 authored by Andrew Heather's avatar Andrew Heather
Browse files

ENH: Added tutorials to show extraction of particle data from eulerian cases... 

ENH: Added tutorials to show extraction of particle data from eulerian cases and subsequent injjection via lagrangian cases
parent 7af521e0
Branches
Tags
No related merge requests found
Hide whitespace changes
Inline Side-by-side
Showing
with 780 additions and 0 deletions
tutorials/multiphase/interFoam/laminar/vofToLagrangian/Allrun 0 → 100755
+ 9
− 0
View file @ 7f2907f6
#!/bin/sh
cd ${0%/*} || exit 1 # run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
(cd eulerianInjection && ./Allrun)
(cd lagrangianParticleInjection && ./Allrun)
(cd lagrangianDistributionInjection && ./Allrun)
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/0.orig/U 0 → 100644
+ 42
− 0
View file @ 7f2907f6
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: plus-develop |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format binary;
class volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
top
{
type fixedValue;
value $internalField;
}
bottom
{
type fixedValue;
value $internalField;
}
sides
{
type pressureInletOutletVelocity;
value $internalField;
}
}
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/0.orig/alpha.water 0 → 100644
+ 42
− 0
View file @ 7f2907f6
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: plus-develop |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format binary;
class volScalarField;
location "0";
object alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
top
{
type fixedValue;
value uniform 0;
}
bottom
{
type zeroGradient;
}
sides
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
}
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/0.orig/p_rgh 0 → 100644
+ 44
− 0
View file @ 7f2907f6
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: plus-develop |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format binary;
class volScalarField;
location "0";
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
top
{
type fixedFluxPressure;
gradient uniform 0;
value uniform 0;
}
bottom
{
type fixedFluxPressure;
gradient uniform 0;
value uniform 0;
}
sides
{
type fixedValue;
value uniform 0;
}
}
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/Allclean 0 → 100755
+ 10
− 0
View file @ 7f2907f6
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial clean functions
. $WM_PROJECT_DIR/bin/tools/CleanFunctions
cleanCase
\rm -rf 0
#------------------------------------------------------------------------------
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/Allrun 0 → 100755
+ 20
− 0
View file @ 7f2907f6
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
runApplication blockMesh
runApplication -s createBlockage topoSet -dict system/topoSetDict.createBlockage
runApplication subsetMesh -overwrite blockage -patch bottom
runApplication -s createPatch topoSet -dict system/topoSetDict.createPatch
runApplication -s createCollector topoSet -dict system/topoSetDict.createCollector
restore0Dir
runApplication decomposePar
runParallel setFields
runParallel $(getApplication)
#------------------------------------------------------------------------------
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/constant/g 0 → 100644
+ 22
− 0
View file @ 7f2907f6
/*--------------------------------*- 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 uniformDimensionedVectorField;
location "constant";
object g;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -2 0 0 0 0];
value (0 -9.81 0);
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/constant/transportProperties 0 → 100644
+ 37
− 0
View file @ 7f2907f6
/*--------------------------------*- 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 transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
phases (water air);
water
{
transportModel Newtonian;
nu [0 2 -1 0 0 0 0] 1e-06;
rho [1 -3 0 0 0 0 0] 1000;
}
air
{
transportModel Newtonian;
nu [0 2 -1 0 0 0 0] 1.48e-05;
rho [1 -3 0 0 0 0 0] 1;
}
sigma [1 0 -2 0 0 0 0] 0.07;
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/constant/turbulenceProperties 0 → 100644
+ 21
− 0
View file @ 7f2907f6
/*--------------------------------*- 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;
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/system/blockMeshDict 0 → 100644
+ 75
− 0
View file @ 7f2907f6
/*--------------------------------*- 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;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.05;
vertices
(
(0 0 0)
(1 0 0)
(1 1 0)
(0 1 0)
(0 0 1)
(1 0 1)
(1 1 1)
(0 1 1)
);
blocks
(
hex (0 1 2 3 4 5 6 7) (75 75 75) simpleGrading (1 1 1)
);
edges
(
);
boundary
(
top
{
type patch;
faces
(
(3 7 6 2)
);
}
bottom
{
type wall;
faces
(
(1 5 4 0)
);
}
sides
{
type patch;
faces
(
(0 4 7 3)
(2 6 5 1)
(0 3 2 1)
(4 5 6 7)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/system/controlDict 0 → 100644
+ 70
− 0
View file @ 7f2907f6
/*--------------------------------*- 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 "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application interFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 0.2;
deltaT 1e-4;
writeControl adjustableRunTime;
writeInterval 0.001;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression uncompressed;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
adjustTimeStep yes;
maxCo 0.5;
maxAlphaCo 1;
maxDeltaT 1;
functions
{
extractEulerianParticles1
{
type extractEulerianParticles;
libs ("libfieldFunctionObjects.so");
writeControl writeTime;
faceZone collector;
alpha alpha.water;
nLocations 20;
}
}
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/system/decomposeParDict 0 → 100644
+ 30
− 0
View file @ 7f2907f6
/*--------------------------------*- 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;
note "mesh decomposition control dictionary";
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 4;
method simple;
simpleCoeffs
{
n (2 1 2);
delta 0.001;
}
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/system/fvSchemes 0 → 100644
+ 52
− 0
View file @ 7f2907f6
/*--------------------------------*- 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 "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
div(rhoPhi,U) Gauss limitedLinear 0.2;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss linear;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear orthogonal;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default orthogonal;
}
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/system/fvSolution 0 → 100644
+ 67
− 0
View file @ 7f2907f6
/*--------------------------------*- 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 "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
alpha.water
{
nAlphaCorr 1;
nAlphaSubCycles 5;
cAlpha 2;
}
pcorr
{
solver GAMG;
smoother GaussSeidel;
tolerance 1e-10;
relTol 0;
}
p_rgh
{
solver GAMG;
smoother GaussSeidel;
tolerance 1e-07;
relTol 0.05;
}
p_rghFinal
{
$p_rgh;
tolerance 1e-07;
relTol 0;
}
U
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-06;
relTol 0;
}
}
PIMPLE
{
momentumPredictor no;
nCorrectors 3;
nNonOrthogonalCorrectors 0;
}
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/system/setFieldsDict 0 → 100644
+ 38
− 0
View file @ 7f2907f6
/*--------------------------------*- 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 "system";
object setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
defaultFieldValues
(
volScalarFieldValue alpha.water 0
);
regions
(
faceToFace
{
set injectorFaces;
fieldValues
(
volScalarFieldValue alpha.water 1
volVectorFieldValue U (0 -15 0)
);
}
);
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/system/topoSetDict.createBlockage 0 → 100644
+ 42
− 0
View file @ 7f2907f6
/*--------------------------------*- 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;
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
// Create blockage cellSet
{
name blockage;
type cellSet;
action new;
// source boxToCell;
source cylinderToCell;
sourceInfo
{
// box (0.015 0.010 0.015) (0.035 0.015 0.035);
p1 (0.025 0.02 0.025);
p2 (0.025 0.022 0.025);
radius 0.01;
}
}
{
name blockage;
type cellSet;
action invert;
}
);
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/system/topoSetDict.createCollector 0 → 100644
+ 43
− 0
View file @ 7f2907f6
/*--------------------------------*- 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;
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
// Get all faces in cellSet
{
name f0;
type faceSet;
action new;
source patchToFace;
sourceInfo
{
name sides;
}
}
{
name collector;
type faceZoneSet;
action new;
source setToFaceZone;
sourceInfo
{
faceSet f0;
}
}
);
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/eulerianInjection/system/topoSetDict.createPatch 0 → 100644
+ 58
− 0
View file @ 7f2907f6
/*--------------------------------*- 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;
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
// Load initial cellSet
{
name c0;
type cellSet;
action new;
source cylinderToCell;
sourceInfo
{
p1 (0.025 1 0.025);
p2 (0.025 0.049 0.025);
radius 0.0015;
}
}
// Get all faces in cellSet and assign to injectorFaces
{
name injectorFaces;
type faceSet;
action new;
source cellToFace;
sourceInfo
{
set c0;
option all;
}
}
// Keep in injectorFaces all faces in boundary faces
{
name injectorFaces;
type faceSet;
action subset;
source boundaryToFace;
sourceInfo
{
}
}
);
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/lagrangianDistributionInjection/0.orig/N2 0 → 100644
+ 29
− 0
View file @ 7f2907f6
/*--------------------------------*- 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 volScalarField;
object N2;
}
// ************************************************************************* //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0.766;
boundaryField
{
walls
{
type zeroGradient;
}
}
// ************************************************************************* //
tutorials/multiphase/interFoam/laminar/vofToLagrangian/lagrangianDistributionInjection/0.orig/O2 0 → 100644
+ 29
− 0
View file @ 7f2907f6
/*--------------------------------*- 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 volScalarField;
object O2;
}
// ************************************************************************* //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0.234;
boundaryField
{
walls
{
type zeroGradient;
}
}
// ************************************************************************* //
0% or .
You are about to add 0 people to the discussion. Proceed with caution.
Finish editing this message first!
Please register or to comment