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

solvers::multiphaseEuler: New solver module for Euler-Euler multiphase simulations

Browse Source 
executed with foamRun for single region simulations of foamMultiRun for
multi-region simulations.  Replaces multiphaseEulerFoam and all the
corresponding tutorials have been updated and moved to
tutorials/modules/multiphaseEuler.

Class
    Foam::solvers::multiphaseEuler

Description
    Solver module for a system of any number of compressible fluid phases with a
    common pressure, but otherwise separate properties. The type of phase model
    is run time selectable and can optionally represent multiple species and
    in-phase reactions. The phase system is also run time selectable and can
    optionally represent different types of momentum, heat and mass transfer.

    Uses the flexible PIMPLE (PISO-SIMPLE) solution for time-resolved and
    pseudo-transient and steady simulations.

    Optional fvModels and fvConstraints are provided to enhance the simulation
    in many ways including adding various sources, Lagrangian
    particles, surface film etc. and constraining or limiting the solution.

SourceFiles
    multiphaseEuler.C

See also
    Foam::solvers::compressibleVoF
    Foam::solvers::fluidSolver
    Foam::solvers::incompressibleFluid
This commit is contained in:
Henry Weller
2022-11-03 14:49:56 +00:00
parent 879f852b80
commit cec0359871
1621 changed files with 127852 additions and 0 deletions
Download Patch File Download Diff File Expand all files Collapse all files

96
tutorials/modules/multiphaseEuler/wallBoilingPolydisperseTwoGroups/system/blockMeshDict Normal file
View File

@ -0,0 +1,96 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
backgroundMesh
{
length 3.5;
rA 0.0096;
lengthCells 350;
rAcells 40;
}
convertToMeters 1;
vertices
(
( 0 0 -1)
($!backgroundMesh/length 0 -1)
( 0 $!backgroundMesh/rA -1)
($!backgroundMesh/length $!backgroundMesh/rA -1)
( 0 0 0)
($!backgroundMesh/length 0 0)
( 0 $!backgroundMesh/rA 0)
($!backgroundMesh/length $!backgroundMesh/rA 0)
);
blocks
(
hex (0 1 3 2 4 5 7 6)
($!backgroundMesh/lengthCells $!backgroundMesh/rAcells 1)
simpleGrading (1 0.5 1)
);
boundary
(
inlet
{
type mappedInternal;
offset (0.05 0 0);
faces
(
(0 4 6 2)
);
}
outlet
{
type patch;
faces
(
(1 5 7 3)
);
}
front
{
type symmetry;
faces
(
(4 5 7 6)
);
}
back
{
type symmetry;
faces
(
(0 1 3 2)
);
}
wall
{
type wall;
faces
(
(3 2 6 7)
(1 0 4 5)
);
}
);
// ************************************************************************* //

197
tutorials/modules/multiphaseEuler/wallBoilingPolydisperseTwoGroups/system/controlDict.orig Normal file
View File

@ -0,0 +1,197 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application foamRun;
solver multiphaseEuler;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 0.5;
deltaT 0.0001;
writeControl adjustableRunTime;
writeInterval 0.5;
purgeWrite 0;
writeFormat ascii;
writePrecision 9;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
adjustTimeStep yes;
maxCo 0.5;
maxDeltaT 0.001;
functions
{
volumeDensity.diameter.bubbles
{
type populationBalanceSizeDistribution;
functionObjectLibs ( "libmultiphaseEulerFoamFunctionObjects.so" );
writeControl runTime;
writeInterval 0.5;
setFormat raw;
log yes;
functionType volumeConcentration;
coordinateType diameter;
regionType cellZone;
name x349;
populationBalance bubbles;
}
volumeDensity_bulk.diameter.bubbles
{
type populationBalanceSizeDistribution;
functionObjectLibs ( "libmultiphaseEulerFoamFunctionObjects.so" );
writeControl runTime;
writeInterval 0.5;
setFormat raw;
log yes;
functionType volumeConcentration;
coordinateType diameter;
regionType cellZone;
name x349_bulk;
populationBalance bubbles;
}
volumeDensity_wall.diameter.bubbles
{
type populationBalanceSizeDistribution;
functionObjectLibs ( "libmultiphaseEulerFoamFunctionObjects.so" );
writeControl runTime;
writeInterval 0.5;
setFormat raw;
log yes;
functionType volumeConcentration;
coordinateType diameter;
regionType cellZone;
name x349_wall;
populationBalance bubbles;
}
outflow
{
type surfaceFieldValue;
functionObjectLibs ( "libfieldFunctionObjects.so" );
log yes;
writeFields false;
regionType patch;
name outlet;
operation sum;
fields ( alphaRhoPhi.gas alphaRhoPhi.gas2 alphaRhoPhi.liquid );
}
inflow
{
type surfaceFieldValue;
functionObjectLibs ( "libfieldFunctionObjects.so" );
log yes;
writeFields false;
regionType patch;
name inlet;
operation sum;
fields ( alphaRhoPhi.gas alphaRhoPhi.gas2 alphaRhoPhi.liquid );
}
outletGas
{
type surfaceFieldValue;
functionObjectLibs ( "libfieldFunctionObjects.so" );
log yes;
writeFields false;
regionType patch;
name outlet;
operation sum;
weightField alphaRhoPhi.gas;
fields ( h.gas );
}
outletGas2
{
type surfaceFieldValue;
functionObjectLibs ( "libfieldFunctionObjects.so" );
log yes;
writeFields false;
regionType patch;
name outlet;
operation sum;
weightField alphaRhoPhi.gas2;
fields ( h.gas2 );
}
outletLiquid
{
type surfaceFieldValue;
functionObjectLibs ( "libfieldFunctionObjects.so" );
log yes;
writeFields false;
regionType patch;
name outlet;
operation sum;
weightField alphaRhoPhi.liquid;
fields ( h.liquid );
}
inletGas
{
type surfaceFieldValue;
functionObjectLibs ( "libfieldFunctionObjects.so" );
log yes;
writeFields false;
regionType patch;
name inlet;
operation sum;
weightField alphaRhoPhi.gas;
fields ( h.gas );
}
inletGas2
{
type surfaceFieldValue;
functionObjectLibs ( "libfieldFunctionObjects.so" );
log yes;
writeFields false;
regionType patch;
name inlet;
operation sum;
weightField alphaRhoPhi.gas2;
fields ( h.gas2 );
}
inletLiquid
{
type surfaceFieldValue;
functionObjectLibs ( "libfieldFunctionObjects.so" );
log yes;
writeFields false;
regionType patch;
name inlet;
operation sum;
weightField alphaRhoPhi.liquid;
fields ( h.liquid );
}
#includeFunc writeObjects(d.gas, d.gas2)
}
// ************************************************************************* //

38
tutorials/modules/multiphaseEuler/wallBoilingPolydisperseTwoGroups/system/decomposeParDict Normal file
View File

@ -0,0 +1,38 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 4;
method scotch;
simpleCoeffs
{
n (1 1 24);
}
hierarchicalCoeffs
{
n (1 1 1);
order xyz;
}
distributed no;
roots
(
);
// ************************************************************************* //

34
tutorials/modules/multiphaseEuler/wallBoilingPolydisperseTwoGroups/system/extrudeMeshDict Normal file
View File

@ -0,0 +1,34 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object extrudeProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
constructFrom patch;
sourceCase "$FOAM_CASE";
sourcePatches (front);
exposedPatchName back;
extrudeModel wedge;
sectorCoeffs
{
axisPt (0 0 0);
axis (1 0 0);
angle 1;
}
flipNormals false;
mergeFaces false;
// ************************************************************************* //

23
tutorials/modules/multiphaseEuler/wallBoilingPolydisperseTwoGroups/system/fvConstraints Normal file
View File

@ -0,0 +1,23 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object fvConstraints;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
limitp
{
type limitPressure;
min 1e4;
}
// ************************************************************************* //

76
tutorials/modules/multiphaseEuler/wallBoilingPolydisperseTwoGroups/system/fvSchemes Normal file
View File

@ -0,0 +1,76 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
limited cellLimited Gauss linear 1;
}
divSchemes
{
default none;
div(phi,alpha) Gauss vanLeer;
div(phir,alpha) Gauss vanLeer;
div(alphaRhoPhi,U) Gauss linearUpwind limited;
div(phi,U) Gauss linearUpwind limited;
div(alphaRhoPhi,Yi) Gauss linearUpwind limited;
"div\(alphaRhoPhi,(h|e)\)" Gauss linearUpwind limited;
"div\(alphaPhi,f.*\)" Gauss linearUpwind limited;
div(alphaRhoPhi,K) Gauss linearUpwind limited;
div(alphaRhoPhi,(p|rho)) Gauss linearUpwind limited;
"div\(alphaRhoPhi,(k|epsilon|omega)\)" Gauss linearUpwind limited;
"div\(phim,(k|epsilon)m\)" Gauss linearUpwind limited;
div((((alpha*rho)*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
fluxRequired
{
default no;
}
wallDist
{
method meshWave;
nRequired yes;
}
// ************************************************************************* //

104
tutorials/modules/multiphaseEuler/wallBoilingPolydisperseTwoGroups/system/fvSolution Normal file
View File

@ -0,0 +1,104 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"alpha.*"
{
nAlphaCorr 1;
nAlphaSubCycles 1;
}
bubbles
{
nCorr 1;
tolerance 1e-4;
scale true;
solveOnFinalIterOnly true;
sourceUpdateInterval 20;
}
p_rgh
{
solver GAMG;
smoother DIC;
tolerance 1e-8;
relTol 0.01;
maxIter 20;
minIter 2;
}
p_rghFinal
{
$p_rgh;
relTol 0;
}
"(e|h).*"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-12;
relTol 0.001;
minIter 1;
maxIter 20;
}
"(k|epsilon|omega).*"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-8;
relTol 0;
minIter 1;
}
"f.*"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-6;
relTol 0;
}
}
PIMPLE
{
nOuterCorrectors 1;
nCorrectors 1;
nNonOrthogonalCorrectors 0;
nEnergyCorrectors 1;
faceMomentum yes;
}
relaxationFactors
{
fields
{
thermalPhaseChange:dmdtf 1.0;
}
equations
{
".*" 1;
"h\..*" 1;
}
}
// ************************************************************************* //

68
tutorials/modules/multiphaseEuler/wallBoilingPolydisperseTwoGroups/system/topoSetDict Normal file
View File

@ -0,0 +1,68 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name x349;
type cellSet;
action new;
source boxToCell;
box (3.48 -0.1 -0.1) (3.5 0.1 0.1);
}
{
name x349;
type cellZoneSet;
action new;
source setToCellZone;
set x349;
}
{
name x349_wall;
type cellSet;
action new;
source boxToCell;
box (3.48 0.0093 -0.1) (3.5 0.1 0.1);
}
{
name x349_wall;
type cellZoneSet;
action new;
source setToCellZone;
set x349_wall;
}
{
name x349_bulk;
type cellSet;
action new;
source boxToCell;
box (3.48 0.0 -0.1) (3.5 0.005 0.1);
}
{
name x349_bulk;
type cellZoneSet;
action new;
source setToCellZone;
set x349_bulk;
}
);
// ************************************************************************* //