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

New modular solver framework for single- and multi-region simulations

Browse Source 
in which different solver modules can be selected in each region to for complex
conjugate heat-transfer and other combined physics problems such as FSI
(fluid-structure interaction).

For single-region simulations the solver module is selected, instantiated and
executed in the PIMPLE loop in the new foamRun application.

For multi-region simulations the set of solver modules, one for each region, are
selected, instantiated and executed in the multi-region PIMPLE loop of new the
foamMultiRun application.

This provides a very general, flexible and extensible framework for complex
coupled problems by creating more solver modules, either by converting existing
solver applications or creating new ones.

The current set of solver modules provided are:

isothermalFluid
    Solver module for steady or transient turbulent flow of compressible
    isothermal fluids with optional mesh motion and mesh topology changes.

    Created from the rhoSimpleFoam, rhoPimpleFoam and buoyantFoam solvers but
    without the energy equation, hence isothermal.  The buoyant pressure
    formulation corresponding to the buoyantFoam solver is selected
    automatically by the presence of the p_rgh pressure field in the start-time
    directory.

fluid
    Solver module for steady or transient turbulent flow of compressible fluids
    with heat-transfer for HVAC and similar applications, with optional
    mesh motion and mesh topology changes.

    Derived from the isothermalFluid solver module with the addition of the
    energy equation from the rhoSimpleFoam, rhoPimpleFoam and buoyantFoam
    solvers, thus providing the equivalent functionality of these three solvers.

multicomponentFluid
    Solver module for steady or transient turbulent flow of compressible
    reacting fluids with optional mesh motion and mesh topology changes.

    Derived from the isothermalFluid solver module with the addition of
    multicomponent thermophysical properties energy and specie mass-fraction
    equations from the reactingFoam solver, thus providing the equivalent
    functionality in reactingFoam and buoyantReactingFoam.  Chemical reactions
    and/or combustion modelling may be optionally selected to simulate reacting
    systems including fires, explosions etc.

solid
    Solver module for turbulent flow of compressible fluids for conjugate heat
    transfer, HVAC and similar applications, with optional mesh motion and mesh
    topology changes.

    The solid solver module may be selected in solid regions of a CHT case, with
    either the fluid or multicomponentFluid solver module in the fluid regions
    and executed with foamMultiRun to provide functionality equivalent
    chtMultiRegionFoam but in a flexible and extensible framework for future
    extension to more complex coupled problems.

All the usual fvModels, fvConstraints, functionObjects etc. are available with
these solver modules to support simulations including body-forces, local sources,
Lagrangian clouds, liquid films etc. etc.

Converting compressibleInterFoam and multiphaseEulerFoam into solver modules
would provide a significant enhancement to the CHT capability and incompressible
solvers like pimpleFoam run in conjunction with solidDisplacementFoam in
foamMultiRun would be useful for a range of FSI problems.  Many other
combinations of existing solvers converted into solver modules could prove
useful for a very wide range of complex combined physics simulations.

All tutorials from the rhoSimpleFoam, rhoPimpleFoam, buoyantFoam, reactingFoam,
buoyantReactingFoam and chtMultiRegionFoam solver applications replaced by
solver modules have been updated and moved into the tutorials/modules directory:

modules
├── CHT
│   ├── coolingCylinder2D
│   ├── coolingSphere
│   ├── heatedDuct
│   ├── heatExchanger
│   ├── reverseBurner
│   └── shellAndTubeHeatExchanger
├── fluid
│   ├── aerofoilNACA0012
│   ├── aerofoilNACA0012Steady
│   ├── angledDuct
│   ├── angledDuctExplicitFixedCoeff
│   ├── angledDuctLTS
│   ├── annularThermalMixer
│   ├── BernardCells
│   ├── blockedChannel
│   ├── buoyantCavity
│   ├── cavity
│   ├── circuitBoardCooling
│   ├── decompressionTank
│   ├── externalCoupledCavity
│   ├── forwardStep
│   ├── helmholtzResonance
│   ├── hotRadiationRoom
│   ├── hotRadiationRoomFvDOM
│   ├── hotRoom
│   ├── hotRoomBoussinesq
│   ├── hotRoomBoussinesqSteady
│   ├── hotRoomComfort
│   ├── iglooWithFridges
│   ├── mixerVessel2DMRF
│   ├── nacaAirfoil
│   ├── pitzDaily
│   ├── prism
│   ├── shockTube
│   ├── squareBend
│   ├── squareBendLiq
│   └── squareBendLiqSteady
└── multicomponentFluid
    ├── aachenBomb
    ├── counterFlowFlame2D
    ├── counterFlowFlame2D_GRI
    ├── counterFlowFlame2D_GRI_TDAC
    ├── counterFlowFlame2DLTS
    ├── counterFlowFlame2DLTS_GRI_TDAC
    ├── cylinder
    ├── DLR_A_LTS
    ├── filter
    ├── hotBoxes
    ├── membrane
    ├── parcelInBox
    ├── rivuletPanel
    ├── SandiaD_LTS
    ├── simplifiedSiwek
    ├── smallPoolFire2D
    ├── smallPoolFire3D
    ├── splashPanel
    ├── verticalChannel
    ├── verticalChannelLTS
    └── verticalChannelSteady

Also redirection scripts are provided for the replaced solvers which call
foamRun -solver <solver module name> or foamMultiRun in the case of
chtMultiRegionFoam for backward-compatibility.

Documentation for foamRun and foamMultiRun:

Application
    foamRun

Description
    Loads and executes an OpenFOAM solver module either specified by the
    optional \c solver entry in the \c controlDict or as a command-line
    argument.

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

Usage
    \b foamRun [OPTION]

      - \par -solver <name>
        Solver name

      - \par -libs '(\"lib1.so\" ... \"libN.so\")'
        Specify the additional libraries loaded

    Example usage:
      - To run a \c rhoPimpleFoam case by specifying the solver on the
        command line:
        \verbatim
            foamRun -solver fluid
        \endverbatim

      - To update and run a \c rhoPimpleFoam case add the following entries to
        the controlDict:
        \verbatim
            application     foamRun;

            solver          fluid;
        \endverbatim
        then execute \c foamRun

Application
    foamMultiRun

Description
    Loads and executes an OpenFOAM solver modules for each region of a
    multiregion simulation e.g. for conjugate heat transfer.

    The region solvers are specified in the \c regionSolvers dictionary entry in
    \c controlDict, containing a list of pairs of region and solver names,
    e.g. for a two region case with one fluid region named
    liquid and one solid region named tubeWall:
    \verbatim
        regionSolvers
        {
            liquid          fluid;
            tubeWall        solid;
        }
    \endverbatim

    The \c regionSolvers entry is a dictionary to support name substitutions to
    simplify the specification of a single solver type for a set of
    regions, e.g.
    \verbatim
        fluidSolver     fluid;
        solidSolver     solid;

        regionSolvers
        {
            tube1             $fluidSolver;
            tubeWall1         solid;
            tube2             $fluidSolver;
            tubeWall2         solid;
            tube3             $fluidSolver;
            tubeWall3         solid;
        }
    \endverbatim

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

Usage
    \b foamMultiRun [OPTION]

      - \par -libs '(\"lib1.so\" ... \"libN.so\")'
        Specify the additional libraries loaded

    Example usage:
      - To update and run a \c chtMultiRegion case add the following entries to
        the controlDict:
        \verbatim
            application     foamMultiRun;

            regionSolvers
            {
                fluid           fluid;
                solid           solid;
            }
        \endverbatim
        then execute \c foamMultiRun
This commit is contained in:
Henry Weller
2022-08-04 21:11:35 +01:00
parent 7e2dd6dda2
commit 968e60148a
1540 changed files with 5034 additions and 5070 deletions
Download Patch File Download Diff File Expand all files Collapse all files

53
tutorials/modules/multicomponentFluid/verticalChannelSteady/0/H2O Normal file
View File

@ -0,0 +1,53 @@
/*--------------------------------*- 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 volScalarField;
location "0";
object H2O;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0.01;
boundaryField
{
back
{
type symmetryPlane;
}
front
{
type symmetryPlane;
}
walls
{
type zeroGradient;
}
outlet
{
type inletOutlet;
inletValue uniform 0.0;
}
inletSides
{
type fixedValue;
value uniform 0.01;
}
inletCentral
{
type fixedValue;
value uniform 0.01;
}
}
// ************************************************************************* //

53
tutorials/modules/multicomponentFluid/verticalChannelSteady/0/T Normal file
View File

@ -0,0 +1,53 @@
/*--------------------------------*- 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 volScalarField;
location "0";
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 473.0;
boundaryField
{
back
{
type symmetryPlane;
}
front
{
type symmetryPlane;
}
walls
{
type zeroGradient;
}
outlet
{
type inletOutlet;
inletValue uniform 473.0;
}
inletSides
{
type fixedValue;
value uniform 473.0;
}
inletCentral
{
type fixedValue;
value uniform 573.0;
}
}
// ************************************************************************* //

59
tutorials/modules/multicomponentFluid/verticalChannelSteady/0/U.orig 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
{
format ascii;
class volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
back
{
type symmetryPlane;
}
front
{
type symmetryPlane;
}
inletCentral
{
type flowRateInletVelocity;
rhoInlet 1.2;
massFlowRate constant 0.00379;
profile turbulentBL;
value uniform (0 14.68 0);
}
inletSides
{
type flowRateInletVelocity;
rhoInlet 1.2;
massFlowRate constant 0.00832;
profile turbulentBL;
value uniform (0 17.79 0);
}
outlet
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
walls
{
type noSlip;
}
}
// ************************************************************************* //

53
tutorials/modules/multicomponentFluid/verticalChannelSteady/0/air Normal file
View File

@ -0,0 +1,53 @@
/*--------------------------------*- 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 volScalarField;
location "0";
object air;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0.99;
boundaryField
{
back
{
type symmetryPlane;
}
front
{
type symmetryPlane;
}
walls
{
type zeroGradient;
}
outlet
{
type inletOutlet;
inletValue uniform 1.0;
}
inletSides
{
type fixedValue;
value uniform 0.99;
}
inletCentral
{
type fixedValue;
value uniform 0.99;
}
}
// ************************************************************************* //

55
tutorials/modules/multicomponentFluid/verticalChannelSteady/0/alphat Normal file
View File

@ -0,0 +1,55 @@
/*--------------------------------*- 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 volScalarField;
location "0";
object alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
back
{
type symmetryPlane;
}
front
{
type symmetryPlane;
}
inletCentral
{
type calculated;
value uniform 0;
}
inletSides
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
walls
{
type compressible::alphatWallFunction;
Prt 0.85;
value uniform 0;
}
}
// ************************************************************************* //

56
tutorials/modules/multicomponentFluid/verticalChannelSteady/0/k 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
{
format ascii;
class volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 3.75e-9;
boundaryField
{
back
{
type symmetryPlane;
}
front
{
type symmetryPlane;
}
inletCentral
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.05;
value uniform 3.75e-9;
}
inletSides
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.05;
value uniform 3.75e-9;
}
outlet
{
type inletOutlet;
inletValue uniform 3.75e-9;
}
walls
{
type kqRWallFunction;
value uniform 0;
}
}
// ************************************************************************* //

57
tutorials/modules/multicomponentFluid/verticalChannelSteady/0/nut 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
{
format ascii;
class volScalarField;
location "0";
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
back
{
type symmetryPlane;
}
front
{
type symmetryPlane;
}
inletCentral
{
type calculated;
value uniform 0;
}
inletSides
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
walls
{
type nutkWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 0;
}
}
// ************************************************************************* //

61
tutorials/modules/multicomponentFluid/verticalChannelSteady/0/omega Normal file
View File

@ -0,0 +1,61 @@
/*--------------------------------*- 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 volScalarField;
location "0";
object omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 -1 0 0 0 0];
internalField uniform 4.5e-3;
boundaryField
{
back
{
type symmetryPlane;
}
front
{
type symmetryPlane;
}
inletCentral
{
type turbulentMixingLengthFrequencyInlet;
mixingLength 0.007;
k k;
value uniform 4.5e-3;
}
inletSides
{
type turbulentMixingLengthFrequencyInlet;
mixingLength 0.007;
k k;
value uniform 4.5e-3;
}
outlet
{
type inletOutlet;
inletValue uniform 4.5e-3;
}
walls
{
type omegaWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value $internalField;
}
}
// ************************************************************************* //

51
tutorials/modules/multicomponentFluid/verticalChannelSteady/0/p Normal file
View File

@ -0,0 +1,51 @@
/*--------------------------------*- 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 volScalarField;
location "0";
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 100000;
boundaryField
{
back
{
type symmetryPlane;
}
front
{
type symmetryPlane;
}
inletCentral
{
type zeroGradient;
}
inletSides
{
type zeroGradient;
}
outlet
{
type totalPressure;
p0 $internalField;
}
walls
{
type zeroGradient;
}
}
// ************************************************************************* //

18
tutorials/modules/multicomponentFluid/verticalChannelSteady/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
runApplication blockMesh
runApplication potentialFoam
# remove incompatible (volumetric) flux field
rm -f 0/phi
runApplication $(getApplication)
runApplication steadyParticleTracks
#------------------------------------------------------------------------------

197
tutorials/modules/multicomponentFluid/verticalChannelSteady/constant/cloudProperties 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 "constant";
object cloudProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
type reactingMultiphaseCloud;
solution
{
calcFrequency 10;
maxTrackTime 5.0;
maxCo 0.3;
coupled true;
cellValueSourceCorrection off;
sourceTerms
{
resetOnStartup false;
schemes
{
rho semiImplicit 1;
U semiImplicit 1;
Yi semiImplicit 1;
h semiImplicit 1;
radiation semiImplicit 1;
}
}
interpolationSchemes
{
rho cell;
U cellPoint;
thermo:mu cell;
T cell;
Cp cell;
thermo:kappa cell;
p cell;
}
integrationSchemes
{
U Euler;
T analytical;
}
}
constantProperties
{
rho0 1000;
T0 350;
Cp0 4100;
constantVolume false;
}
subModels
{
particleForces
{
sphereDrag;
gravity;
}
injectionModels
{
model1
{
type patchInjection;
massFlowRate 0.8e-03;
parcelBasisType mass;
patchName inletCentral;
parcelsPerSecond 100;
duration 1; // NOTE: set to 1 for steady state
U0 (0 40 0);
flowRateProfile constant 1;
sizeDistribution
{
type general;
generalDistribution
{
distribution
(
(10e-06 0.0025)
(15e-06 0.0528)
(20e-06 0.2795)
(25e-06 1.0918)
(30e-06 2.3988)
(35e-06 4.4227)
(40e-06 6.3888)
(45e-06 8.6721)
(50e-06 10.3153)
(55e-06 11.6259)
(60e-06 12.0030)
(65e-06 10.4175)
(70e-06 10.8427)
(75e-06 8.0016)
(80e-06 6.1333)
(85e-06 3.8827)
(90e-06 3.4688)
);
}
}
}
}
dispersionModel stochasticDispersionRAS;
patchInteractionModel standardWallInteraction;
heatTransferModel RanzMarshall;
compositionModel singleMixtureFraction;
phaseChangeModel liquidEvaporation;
devolatilisationModel none;
surfaceReactionModel none;
stochasticCollisionModel none;
surfaceFilmModel none;
radiation off;
standardWallInteractionCoeffs
{
type rebound;
}
RanzMarshallCoeffs
{
BirdCorrection off;
}
singleMixtureFractionCoeffs
{
phases
(
gas
{
}
liquid
{
H2O 1;
}
solid
{
}
);
YGasTot0 0;
YLiquidTot0 1;
YSolidTot0 0;
}
liquidEvaporationCoeffs
{
enthalpyTransfer enthalpyDifference;
activeLiquids ( H2O );
}
}
cloudFunctions
{
patchPostProcessing1
{
type patchPostProcessing;
maxStoredParcels 100;
patches ( outlet );
}
particleTracks1
{
type particleTracks;
trackInterval 5;
maxSamples 1000000;
resetOnWrite yes;
}
}
// ************************************************************************* //

19
tutorials/modules/multicomponentFluid/verticalChannelSteady/constant/combustionProperties Normal file
View File

@ -0,0 +1,19 @@
/*--------------------------------*- 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 "constant";
object combustionProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
combustionModel none;
// ************************************************************************* //

24
tutorials/modules/multicomponentFluid/verticalChannelSteady/constant/fvConstraints 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
{
format ascii;
class dictionary;
object fvConstraints;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
limitp
{
type limitPressure;
minFactor 0.1;
maxFactor 1.5;
}
// ************************************************************************* //

28
tutorials/modules/multicomponentFluid/verticalChannelSteady/constant/fvModels Normal file
View File

@ -0,0 +1,28 @@
/*--------------------------------*- 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 "constant";
object fvModels;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
buoyancyForce
{
type buoyancyForce;
}
clouds
{
type clouds;
libs ("liblagrangianParcel.so" "liblagrangianParcelTurbulence.so");
}
// ************************************************************************* //

21
tutorials/modules/multicomponentFluid/verticalChannelSteady/constant/g 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
{
format ascii;
class uniformDimensionedVectorField;
location "constant";
object g;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -2 0 0 0 0];
value (0 -9.81 0);
// ************************************************************************* //

28
tutorials/modules/multicomponentFluid/verticalChannelSteady/constant/momentumTransport Normal file
View File

@ -0,0 +1,28 @@
/*--------------------------------*- 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 momentumTransport;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RAS;
RAS
{
model kOmegaSST; // kEpsilon;
turbulence on;
printCoeffs on;
}
// ************************************************************************* //

41
tutorials/modules/multicomponentFluid/verticalChannelSteady/constant/physicalProperties Normal file
View File

@ -0,0 +1,41 @@
/*--------------------------------*- 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 "constant";
object physicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type heRhoThermo;
mixture multicomponentMixture;
transport sutherland;
thermo janaf;
energy sensibleEnthalpy;
equationOfState perfectGas;
specie specie;
}
#include "speciesThermo"
defaultSpecie air;
liquids
{
H2O;
}
solids
{}
// ************************************************************************* //

58
tutorials/modules/multicomponentFluid/verticalChannelSteady/constant/speciesThermo Normal file
View File

@ -0,0 +1,58 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
species
(
air
H2O
);
air
{
specie
{
nMoles 1;
molWeight 28.9596;
}
thermodynamics
{
Tlow 200;
Thigh 3500;
Tcommon 1000;
highCpCoeffs ( 3.57304 -7.24383e-04 1.67022e-06 -1.26501e-10 -4.20580e-13 -1047.41 3.12431 );
lowCpCoeffs ( 3.09589 1.22835e-03 -4.14267e-07 6.56910e-11 -3.87021e-15 -983.191 5.34161 );
}
transport
{
As 1.67212e-06;
Ts 170.672;
}
}
H2O
{
specie
{
molWeight 18.0153;
}
thermodynamics
{
Tlow 200;
Thigh 5000;
Tcommon 1000;
highCpCoeffs ( 2.67215 0.00305629 -8.73026e-07 1.201e-10 -6.39162e-15 -29899.2 6.86282 );
lowCpCoeffs ( 3.38684 0.00347498 -6.3547e-06 6.96858e-09 -2.50659e-12 -30208.1 2.59023 );
}
transport
{
As 1.67212e-06;
Ts 170.672;
}
}
// ************************************************************************* //

217
tutorials/modules/multicomponentFluid/verticalChannelSteady/system/blockMeshDict Normal file
View File

@ -0,0 +1,217 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
note "Created Wed Jul 1 19:20:21 2009. Blocks = 8, cells = 9340, vertices = 36";
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.001;
vertices
(
// front vertices
( 0.00000e+00 -2.30000e+02 2.50000e+01) // v0 0
( 0.00000e+00 -3.00000e+01 2.50000e+01) // v1 1
( 0.00000e+00 0.00000e+00 2.50000e+01) // v2 2
( 0.00000e+00 1.05000e+03 2.50000e+01) // v3 3
( 9.00000e+00 1.05000e+03 2.50000e+01) // v4 4
( 1.60000e+01 1.05000e+03 2.50000e+01) // v5 5
( 2.50000e+01 1.05000e+03 2.50000e+01) // v6 6
( 2.50000e+01 0.00000e+00 2.50000e+01) // v7 7
( 2.50000e+01 -3.00000e+01 2.50000e+01) // v8 8
( 2.50000e+01 -2.30000e+02 2.50000e+01) // v9 9
( 1.80000e+01 -2.30000e+02 2.50000e+01) // v10 10
( 1.80000e+01 -3.00000e+01 2.50000e+01) // v11 11
( 1.60000e+01 0.00000e+00 2.50000e+01) // v12 12
( 1.60000e+01 -2.30000e+02 2.50000e+01) // v13 13
( 9.00000e+00 -2.30000e+02 2.50000e+01) // v14 14
( 9.00000e+00 0.00000e+00 2.50000e+01) // v15 15
( 7.00000e+00 -3.00000e+01 2.50000e+01) // v16 16
( 7.00000e+00 -2.30000e+02 2.50000e+01) // v17 17
// back vertices
( 0.00000e+00 -2.30000e+02 -2.50000e+01) // v0 18
( 0.00000e+00 -3.00000e+01 -2.50000e+01) // v1 19
( 0.00000e+00 0.00000e+00 -2.50000e+01) // v2 20
( 0.00000e+00 1.05000e+03 -2.50000e+01) // v3 21
( 9.00000e+00 1.05000e+03 -2.50000e+01) // v4 22
( 1.60000e+01 1.05000e+03 -2.50000e+01) // v5 23
( 2.50000e+01 1.05000e+03 -2.50000e+01) // v6 24
( 2.50000e+01 0.00000e+00 -2.50000e+01) // v7 25
( 2.50000e+01 -3.00000e+01 -2.50000e+01) // v8 26
( 2.50000e+01 -2.30000e+02 -2.50000e+01) // v9 27
( 1.80000e+01 -2.30000e+02 -2.50000e+01) // v10 28
( 1.80000e+01 -3.00000e+01 -2.50000e+01) // v11 29
( 1.60000e+01 0.00000e+00 -2.50000e+01) // v12 30
( 1.60000e+01 -2.30000e+02 -2.50000e+01) // v13 31
( 9.00000e+00 -2.30000e+02 -2.50000e+01) // v14 32
( 9.00000e+00 0.00000e+00 -2.50000e+01) // v15 33
( 7.00000e+00 -3.00000e+01 -2.50000e+01) // v16 34
( 7.00000e+00 -2.30000e+02 -2.50000e+01) // v17 35
);
blocks
(
// block 0
hex (0 1 16 17 18 19 34 35)
(67 10 10)
edgeGrading
(
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
)
// block 1
hex (1 2 15 16 19 20 33 34)
(10 10 10)
edgeGrading
(
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
)
// block 2
hex (2 3 4 15 20 21 22 33)
(234 10 10)
edgeGrading
(
4.00000e+00 4.00000e+00 4.00000e+00 4.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
)
// block 3
hex (14 15 12 13 32 33 30 31)
(77 10 10)
edgeGrading
(
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
)
// block 4
hex (15 4 5 12 33 22 23 30)
(234 10 10)
edgeGrading
(
4.00000e+00 4.00000e+00 4.00000e+00 4.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
)
// block 5
hex (10 11 8 9 28 29 26 27)
(67 10 10)
edgeGrading
(
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
)
// block 6
hex (11 12 7 8 29 30 25 26)
(11 10 10)
edgeGrading
(
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
)
// block 7
hex (12 5 6 7 30 23 24 25)
(234 10 10)
edgeGrading
(
4.00000e+00 4.00000e+00 4.00000e+00 4.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
1.00000e+00 1.00000e+00 1.00000e+00 1.00000e+00
)
);
defaultPatch
{
name walls;
type wall;
}
boundary
(
back
{
type symmetryPlane;
faces
(
(0 1 16 17)
(1 2 15 16)
(2 3 4 15)
(14 15 12 13)
(15 4 5 12)
(10 11 8 9)
(11 12 7 8)
(12 5 6 7)
);
}
front
{
type symmetryPlane;
faces
(
(18 19 34 35)
(19 20 33 34)
(20 21 22 33)
(32 33 30 31)
(33 22 23 30)
(28 29 26 27)
(29 30 25 26)
(30 23 24 25)
);
}
inletCentral
{
type patch;
faces
(
(13 14 32 31)
);
}
inletSides
{
type patch;
faces
(
(17 0 18 35)
(9 10 28 27)
);
}
outlet
{
type patch;
faces
(
(3 4 22 21)
(4 5 23 22)
(5 6 24 23)
);
}
);
// ************************************************************************* //

73
tutorials/modules/multicomponentFluid/verticalChannelSteady/system/controlDict Normal file
View File

@ -0,0 +1,73 @@
/*--------------------------------*- 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 multicomponentFluid;
startFrom latestTime;
startTime 0;
stopAt endTime;
endTime 500;
deltaT 1;
writeControl timeStep;
writeInterval 20;
purgeWrite 10;
writeFormat ascii;
writePrecision 10;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
functions
{
surfaceFieldValue1
{
type surfaceFieldValue;
libs ("libfieldFunctionObjects.so");
enabled yes;
writeControl writeTime;
log yes;
writeFields no;
regionType patch;
name outlet;
operation average;
weightField phi;
fields
(
H2O
T
);
}
}
// ************************************************************************* //

62
tutorials/modules/multicomponentFluid/verticalChannelSteady/system/fvSchemes Normal file
View File

@ -0,0 +1,62 @@
/*--------------------------------*- 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 steadyState;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
default none;
div(phi,U) bounded Gauss upwind;
div(phid,p) Gauss upwind;
div(phi,K) bounded Gauss linear;
div(phi,h) bounded Gauss upwind;
div(phi,k) bounded Gauss upwind;
div(phi,epsilon) bounded Gauss upwind;
div(phi,omega) bounded Gauss upwind;
div(phi,Yi_h) Gauss upwind;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear uncorrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default uncorrected;
}
wallDist
{
method meshWave;
}
// ************************************************************************* //

76
tutorials/modules/multicomponentFluid/verticalChannelSteady/system/fvSolution 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 fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"p.*"
{
solver GAMG;
tolerance 0;
relTol 0.05;
smoother DICGaussSeidel;
maxIter 50;
};
Phi
{
$p;
}
"(U|Yi|h|k|omega).*"
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 0;
relTol 0.1;
maxIter 20;
}
}
potentialFlow
{
nNonOrthogonalCorrectors 5;
}
PIMPLE
{
nCorrectors 1;
nNonOrthogonalCorrectors 0;
}
relaxationFactors
{
fields
{
p 0.3;
rho 1;
}
equations
{
U 0.7;
h 0.7;
".*" 0.7;
}
}
// ************************************************************************* //

22
tutorials/modules/multicomponentFluid/verticalChannelSteady/system/steadyParticleTracksDict 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
{
format ascii;
class dictionary;
location "system";
object steadyParticleTracksDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
cloudName cloudTracks;
fields (d U T);
// ************************************************************************* //