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

48
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/CH4 Normal file
View File

@ -0,0 +1,48 @@
/*--------------------------------*- 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 CH4;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
"(outlet|sides)"
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
base
{
type zeroGradient;
}
inlet
{
type fixedValue;
value uniform 1.0;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

55
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/FSDomega 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 FSDomega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
outlet
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
sides
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
base
{
type zeroGradient;
}
inlet
{
type fixedValue;
value uniform 0.0;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

36
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/G 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
{
format ascii;
class volScalarField;
object G;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 0 -3 0 0 0 0];
internalField uniform 0;
boundaryField
{
".*"
{
type MarshakRadiation;
emissivityMode lookup;
emissivity uniform 1.0;
value uniform 0;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

36
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/IDefault 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
{
format ascii;
class volScalarField;
object IDefault;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 0 -3 0 0 0 0];
internalField uniform 0;
boundaryField
{
".*"
{
type greyDiffusiveRadiation;
emissivityMode lookup;
emissivity uniform 1.0;
value uniform 0;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

48
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/N2 Normal file
View File

@ -0,0 +1,48 @@
/*--------------------------------*- 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 N2;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0.76699;
boundaryField
{
"(outlet|sides)"
{
type calculated;
value $internalField;
}
base
{
type calculated;
value $internalField;
}
inlet
{
type calculated;
value $internalField;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

48
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/O2 Normal file
View File

@ -0,0 +1,48 @@
/*--------------------------------*- 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 O2;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0.23301;
boundaryField
{
"(outlet|sides)"
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
base
{
type zeroGradient;
}
inlet
{
type fixedValue;
value uniform 0;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

48
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/T Normal file
View File

@ -0,0 +1,48 @@
/*--------------------------------*- 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 300;
boundaryField
{
"(outlet|sides)"
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
base
{
type zeroGradient;
}
inlet
{
type fixedValue;
value uniform 300;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

49
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/U 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
{
format ascii;
class volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
"(outlet|sides)"
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
base
{
type noSlip;
}
inlet
{
type fixedValue;
value uniform (0 0.05 0);
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

48
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/Ydefault Normal file
View File

@ -0,0 +1,48 @@
/*--------------------------------*- 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 Ydefault;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
"(outlet|sides)"
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
base
{
type zeroGradient;
}
inlet
{
type fixedValue;
value uniform 0;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

45
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/alphat 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
{
format ascii;
class volScalarField;
location "0";
object alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
"(outlet|sides)"
{
type zeroGradient;
}
base
{
type zeroGradient;
}
inlet
{
type zeroGradient;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

55
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/k 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 k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 1e-4;
boundaryField
{
"(outlet|sides)"
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
sides
{
type inletOutlet;
inletValue uniform 1e-4;
value uniform 1e-4;
}
base
{
type zeroGradient;
}
inlet
{
type fixedValue;
value $internalField;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

45
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/nut 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
{
format ascii;
class volScalarField;
location "0";
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
"(outlet|sides)"
{
type zeroGradient;
}
base
{
type zeroGradient;
}
inlet
{
type zeroGradient;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

48
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/p Normal file
View File

@ -0,0 +1,48 @@
/*--------------------------------*- 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 101325;
boundaryField
{
"(outlet|sides)"
{
type calculated;
value $internalField;
}
base
{
type calculated;
value $internalField;
}
inlet
{
type calculated;
value $internalField;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

49
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/p_rgh 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
{
format ascii;
class volScalarField;
location "0";
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
"(outlet|sides)"
{
type prghTotalHydrostaticPressure;
p0 $internalField;
value $internalField;
}
base
{
type fixedFluxPressure;
value $internalField;
}
inlet
{
type fixedFluxPressure;
value $internalField;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

54
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/ph_rgh.orig Normal file
View File

@ -0,0 +1,54 @@
/*--------------------------------*- 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 ph_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
outlet
{
type fixedValue;
value $internalField;
}
sides
{
type fixedFluxPressure;
value $internalField;
}
base
{
type fixedFluxPressure;
value $internalField;
}
inlet
{
type fixedFluxPressure;
value $internalField;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

36
tutorials/modules/multicomponentFluid/smallPoolFire2D/0/soot 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
{
format ascii;
class volScalarField;
location "0";
object soot;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
".*"
{
type calculated;
value $internalField;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //

11
tutorials/modules/multicomponentFluid/smallPoolFire2D/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 -f 0/ph_rgh
#------------------------------------------------------------------------------

13
tutorials/modules/multicomponentFluid/smallPoolFire2D/Allrun Executable file
View File

@ -0,0 +1,13 @@
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
runApplication blockMesh
runApplication topoSet
runApplication createPatch -overwrite
runApplication $(getApplication)
#------------------------------------------------------------------------------

60
tutorials/modules/multicomponentFluid/smallPoolFire2D/constant/combustionProperties Normal file
View File

@ -0,0 +1,60 @@
/*--------------------------------*- 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 infinitelyFastChemistry;
//combustionModel FSD;
infinitelyFastChemistryCoeffs
{
semiImplicit no;
C 5.0;
}
FSDCoeffs
{
Cv 0.1;
ftVarMin 1e-2;
reactionRateFlameArea relaxation;
fuel Methane;
semiImplicit no;
relaxationCoeffs
{
C 2.0;
alpha 1.0;
Methane
{
omega0 0.5;
eta -0.013;
omegaMin 0.01;
sigmaExt 470;
}
Propane
{
omega0 0.4;
eta -0.00656;
omegaMin 0.01;
sigmaExt 450;
}
}
}
#include "reaction"
// ************************************************************************* //

23
tutorials/modules/multicomponentFluid/smallPoolFire2D/constant/fvModels 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;
location "constant";
object fvModels;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
radiation
{
type radiation;
libs ("libradiationModels.so");
}
// ************************************************************************* //

20
tutorials/modules/multicomponentFluid/smallPoolFire2D/constant/g Normal file
View File

@ -0,0 +1,20 @@
/*--------------------------------*- 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 -9.8 0);
// ************************************************************************* //

20
tutorials/modules/multicomponentFluid/smallPoolFire2D/constant/hRef Normal file
View File

@ -0,0 +1,20 @@
/*--------------------------------*- 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 uniformDimensionedScalarField;
location "constant";
object hRef;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 0 0 0 0 0];
value 1;
// ************************************************************************* //

87
tutorials/modules/multicomponentFluid/smallPoolFire2D/constant/momentumTransport Normal file
View File

@ -0,0 +1,87 @@
/*--------------------------------*- 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 momentumTransport;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType LES;
LES
{
model kEqn;
delta cubeRootVol;
turbulence on;
printCoeffs on;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
PrandtlCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
maxDeltaRatio 1.1;
}
Cdelta 0.158;
}
vanDriestCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
maxDeltaRatio 1.1;
}
Aplus 26;
Cdelta 0.158;
}
smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
maxDeltaRatio 1.1;
}
}
// ************************************************************************* //

20
tutorials/modules/multicomponentFluid/smallPoolFire2D/constant/pRef Normal file
View File

@ -0,0 +1,20 @@
/*--------------------------------*- 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 uniformDimensionedScalarField;
location "constant";
object pRef;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
value 101325;
// ************************************************************************* //

34
tutorials/modules/multicomponentFluid/smallPoolFire2D/constant/physicalProperties 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;
location "constant";
object physicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type hePsiThermo;
mixture multicomponentMixture;
transport sutherland;
thermo janaf;
energy sensibleEnthalpy;
equationOfState perfectGas;
specie specie;
}
defaultSpecie N2;
fuel CH4;
#include "thermo.compressibleGas"
// ************************************************************************* //

196
tutorials/modules/multicomponentFluid/smallPoolFire2D/constant/radiationProperties Normal file
View File

@ -0,0 +1,196 @@
/*--------------------------------*- 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 radiationProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
radiation on;
radiationModel fvDOM;
fvDOMCoeffs
{
nPhi 4; // azimuthal angles in PI/2 on X-Y.(from Y to X)
nTheta 0; // polar angles in PI (from Z to X-Y plane)
tolerance 1e-2; // convergence tolerance for radiation iteration
maxIter 4; // maximum number of iterations
}
// Number of flow iterations per radiation iteration
solverFreq 10;
absorptionEmissionModel greyMeanCombustion;
constantCoeffs
{
absorptivity 0.01;
emissivity 0.01;
E 0;
}
greyMeanCombustionCoeffs
{
lookUpTableFileName none;
EhrrCoeff 0.0;
CO2
{
Tcommon 200; // Common Temp
invTemp true; // Is the polynomial using inverse temperature.
Tlow 200; // Low Temp
Thigh 2500; // High Temp
loTcoeffs // coefss for T < Tcommon
(
0 // a0 +
0 // a1*T +
0 // a2*T^(+/-)2 +
0 // a3*T^(+/-)3 +
0 // a4*T^(+/-)4 +
0 // a5*T^(+/-)5 +
);
hiTcoeffs // coefss for T > Tcommon
(
18.741
-121.31e3
273.5e6
-194.05e9
56.31e12
-5.8169e15
);
}
H2O
{
Tcommon 200;
invTemp true;
Tlow 200;
Thigh 2500;
loTcoeffs
(
0
0
0
0
0
0
);
hiTcoeffs
(
-0.23093
-1.12390e3
9.4153e6
-2.99885e9
0.51382e12
-1.868e10
);
}
CH4
{
Tcommon 200;
Tlow 200;
Thigh 2500;
invTemp false;
loTcoeffs
(
0
0
0
0
0
0
);
hiTcoeffs
(
6.6334
-0.0035686
1.6682e-8
2.5611e-10
-2.6558e-14
0
);
}
O2
{
Tcommon 200;
invTemp true;
Tlow 200;
Thigh 2500;
loTcoeffs
(
0
0
0
0
0
0
);
hiTcoeffs
(
0.1
0
0
0
0
0
);
}
N2
{
Tcommon 200;
invTemp true;
Tlow 200;
Thigh 2500;
loTcoeffs
(
0
0
0
0
0
0
);
hiTcoeffs
(
0.1
0
0
0
0
0
);
}
}
scatterModel none;
sootModel mixtureFraction;
mixtureFractionCoeffs
{
// CH4 + 2O2 + 7.5N2 = CO2 + 2H2O + 7.5N2 + nuSoot soot
nuSoot 0.055;
Wsoot 12;
}
// ************************************************************************* //

14
tutorials/modules/multicomponentFluid/smallPoolFire2D/constant/reaction Normal file
View File

@ -0,0 +1,14 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
reaction
{
reaction "CH4 + 2O2 + 7.5N2 = CO2 + 2H2O + 7.5N2";
}
// ************************************************************************* //

124
tutorials/modules/multicomponentFluid/smallPoolFire2D/constant/thermo.compressibleGas Normal file
View File

@ -0,0 +1,124 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
species
(
O2
H2O
CH4
CO2
N2
);
O2
{
specie
{
molWeight 31.9988;
}
thermodynamics
{
Tlow 200;
Thigh 5000;
Tcommon 1000;
highCpCoeffs ( 3.69758 0.00061352 -1.25884e-07 1.77528e-11 -1.13644e-15 -1233.93 3.18917 );
lowCpCoeffs ( 3.21294 0.00112749 -5.75615e-07 1.31388e-09 -8.76855e-13 -1005.25 6.03474 );
}
transport
{
As 1.753e-6;
Ts 139;
}
}
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 2.978e-7;
Ts 1064;
}
}
CH4
{
specie
{
molWeight 16.0428;
}
thermodynamics
{
Tlow 200;
Thigh 6000;
Tcommon 1000;
highCpCoeffs ( 1.63543 0.0100844 -3.36924e-06 5.34973e-10 -3.15528e-14 -10005.6 9.9937 );
lowCpCoeffs ( 5.14988 -0.013671 4.91801e-05 -4.84744e-08 1.66694e-11 -10246.6 -4.64132 );
}
transport
{
As 1.0194e-06;
Ts 171.06;
}
}
CO2
{
specie
{
molWeight 44.01;
}
thermodynamics
{
Tlow 200;
Thigh 5000;
Tcommon 1000;
highCpCoeffs ( 4.45362 0.00314017 -1.27841e-06 2.394e-10 -1.66903e-14 -48967 -0.955396 );
lowCpCoeffs ( 2.27572 0.00992207 -1.04091e-05 6.86669e-09 -2.11728e-12 -48373.1 10.1885 );
}
transport
{
As 1.503e-6;
Ts 222;
}
}
N2
{
specie
{
molWeight 28.0134;
}
thermodynamics
{
Tlow 200;
Thigh 5000;
Tcommon 1000;
highCpCoeffs ( 2.92664 0.00148798 -5.68476e-07 1.0097e-10 -6.75335e-15 -922.798 5.98053 );
lowCpCoeffs ( 3.29868 0.00140824 -3.96322e-06 5.64152e-09 -2.44486e-12 -1020.9 3.95037 );
}
transport
{
As 1.401e-6;
Ts 107;
}
}
// ************************************************************************* //

75
tutorials/modules/multicomponentFluid/smallPoolFire2D/system/blockMeshDict Normal file
View File

@ -0,0 +1,75 @@
/*--------------------------------*- 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;
vertices
(
(-0.5 0 -0.01)
( 0.5 0 -0.01)
( 0.5 1 -0.01)
(-0.5 1 -0.01)
(-0.5 0 0.01)
( 0.5 0 0.01)
( 0.5 1 0.01)
(-0.5 1 0.01)
);
blocks
(
hex (0 1 2 3 4 5 6 7) (150 150 1) simpleGrading (1 1 1)
);
boundary
(
base
{
type patch;
faces
(
(0 1 5 4)
);
}
outlet
{
type patch;
faces
(
(3 2 6 7)
);
}
sides
{
type patch;
faces
(
(1 5 6 2)
(0 4 7 3)
);
}
frontAndBack
{
type empty;
faces
(
(0 1 2 3)
(4 5 6 7)
);
}
);
// ************************************************************************* //

54
tutorials/modules/multicomponentFluid/smallPoolFire2D/system/controlDict Normal file
View File

@ -0,0 +1,54 @@
/*--------------------------------*- 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 controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application foamRun;
solver multicomponentFluid;
startFrom startTime;
startTime 0.0;
stopAt endTime;
endTime 3.0;
deltaT 0.001;
writeControl adjustableRunTime;
writeInterval 0.1;
purgeWrite 0;
writeFormat binary;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
graphFormat raw;
runTimeModifiable yes;
adjustTimeStep yes;
maxCo 0.5;
// ************************************************************************* //

36
tutorials/modules/multicomponentFluid/smallPoolFire2D/system/createPatchDict 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
{
format ascii;
class dictionary;
object createPatchDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
patches
(
{
// Name of new patch
name inlet;
// Dictionary to construct new patch from
patchInfo
{
type patch;
}
// How to construct: either from 'patches' or 'set'
constructFrom set;
// If constructFrom = set : name of faceSet
set f0;
}
);
// ************************************************************************* //

65
tutorials/modules/multicomponentFluid/smallPoolFire2D/system/fvSchemes Normal file
View File

@ -0,0 +1,65 @@
/*--------------------------------*- 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;
}
divSchemes
{
default none;
div(phi,U) Gauss LUST grad(U);
div(U) Gauss linear;
div(phi,K) Gauss linear;
div(phi,k) Gauss limitedLinear 1;
div(phi,FSDomega) Gauss limitedLinear 1;
div(phi,Yi_h) Gauss multivariateSelection
{
O2 limitedLinear01 1;
CH4 limitedLinear01 1;
N2 limitedLinear01 1;
H2O limitedLinear01 1;
CO2 limitedLinear01 1;
h limitedLinear 1;
};
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
div(Ji,Ii_h) Gauss upwind;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
// ************************************************************************* //

113
tutorials/modules/multicomponentFluid/smallPoolFire2D/system/fvSolution Normal file
View File

@ -0,0 +1,113 @@
/*--------------------------------*- 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
{
rho
{
solver PCG;
preconditioner DIC;
tolerance 1e-6;
relTol 0.1;
};
rhoFinal
{
$rho;
tolerance 1e-6;
relTol 0;
};
p_rgh
{
solver GAMG;
tolerance 1e-6;
relTol 0.05;
smoother GaussSeidel;
};
p_rghFinal
{
$p_rgh;
tolerance 1e-6;
relTol 0;
};
ph_rgh
{
$p_rgh;
}
"(U|Yi|k|h|FSDomega)"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-6;
relTol 0.1;
nSweeps 1;
};
"(U|Yi|k|h|FSDomega)Final"
{
$U;
tolerance 1e-6;
relTol 0;
};
"Ii.*"
{
solver GAMG;
tolerance 1e-4;
relTol 0.1;
smoother symGaussSeidel;
maxIter 3;
nPostSweeps 1;
}
"G.*"
{
solver PCG;
preconditioner DIC;
tolerance 1e-04;
relTol 0;
}
}
PIMPLE
{
momentumPredictor yes;
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
hydrostaticInitialisation yes;
nHydrostaticCorrectors 5;
}
relaxationFactors
{
equations
{
"(U|k).*" 1;
"(C3H8|O2|H2O|CO2|h).*" 1;
}
}
// ************************************************************************* //

28
tutorials/modules/multicomponentFluid/smallPoolFire2D/system/topoSetDict 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 topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name f0;
type faceSet;
action new;
source boxToFace;
box (-0.0529 -0.001 -0.1)(0.0529 0.002 0.1);
}
);
// ************************************************************************* //