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

26
tutorials/modules/CHT/coolingSphere/Allclean Executable file
View File

@ -0,0 +1,26 @@
#!/bin/sh
cd "${0%/*}" || exit 1 # Run from this directory
# Source tutorial clean functions
. "$WM_PROJECT_DIR/bin/tools/CleanFunctions"
removeRegionDirs ()
{
_regionDirs="$(foamDictionary -keywords constant/materialProperties)"
for _d in system constant
do
for _r in $_regionDirs
do
_dir="${_d}/${_r}"
[ -d "$_dir" ] && rm -rf "$_dir"
done
done
}
cleanCase
removeRegionDirs
rm -rf 0
rm -f system/regionSolvers
#------------------------------------------------------------------------------

12
tutorials/modules/CHT/coolingSphere/Allmesh Executable file
View File

@ -0,0 +1,12 @@
#!/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 transformPoints "scale=(0.01 0.01 0.01)"
runApplication splitMeshRegions -cellZones -defaultRegionName fluid -overwrite
#------------------------------------------------------------------------------

23
tutorials/modules/CHT/coolingSphere/Allrun Executable file
View File

@ -0,0 +1,23 @@
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
./Allmesh
runApplication foamSetupCHT
runApplication foamDictionary -entry internalField -set "uniform 348" 0/solid/T
runApplication decomposePar -allRegions
printf "\n%s\n" "Creating files for paraview post-processing"
paraFoam -touchAll
echo
runParallel $(getApplication)
runApplication reconstructPar -allRegions
#------------------------------------------------------------------------------

19
tutorials/modules/CHT/coolingSphere/constant/initialConditions 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;
object initialConditions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Tinitial 296;
pInitial 1e5;
// ************************************************************************* //

28
tutorials/modules/CHT/coolingSphere/constant/materialProperties 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 materialProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
fluid
{
solver fluid;
material air;
}
solid
{
solver solid;
material copper;
}
// ************************************************************************* //

149
tutorials/modules/CHT/coolingSphere/system/blockMeshDict Normal file
View File

@ -0,0 +1,149 @@
/*--------------------------------*- 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
bp 0.4;
bn -0.4;
dp 4;
dn -4;
dl 10;
nb 15;
nd 30;
nl 20;
gd 20;
gl 1;
geometry
{
sphere
{
type searchableSphere;
centre (0 0 0);
radius 0.5;
}
}
convertToMeters 1;
vertices
(
project ($bn $bn $bn) (sphere)
project ($bp $bn $bn) (sphere)
project ($bn $bp $bn) (sphere)
project ($bp $bp $bn) (sphere)
project ($bn $bn $bp) (sphere)
project ($bp $bn $bp) (sphere)
project ($bn $bp $bp) (sphere)
project ($bp $bp $bp) (sphere)
($dn $dn $dn)
($dp $dn $dn)
($dn $dp $dn)
($dp $dp $dn)
($dn $dn $dp)
($dp $dn $dp)
($dn $dp $dp)
($dp $dp $dp)
($dl $dn $dn)
($dl $dp $dn)
($dl $dn $dp)
($dl $dp $dp)
);
blocks
(
hex (1 0 8 9 5 4 12 13) ($nb $nd $nb) simpleGrading (1 $gd 1)
hex (0 2 10 8 4 6 14 12) ($nb $nd $nb) simpleGrading (1 $gd 1)
hex (2 3 11 10 6 7 15 14) ($nb $nd $nb) simpleGrading (1 $gd 1)
hex (3 1 9 11 7 5 13 15) ($nb $nd $nb) simpleGrading (1 $gd 1)
hex (0 1 9 8 2 3 11 10) ($nb $nd $nb) simpleGrading (1 $gd 1)
hex (5 4 12 13 7 6 14 15) ($nb $nd $nb) simpleGrading (1 $gd 1)
hex (9 16 17 11 13 18 19 15) ($nl $nb $nb) simpleGrading (1 1 1)
// Solid region
hex (0 1 3 2 4 5 7 6) ($nb $nb $nb) simpleGrading (1 1 1)
);
edges
(
project 0 2 (sphere)
project 2 3 (sphere)
project 3 1 (sphere)
project 1 0 (sphere)
project 4 6 (sphere)
project 6 7 (sphere)
project 7 5 (sphere)
project 5 4 (sphere)
project 0 4 (sphere)
project 2 6 (sphere)
project 3 7 (sphere)
project 1 5 (sphere)
);
faces
(
project (0 2 6 4) sphere
project (2 3 7 6) sphere
project (3 1 5 7) sphere
project (1 0 4 5) sphere
project (0 1 3 2) sphere
project (4 5 7 6) sphere
);
boundary
(
inlet
{
type patch;
faces
(
(8 10 14 12)
);
}
walls
{
type wall;
inGroups (externalWall);
faces
(
(8 9 11 10)
(12 13 15 14)
(10 11 15 14)
(11 17 19 15)
(9 16 17 11)
(13 18 19 15)
(8 9 13 12)
(9 16 18 13)
);
}
outlet
{
type patch;
faces
(
(16 17 19 18)
);
}
);
// ************************************************************************* //

52
tutorials/modules/CHT/coolingSphere/system/controlDict Normal file
View File

@ -0,0 +1,52 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application foamMultiRun;
#includeIfPresent "regionSolvers"
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 1;
deltaT 5e-4;
writeControl runTime;
writeInterval 0.05;
purgeWrite 0;
writeFormat ascii;
writePrecision 8;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
functions
{
}
// ************************************************************************* //

32
tutorials/modules/CHT/coolingSphere/system/decomposeParDict Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- 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 (2 2 1);
}
hierarchicalCoeffs
{
n (2 2 1);
order xyz;
}
// ************************************************************************* //

45
tutorials/modules/CHT/coolingSphere/system/fvSchemes 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 dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
}
gradSchemes
{
}
divSchemes
{
}
laplacianSchemes
{
}
interpolationSchemes
{
}
snGradSchemes
{
}
fluxRequired
{
}
// ************************************************************************* //

21
tutorials/modules/CHT/coolingSphere/system/fvSolution 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 dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
"(PIMPLE|PISO)"
{
nOuterCorrectors 1;
}
// ************************************************************************* //

38
tutorials/modules/CHT/coolingSphere/system/topoSetDict 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 topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#include "$FOAM_CASE/system/blockMeshDict"
actions
(
{
name cs;
type cellSet;
action new;
source sphereToCell;
centre (0 0 0);
radius $!geometry/sphere/radius;
}
{
name solid;
type cellZoneSet;
action new;
source setToCellZone;
set cs;
}
);
// ************************************************************************* //

55
tutorials/modules/CHT/coolingSphere/templates/0/fluid/T 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;
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#include "$FOAM_CASE/constant/initialConditions"
dimensions [0 0 0 1 0 0 0];
internalField uniform $Tinitial;
boundaryField
{
inlet
{
type fixedValue;
value uniform $Tinitial;
}
outlet
{
type inletOutlet;
inletValue uniform $Tinitial;
value uniform $Tinitial;
}
wall
{
type compressible::turbulentTemperatureCoupledBaffleMixed;
kappa kappa;
Tnbr T;
value uniform $Tinitial;
}
externalWall
{
type fixedValue;
value uniform $Tinitial;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

45
tutorials/modules/CHT/coolingSphere/templates/0/fluid/U 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 volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Uinlet (10 0 0);
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
inlet
{
type fixedValue;
value uniform $Uinlet;
}
outlet
{
type pressureInletOutletVelocity;
value uniform $Uinlet;
}
wall
{
type noSlip;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

43
tutorials/modules/CHT/coolingSphere/templates/0/fluid/alphat Normal file
View File

@ -0,0 +1,43 @@
/*--------------------------------*- 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 alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
wall
{
type compressible::alphatWallFunction;
value uniform 0;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

49
tutorials/modules/CHT/coolingSphere/templates/0/fluid/epsilon 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;
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
epsilonInlet 0.001;
mixingLengthInlet 0.007;
dimensions [0 2 -3 0 0 0 0];
internalField uniform $epsilonInlet;
boundaryField
{
inlet
{
type turbulentMixingLengthDissipationRateInlet;
mixingLength $mixingLengthInlet;
value uniform $epsilonInlet;
}
outlet
{
type inletOutlet;
value uniform $epsilonInlet;
inletValue uniform $epsilonInlet;
}
wall
{
type compressible::epsilonWallFunction;
value uniform $epsilonInlet;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

49
tutorials/modules/CHT/coolingSphere/templates/0/fluid/k 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;
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
kInlet 0.02;
intensityInlet 0.01;
dimensions [0 2 -2 0 0 0 0];
internalField uniform $kInlet;
boundaryField
{
inlet
{
type turbulentIntensityKineticEnergyInlet;
intensity $intensityInlet;
value uniform $kInlet;
}
outlet
{
type inletOutlet;
inletValue uniform $kInlet;
value uniform $kInlet;
}
wall
{
type kqRWallFunction;
value uniform $kInlet;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

43
tutorials/modules/CHT/coolingSphere/templates/0/fluid/nut Normal file
View File

@ -0,0 +1,43 @@
/*--------------------------------*- 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 nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
wall
{
type nutkWallFunction;
value uniform 0;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

48
tutorials/modules/CHT/coolingSphere/templates/0/fluid/omega 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;
object omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
omegaInlet 10;
mixingLengthInlet 0.0035;
dimensions [0 0 -1 0 0 0 0];
internalField uniform $omegaInlet;
boundaryField
{
inlet
{
type turbulentMixingLengthFrequencyInlet;
mixingLength $mixingLengthInlet;
value uniform $omegaInlet;
}
outlet
{
type inletOutlet;
inletValue uniform $omegaInlet;
value uniform $omegaInlet;
}
wall
{
type omegaWallFunction;
value uniform $omegaInlet;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

44
tutorials/modules/CHT/coolingSphere/templates/0/fluid/p Normal file
View File

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

45
tutorials/modules/CHT/coolingSphere/templates/0/fluid/p_rgh Normal file
View File

@ -0,0 +1,45 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class volScalarField;
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#include "$FOAM_CASE/constant/initialConditions"
dimensions [ 1 -1 -2 0 0 0 0 ];
internalField uniform 0;
boundaryField
{
outlet
{
type fixedValue;
value uniform 0;
}
inlet
{
type fixedFluxPressure;
value uniform 0;
}
wall
{
$inlet;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

33
tutorials/modules/CHT/coolingSphere/templates/0/solid/T Normal file
View File

@ -0,0 +1,33 @@
/*--------------------------------*- 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 T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#include "$FOAM_CASE/constant/initialConditions"
dimensions [ 0 0 0 1 0 0 0 ];
internalField uniform $Tinitial;
boundaryField
{
wall
{
type compressible::turbulentTemperatureCoupledBaffleMixed;
value $internalField;
kappa kappa;
Tnbr T;
}
}
// ************************************************************************* //

19
tutorials/modules/CHT/coolingSphere/templates/constant/fluid/g 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 uniformDimensionedVectorField;
object g;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -2 0 0 0 0];
value (0 -9.81 0);
// ************************************************************************* //

22
tutorials/modules/CHT/coolingSphere/templates/constant/fluid/pRef 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 uniformDimensionedScalarField;
location "constant";
object pRef;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#include "$FOAM_CASE/constant/initialConditions"
dimensions [1 -1 -2 0 0 0 0];
value $pInitial;
// ************************************************************************* //

39
tutorials/modules/CHT/coolingSphere/templates/constant/solid/fvModels Normal file
View File

@ -0,0 +1,39 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object fvModels;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
/*
fixedTemperature
{
type fixedTemperatureConstraint;
selectionMode all;
mode uniform;
temperature constant 300; // Set temperature (K)
}
*/
/*
fixedPower
{
type heatSource;
selectionMode all;
Q 100; // Set power (W)
}
*/
//************************************************************************** //

50
tutorials/modules/CHT/coolingSphere/templates/materials/air/momentumTransport Normal file
View File

@ -0,0 +1,50 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object momentumTransport;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RAS;
RAS
{
model kOmegaSST;
turbulence on;
printCoeffs on;
}
LES
{
model SpalartAllmarasDDES;
delta cubeRootVol;
turbulence on;
printCoeffs on;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
maxDeltaRatio 1.1;
}
}
// ************************************************************************* //

47
tutorials/modules/CHT/coolingSphere/templates/materials/air/physicalProperties Normal file
View File

@ -0,0 +1,47 @@
/*--------------------------------*- 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 physicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type heRhoThermo;
mixture pureMixture;
transport const;
thermo hConst;
equationOfState perfectGas;
specie specie;
energy sensibleEnthalpy;
}
mixture
{
specie
{
nMoles 1;
molWeight 28.9; // [g/mol]
}
thermodynamics
{
Cp 1005; // [J/kg/K]
Hf 0;
}
transport
{
mu 1.8e-05; // [kg/m/s]
Pr 0.7;
}
}
// ************************************************************************* //

25
tutorials/modules/CHT/coolingSphere/templates/materials/air/thermophysicalTransport Normal file
View File

@ -0,0 +1,25 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "constant";
object thermophysicalTransport;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
RAS
{
model eddyDiffusivity;
Prt 0.85;
}
// ************************************************************************* //

52
tutorials/modules/CHT/coolingSphere/templates/materials/aluminium/physicalProperties Normal file
View File

@ -0,0 +1,52 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object physicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type heSolidThermo;
mixture pureMixture;
transport constIsoSolid;
thermo eConst;
equationOfState rhoConst;
specie specie;
energy sensibleInternalEnergy;
}
mixture
{
specie
{
nMoles 1;
molWeight 27; // [g/mol]
}
transport
{
kappa 240; // [W/m/K]
}
thermodynamics
{
Hf 0;
Cv 896; // [J/kg/K]
}
equationOfState
{
rho 2712; // [kg/m^3]
}
}
// ************************************************************************* //

52
tutorials/modules/CHT/coolingSphere/templates/materials/copper/physicalProperties Normal file
View File

@ -0,0 +1,52 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object physicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type heSolidThermo;
mixture pureMixture;
transport constIsoSolid;
thermo eConst;
equationOfState rhoConst;
specie specie;
energy sensibleInternalEnergy;
}
mixture
{
specie
{
nMoles 1;
molWeight 63.5; // [g/mol]
}
transport
{
kappa 380; // [W/m/K]
}
thermodynamics
{
Hf 0;
Cv 385; // [J/kg/K]
}
equationOfState
{
rho 8940; // [kg/m^3]
}
}
// ************************************************************************* //

50
tutorials/modules/CHT/coolingSphere/templates/materials/water/momentumTransport Normal file
View File

@ -0,0 +1,50 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object momentumTransport;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RAS;
RAS
{
model kOmegaSST;
turbulence on;
printCoeffs on;
}
LES
{
model SpalartAllmarasDDES;
delta cubeRootVol;
turbulence on;
printCoeffs on;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
maxDeltaRatio 1.1;
}
}
// ************************************************************************* //

51
tutorials/modules/CHT/coolingSphere/templates/materials/water/physicalProperties 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 dictionary;
object physicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type heRhoThermo;
mixture pureMixture;
transport const;
thermo eConst;
equationOfState rPolynomial;
specie specie;
energy sensibleInternalEnergy;
}
mixture
{
specie
{
nMoles 1;
molWeight 18.0; // [g/mol]
}
equationOfState
{
C (0.001278 -2.1055e-06 3.9689e-09 4.3772e-13 -2.0225e-16); // [J/kg/K]
}
thermodynamics
{
Cv 4181; // [J/kg/K] at T = 293 K
Hf 0;
}
transport
{
mu 1.0e-03; // [kg/m/s]
Pr 7;
}
}
// ************************************************************************* //

25
tutorials/modules/CHT/coolingSphere/templates/materials/water/thermophysicalTransport Normal file
View File

@ -0,0 +1,25 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "constant";
object thermophysicalTransport;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
RAS
{
model eddyDiffusivity;
Prt 0.85;
}
// ************************************************************************* //

80
tutorials/modules/CHT/coolingSphere/templates/system/fluid/fvSchemes Normal file
View File

@ -0,0 +1,80 @@
/*--------------------------------*- 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 fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
limited cellLimited Gauss linear 1;
grad(U) $limited;
grad(k) $limited;
grad(omega) $limited;
grad(epsilon) $limited;
}
divSchemes
{
default none;
div(phi,U) Gauss linearUpwind limited;
turbulence Gauss limitedLinear 1;
div(phi,k) $turbulence;
div(phi,omega) $turbulence;
div(phi,epsilon) $turbulence;
div(phi,e) $turbulence;
div(phi,h) $turbulence;
div(phi,K) $turbulence;
div(phi,Ekp) $turbulence;
div(phid,p) Gauss upwind;
div((phi|interpolate(rho)),p) Gauss upwind;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
fluxRequired
{
default no;
p ;
}
wallDist
{
method meshWave;
}
// ************************************************************************* //

75
tutorials/modules/CHT/coolingSphere/templates/system/fluid/fvSolution 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 fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"(rho|rhoFinal)"
{
solver PCG
preconditioner DIC;
tolerance 1e-7;
relTol 0;
}
p_rgh
{
solver GAMG;
tolerance 1e-7;
relTol 0.01;
smoother GaussSeidel;
maxIter 100;
}
"(U|h|e|k|omega|epsilon)"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-6;
relTol 0.1;
}
p_rghFinal
{
$p_rgh;
relTol 0;
}
"(U|h|e|k|omega|epsilon)Final"
{
$U;
relTol 0;
}
}
PIMPLE
{
nCorrectors 2;
nNonOrthogonalCorrectors 1;
pRefCell 0;
pRefValue 0;
}
relaxationFactors
{
equations
{
".*" 1;
}
}
// ************************************************************************* //

26
tutorials/modules/CHT/coolingSphere/templates/system/solid/fvConstraints Normal file
View File

@ -0,0 +1,26 @@
/*--------------------------------*- 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// fixedTemperature
// {
// type fixedTemperatureConstraint;
// selectionMode all;
// mode uniform;
// temperature constant 300; // Set temperature (K)
// }
//************************************************************************** //

46
tutorials/modules/CHT/coolingSphere/templates/system/solid/fvSchemes Normal file
View File

@ -0,0 +1,46 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
default none;
}
laplacianSchemes
{
default Gauss linear uncorrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default uncorrected;
}
// ************************************************************************* //

46
tutorials/modules/CHT/coolingSphere/templates/system/solid/fvSolution Normal file
View File

@ -0,0 +1,46 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"(h|e)"
{
solver PCG;
preconditioner DIC;
tolerance 1e-06;
relTol 0.1;
}
"(h|e)Final"
{
$h;
relTol 0;
}
}
PIMPLE
{
nNonOrthogonalCorrectors 0;
}
relaxationFactors
{
equations
{
".*" 1;
}
}
// ************************************************************************* //