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

55
tutorials/modules/fluid/externalCoupledCavity/0/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;
location "0";
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 293;
boundaryField
{
frontAndBack
{
type zeroGradient;
}
topAndBottom
{
type zeroGradient;
}
hot
{
type externalCoupledTemperature;
commsDir "${FOAM_CASE}/comms";
file "data";
initByExternal yes;
log true;
value uniform 307.75; // 34.6 degC
}
cold
{
type externalCoupledTemperature;
commsDir "${FOAM_CASE}/comms";
file "data";
initByExternal yes;
log true;
value uniform 288.15; // 15 degC
}
}
// ************************************************************************* //

45
tutorials/modules/fluid/externalCoupledCavity/0/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;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
frontAndBack
{
type noSlip;
}
topAndBottom
{
type noSlip;
}
hot
{
type noSlip;
}
cold
{
type noSlip;
}
}
// ************************************************************************* //

50
tutorials/modules/fluid/externalCoupledCavity/0/alphat 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 volScalarField;
location "0";
object alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
frontAndBack
{
type compressible::alphatWallFunction;
Prt 0.85;
value uniform 0;
}
topAndBottom
{
type compressible::alphatWallFunction;
Prt 0.85;
value uniform 0;
}
hot
{
type compressible::alphatWallFunction;
Prt 0.85;
value uniform 0;
}
cold
{
type compressible::alphatWallFunction;
Prt 0.85;
value uniform 0;
}
}
// ************************************************************************* //

46
tutorials/modules/fluid/externalCoupledCavity/0/epsilon 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 volScalarField;
location "0";
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -3 0 0 0 0];
internalField uniform 4e-06;
boundaryField
{
frontAndBack
{
type epsilonWallFunction;
value uniform 4e-06;
}
topAndBottom
{
type epsilonWallFunction;
value uniform 4e-06;
}
hot
{
type epsilonWallFunction;
value uniform 4e-06;
}
cold
{
type epsilonWallFunction;
value uniform 4e-06;
}
}
// ************************************************************************* //

46
tutorials/modules/fluid/externalCoupledCavity/0/k 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 volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 3.75e-04;
boundaryField
{
frontAndBack
{
type kqRWallFunction;
value uniform 3.75e-04;
}
topAndBottom
{
type kqRWallFunction;
value uniform 3.75e-04;
}
hot
{
type kqRWallFunction;
value uniform 3.75e-04;
}
cold
{
type kqRWallFunction;
value uniform 3.75e-04;
}
}
// ************************************************************************* //

46
tutorials/modules/fluid/externalCoupledCavity/0/nut 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 volScalarField;
location "0";
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
frontAndBack
{
type nutUWallFunction;
value uniform 0;
}
topAndBottom
{
type nutUWallFunction;
value uniform 0;
}
hot
{
type nutUWallFunction;
value uniform 0;
}
cold
{
type nutUWallFunction;
value uniform 0;
}
}
// ************************************************************************* //

46
tutorials/modules/fluid/externalCoupledCavity/0/omega 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 volScalarField;
location "0";
object omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 -1 0 0 0 0];
internalField uniform 0.12;
boundaryField
{
frontAndBack
{
type omegaWallFunction;
value uniform 0.12;
}
topAndBottom
{
type omegaWallFunction;
value uniform 0.12;
}
hot
{
type omegaWallFunction;
value uniform 0.12;
}
cold
{
type omegaWallFunction;
value uniform 0.12;
}
}
// ************************************************************************* //

49
tutorials/modules/fluid/externalCoupledCavity/0/p 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 1e5;
boundaryField
{
frontAndBack
{
type calculated;
value $internalField;
}
topAndBottom
{
type calculated;
value $internalField;
}
hot
{
type calculated;
value $internalField;
}
cold
{
type calculated;
value $internalField;
}
}
// ************************************************************************* //

49
tutorials/modules/fluid/externalCoupledCavity/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
{
frontAndBack
{
type fixedFluxPressure;
value $internalField;
}
topAndBottom
{
type fixedFluxPressure;
value $internalField;
}
hot
{
type fixedFluxPressure;
value $internalField;
}
cold
{
type fixedFluxPressure;
value $internalField;
}
}
// ************************************************************************* //

13
tutorials/modules/fluid/externalCoupledCavity/Allclean 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/CleanFunctions
cleanCase
rm -rf comms
killall -q externalSolver
#------------------------------------------------------------------------------

10
tutorials/modules/fluid/externalCoupledCavity/Allmesh Executable file
View File

@ -0,0 +1,10 @@
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
runApplication blockMesh
runApplication createExternalCoupledPatchGeometry T
#------------------------------------------------------------------------------

13
tutorials/modules/fluid/externalCoupledCavity/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
./Allmesh
runApplication $(getApplication) &
./externalSolver
#------------------------------------------------------------------------------

15
tutorials/modules/fluid/externalCoupledCavity/Allrun-parallel Executable file
View File

@ -0,0 +1,15 @@
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
./Allmesh
runApplication decomposePar
runParallel $(getApplication) &
./externalSolver
#------------------------------------------------------------------------------

5
tutorials/modules/fluid/externalCoupledCavity/README Normal file
View File

@ -0,0 +1,5 @@
Example of an explicit coupling between OpenFOAM and an external application
using the externalCoupled boundary conditions.
The case is based on the buoyantCavity tutorial case, whereby on each iteration
the 'hot' and 'cold' patch temperatures are incremented by 1K.

21
tutorials/modules/fluid/externalCoupledCavity/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/fluid/externalCoupledCavity/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 RASProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RAS;
RAS
{
model kOmegaSST;
turbulence on;
printCoeffs on;
}
// ************************************************************************* //

20
tutorials/modules/fluid/externalCoupledCavity/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 1e5;
// ************************************************************************* //

47
tutorials/modules/fluid/externalCoupledCavity/constant/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;
location "constant";
object physicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type heRhoThermo;
mixture pureMixture;
transport const;
thermo hConst;
equationOfState perfectGas;
specie specie;
energy sensibleEnthalpy;
}
mixture
{
specie
{
molWeight 28.96;
}
thermodynamics
{
Cp 1004.4;
Hf 0;
}
transport
{
mu 1.831e-05;
Pr 0.705;
}
}
// ************************************************************************* //

85
tutorials/modules/fluid/externalCoupledCavity/externalSolver Executable file
View File

@ -0,0 +1,85 @@
#!/bin/sh
#
# Dummy external solver to communicate with OpenFOAM via externalCoupled
# boundary conditions
#
# Functionality is hard-coded for this particular test case
# - patch temperatures increased by 1K on each step
#
cd ${0%/*} || exit 1 # run from this directory
echo "Executing dummy external solver"
commsDir="comms"
lockFile="${commsDir}/OpenFOAM.lock"
dataFile="${commsDir}/data"
waitSec=1
timeOut=10
refGrad=0
valueFraction=1
log()
{
echo "External: $@"
}
init()
{
log "initialisation: creating ${dataFile}.in"
# Hard-coded for 2 patches of size 2250
n=2250
refCold=283
refHot=303
touch "${dataFile}.in"
for i in $(seq 1 $n); do
echo "$refHot $refGrad $valueFraction" >> "${dataFile}.in"
done
for i in $(seq 1 $n); do
echo "$refCold $refGrad $valueFraction" >> "${dataFile}.in"
done
# create lock file to pass control to OF
touch ${lockFile}
}
# tutorial case employs the 'initByExternalOption', so we need to provide
# the initial values
init
totalWait=0
step=0
while [ 1 ]; do
if [ -f $lockFile ]; then
log "found lock file ${lockFile} - waiting"
totalWait=$(expr $totalWait + $waitSec)
if [ $totalWait -gt $timeOut ]; then
log "timeout"
break
else
sleep $waitSec
fi
else
totalWait=0
step=$(expr $step + 1)
log "step $step"
log "lock not present - taking control"
log "sleeping for $waitSec secs to simulate external process"
sleep $waitSec
log "creating ${dataFile}.in"
awk '{if( $1 != "#" ){print $2+1 " 0 1"}}' ${dataFile}.out > ${dataFile}.in
log "creating lock file ${lockFile}"
touch ${lockFile}
fi
done
log "done"
#------------------------------------------------------------------------------

77
tutorials/modules/fluid/externalCoupledCavity/system/blockMeshDict Normal file
View File

@ -0,0 +1,77 @@
/*--------------------------------*- 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 0.001;
vertices
(
( 0 0 -260)
(76 0 -260)
(76 2180 -260)
( 0 2180 -260)
( 0 0 260)
(76 0 260)
(76 2180 260)
( 0 2180 260)
);
blocks
(
hex (0 1 2 3 4 5 6 7) (35 150 15) simpleGrading (1 1 1)
);
boundary
(
frontAndBack
{
type wall;
faces
(
(0 1 5 4)
(2 3 7 6)
);
}
topAndBottom
{
type wall;
faces
(
(4 5 6 7)
(3 2 1 0)
);
}
hot
{
type wall;
faces
(
(6 5 1 2)
);
}
cold
{
type wall;
faces
(
(4 7 3 0)
);
}
);
// ************************************************************************* //

49
tutorials/modules/fluid/externalCoupledCavity/system/controlDict 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 dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application foamRun;
solver fluid;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 100;
deltaT 1;
writeControl timeStep;
writeInterval 10;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* //

27
tutorials/modules/fluid/externalCoupledCavity/system/decomposeParDict Normal file
View File

@ -0,0 +1,27 @@
/*--------------------------------*- 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 decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 4;
method simple;
simpleCoeffs
{
n (2 2 1);
}
// ************************************************************************* //

60
tutorials/modules/fluid/externalCoupledCavity/system/fvSchemes 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;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
default none;
div(phi,U) bounded Gauss limitedLinear 0.2;
div(phi,K) bounded Gauss limitedLinear 0.2;
div(phi,h) bounded Gauss limitedLinear 0.2;
div(phi,k) bounded Gauss limitedLinear 0.2;
div(phi,epsilon) bounded Gauss limitedLinear 0.2;
div(phi,omega) bounded Gauss limitedLinear 0.2;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear orthogonal;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default orthogonal;
}
wallDist
{
method meshWave;
}
// ************************************************************************* //

72
tutorials/modules/fluid/externalCoupledCavity/system/fvSolution Normal file
View File

@ -0,0 +1,72 @@
/*--------------------------------*- 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_rgh
{
solver GAMG;
tolerance 1e-7;
relTol 0.01;
smoother DICGaussSeidel;
}
"(U|h|k|epsilon|omega)"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-8;
relTol 0.1;
}
}
PIMPLE
{
momentumPredictor yes;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
residualControl
{
p_rgh 1e-2;
U 1e-3;
h 1e-3;
// possibly check turbulence fields
"(k|epsilon|omega)" 1e-3;
}
}
relaxationFactors
{
fields
{
rho 1.0;
p_rgh 0.7;
}
equations
{
U 0.3;
h 0.3;
"(k|epsilon|omega)" 0.7;
}
}
// ************************************************************************* //