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

semiPermeableBaffle: Added two new boundary conditions and a tutorial

Browse Source 
Two boundary conditions for the modelling of semi-permeable baffles have
been added. These baffles are permeable to a number of species within
the flow, and are impermeable to others. The flux of a given species is
calculated as a constant multipled by the drop in mass fraction across
the baffle.

The species mass-fraction condition requires the transfer constant and
the name of the patch on the other side of the baffle:

boundaryField
{
    // ...

    membraneA
    {
        type            semiPermeableBaffleMassFraction;
        samplePatch     membranePipe;
        c               0.1;
        value           uniform 0;
    }
    membraneB
    {
        type            semiPermeableBaffleMassFraction;
        samplePatch     membraneSleeve;
        c               0.1;
        value           uniform 1;
    }
}

If the value of c is omitted, or set to zero, then the patch is
considered impermeable to the species in question. The samplePatch entry
can also be omitted in this case.

The velocity condition does not require any special input:

boundaryField
{
    // ...

    membraneA
    {
        type            semiPermeableBaffleVelocity;
        value           uniform (0 0 0);
    }
    membraneB
    {
        type            semiPermeableBaffleVelocity;
        value           uniform (0 0 0);
    }
}

These two boundary conditions must be used in conjunction, and the
mass-fraction condition must be applied to all species in the
simulation. The calculation will fail with an error message if either is
used in isolation.

A tutorial, combustion/reactingFoam/RAS/membrane, has been added which
demonstrates this transfer process.

This work was done with support from Stefan Lipp, at BASF.
This commit is contained in:
Will Bainbridge
2017-10-19 10:00:36 +01:00
parent 644253773f
commit 3055587a5c
37 changed files with 2195 additions and 0 deletions
Download Patch File Download Diff File Expand all files Collapse all files

69
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/CH4 Normal file
View File

@ -0,0 +1,69 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object CH4;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#include "include"
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
inletSleeve
{
type fixedValue;
value uniform $:sleeve.CH4;
}
inletPipe
{
type fixedValue;
value uniform $:pipe.CH4;
}
outletSleeve
{
type inletOutlet;
inletValue uniform $:sleeve.CH4;
value uniform $:sleeve.CH4;
}
outletPipe
{
type inletOutlet;
inletValue uniform $:pipe.CH4;
value uniform $:pipe.CH4;
}
wall
{
type zeroGradient;
}
membraneSleeve
{
type semiPermeableBaffleMassFraction;
samplePatch membranePipe;
c 0.1;
value uniform $:sleeve.CH4;
}
membranePipe
{
type semiPermeableBaffleMassFraction;
samplePatch membraneSleeve;
c 0.1;
value uniform $:pipe.CH4;
}
}
// ************************************************************************* //

65
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/N2 Normal file
View File

@ -0,0 +1,65 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object N2;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#include "include"
dimensions [0 0 0 0 0 0 0];
internalField uniform 1;
boundaryField
{
inletSleeve
{
type fixedValue;
value uniform $:sleeve.N2;
}
inletPipe
{
type fixedValue;
value uniform $:pipe.N2;
}
outletSleeve
{
type inletOutlet;
inletValue uniform $:sleeve.N2;
value uniform $:sleeve.N2;
}
outletPipe
{
type inletOutlet;
inletValue uniform $:pipe.N2;
value uniform $:pipe.N2;
}
wall
{
type zeroGradient;
}
membraneSleeve
{
type semiPermeableBaffleMassFraction;
value uniform $:sleeve.N2;
}
membranePipe
{
type semiPermeableBaffleMassFraction;
value uniform $:pipe.N2;
}
}
// ************************************************************************* //

65
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/O2 Normal file
View File

@ -0,0 +1,65 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object O2;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#include "include"
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
inletSleeve
{
type fixedValue;
value uniform $:sleeve.O2;
}
inletPipe
{
type fixedValue;
value uniform $:pipe.O2;
}
outletSleeve
{
type inletOutlet;
inletValue uniform $:sleeve.O2;
value uniform $:sleeve.O2;
}
outletPipe
{
type inletOutlet;
inletValue uniform $:pipe.O2;
value uniform $:pipe.O2;
}
wall
{
type zeroGradient;
}
membraneSleeve
{
type semiPermeableBaffleMassFraction;
value uniform $:sleeve.O2;
}
membranePipe
{
type semiPermeableBaffleMassFraction;
value uniform $:pipe.O2;
}
}
// ************************************************************************* //

42
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/T Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 293;
boundaryField
{
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
"(wall|membrane).*"
{
type zeroGradient;
}
}
// ************************************************************************* //

56
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/U Normal file
View File

@ -0,0 +1,56 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
inletSleeve
{
type fixedValue;
value uniform (1 0 0);
}
inletPipe
{
type fixedValue;
value uniform (0 0 1);
}
outlet
{
type pressureInletOutletVelocity;
value $internalField;
}
wall
{
type noSlip;
}
membraneSleeve
{
type semiPermeableBaffleVelocity;
value $internalField;
}
membranePipe
{
type semiPermeableBaffleVelocity;
value $internalField;
}
}
// ************************************************************************* //

52
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/Ydefault Normal file
View File

@ -0,0 +1,52 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object Ydefault;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
wall
{
type zeroGradient;
}
membraneSleeve
{
type semiPermeableBaffleMassFraction;
value $internalField;
}
membranePipe
{
type semiPermeableBaffleMassFraction;
value $internalField;
}
}
// ************************************************************************* //

42
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/alphat Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type zeroGradient;
}
"(wall|membrane).*"
{
type compressible::alphatWallFunction;
Prt 0.85;
value $internalField;
}
}
// ************************************************************************* //

44
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/epsilon Normal file
View File

@ -0,0 +1,44 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -3 0 0 0 0];
internalField uniform 0.012;
boundaryField
{
inlet
{
type turbulentMixingLengthDissipationRateInlet;
mixingLength 0.1;
value $internalField;
}
outlet
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
"(wall|membrane).*"
{
type epsilonWallFunction;
value $internalField;
}
}
// ************************************************************************* //

33
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/include Normal file
View File

@ -0,0 +1,33 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "0";
object include;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
sleeve
{
CH4 0;
N2 0.79;
O2 0.21;
}
pipe
{
CH4 0.5;
O2 0;
N2 0.5;
}
// ************************************************************************* //

44
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/k Normal file
View File

@ -0,0 +1,44 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0.00375;
boundaryField
{
inlet
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.05;
value $internalField;
}
outlet
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
"(wall|membrane).*"
{
type kqRWallFunction;
value $internalField;
}
}
// ************************************************************************* //

42
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/nut Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type calculated;
value $internalField;
}
outlet
{
type calculated;
value $internalField;
}
"(wall|membrane).*"
{
type nutkWallFunction;
value $internalField;
}
}
// ************************************************************************* //

40
tutorials/combustion/reactingFoam/RAS/membrane/0.orig/p Normal file
View File

@ -0,0 +1,40 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 1e5;
boundaryField
{
inlet
{
type fixedFluxPressure;
}
outlet
{
type totalPressure;
p0 $internalField;
}
"(wall|membrane).*"
{
type fixedFluxPressure;
}
}
// ************************************************************************* //

7
tutorials/combustion/reactingFoam/RAS/membrane/Allclean Executable file
View File

@ -0,0 +1,7 @@
#!/bin/sh
cd ${0%/*} || exit 1
. $WM_PROJECT_DIR/bin/tools/CleanFunctions
rm -rf 0 constant/triSurface/membrane-*.stl.gz && cleanCase

20
tutorials/combustion/reactingFoam/RAS/membrane/Allrun Executable file
View File

@ -0,0 +1,20 @@
#!/bin/sh
cd ${0%/*} || exit 1 cd ${0%/*} || exit 1
. $WM_PROJECT_DIR/bin/tools/RunFunctions
cp \
$FOAM_TUTORIALS/resources/geometry/membrane-boundaries.stl.gz \
$FOAM_TUTORIALS/resources/geometry/membrane-membrane.stl.gz \
constant/triSurface
runApplication blockMesh
runApplication snappyHexMesh -overwrite
runApplication createBaffles -overwrite
cp -r 0.orig 0
runApplication setFields
runApplication reactingFoam

35
tutorials/combustion/reactingFoam/RAS/membrane/constant/chemistryProperties Normal file
View File

@ -0,0 +1,35 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object chemistryProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
chemistryType
{
chemistrySolver EulerImplicit;
chemistryThermo psi;
}
chemistry off;
initialChemicalTimeStep 1e-07;
EulerImplicitCoeffs
{
cTauChem 1;
equilibriumRateLimiter off;
}
// ************************************************************************* //

21
tutorials/combustion/reactingFoam/RAS/membrane/constant/combustionProperties Normal file
View File

@ -0,0 +1,21 @@
/*-----------------m---------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object combustionProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
combustionModel noCombustion<psiThermoCombustion>;
// ************************************************************************* //

40
tutorials/combustion/reactingFoam/RAS/membrane/constant/reactions Normal file
View File

@ -0,0 +1,40 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class IOobject;
location "constant";
object reactions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
species
(
O2
H2O
CH4
CO2
N2
);
reactions
{
methaneReaction
{
type irreversibleArrheniusReaction;
reaction "CH4 + 2O2 = CO2 + 2H2O";
A 5.2e16;
beta 0;
Ta 14906;
}
}
// ************************************************************************* //

124
tutorials/combustion/reactingFoam/RAS/membrane/constant/thermo.compressibleGas Normal file
View File

@ -0,0 +1,124 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object thermo.compressibleGas;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
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 1.67212e-06;
Ts 170.672;
}
}
H2O
{
specie
{
molWeight 18.0153;
}
thermodynamics
{
Tlow 200;
Thigh 5000;
Tcommon 1000;
highCpCoeffs ( 2.67215 0.00305629 -8.73026e-07 1.201e-10 -6.39162e-15 -29899.2 6.86282 );
lowCpCoeffs ( 3.38684 0.00347498 -6.3547e-06 6.96858e-09 -2.50659e-12 -30208.1 2.59023 );
}
transport
{
As 1.67212e-06;
Ts 170.672;
}
}
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 1.67212e-06;
Ts 170.672;
}
}
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 1.67212e-06;
Ts 170.672;
}
}
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 1.67212e-06;
Ts 170.672;
}
}
// ************************************************************************* //

38
tutorials/combustion/reactingFoam/RAS/membrane/constant/thermophysicalProperties Normal file
View File

@ -0,0 +1,38 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type hePsiThermo;
mixture reactingMixture;
transport sutherland;
thermo janaf;
energy sensibleEnthalpy;
equationOfState perfectGas;
specie specie;
}
inertSpecie N2;
chemistryReader foamChemistryReader;
foamChemistryFile "$FOAM_CASE/constant/reactions";
foamChemistryThermoFile "$FOAM_CASE/constant/thermo.compressibleGas";
// ************************************************************************* //

4
tutorials/combustion/reactingFoam/RAS/membrane/constant/triSurface/README Normal file
View File

@ -0,0 +1,4 @@
Directory to house tri-surfaces
The Allrun script copies the surface from the $FOAM_TUTORIALS/resources/geometry
directory

28
tutorials/combustion/reactingFoam/RAS/membrane/constant/turbulenceProperties Normal file
View File

@ -0,0 +1,28 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RAS;
RAS
{
RASModel kEpsilon;
turbulence on;
printCoeffs on;
}
// ************************************************************************* //

49
tutorials/combustion/reactingFoam/RAS/membrane/system/blockMeshDict Normal file
View File

@ -0,0 +1,49 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;
vertices
(
(-2.5 -1.2 -3.0)
( 2.5 -1.2 -3.0)
(-2.5 1.2 -3.0)
( 2.5 1.2 -3.0)
(-2.5 -1.2 3.0)
( 2.5 -1.2 3.0)
(-2.5 1.2 3.0)
( 2.5 1.2 3.0)
);
blocks
(
hex (0 1 3 2 4 5 7 6) (50 24 60) simpleGrading (1 1 1)
);
edges
(
);
boundary
(
);
mergePatchPairs
(
);
// ************************************************************************* //

55
tutorials/combustion/reactingFoam/RAS/membrane/system/controlDict Normal file
View File

@ -0,0 +1,55 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application reactingFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 10;
deltaT 1e-3;
writeControl adjustableRunTime;
writeInterval 0.1;
purgeWrite 0;
writeFormat binary;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
adjustTimeStep yes;
maxCo 1;
libs ( "libsemiPermeableBaffle.so" );
// ************************************************************************* //

43
tutorials/combustion/reactingFoam/RAS/membrane/system/createBafflesDict Normal file
View File

@ -0,0 +1,43 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object createBafflesDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
internalFacesOnly true;
baffles
{
membrane
{
type faceZone;
zoneName membrane;
patches
{
master
{
name membranePipe;
type wall;
}
slave
{
name membraneSleeve;
type wall;
}
}
}
}
// ************************************************************************* //

57
tutorials/combustion/reactingFoam/RAS/membrane/system/fvSchemes Normal file
View File

@ -0,0 +1,57 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
default none;
div(phi,U) Gauss limitedLinearV 1;
div(phi,Yi_h) Gauss limitedLinear 1;
div(phi,K) Gauss limitedLinear 1;
div(phid,p) Gauss limitedLinear 1;
div(phi,epsilon) Gauss limitedLinear 1;
div(phi,k) Gauss limitedLinear 1;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear orthogonal;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default orthogonal;
}
// ************************************************************************* //

69
tutorials/combustion/reactingFoam/RAS/membrane/system/fvSolution Normal file
View File

@ -0,0 +1,69 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"rho.*"
{
solver diagonal;
}
p
{
solver PCG;
preconditioner DIC;
tolerance 1e-6;
relTol 0.1;
}
pFinal
{
$p;
tolerance 1e-6;
relTol 0.0;
}
"(U|h|k|epsilon)"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-6;
relTol 0.1;
}
"(U|h|k|epsilon)Final"
{
$U;
relTol 0;
}
Yi
{
$hFinal;
}
}
PIMPLE
{
momentumPredictor yes;
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
}
// ************************************************************************* //

20
tutorials/combustion/reactingFoam/RAS/membrane/system/meshQualityDict Normal file
View File

@ -0,0 +1,20 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object meshQualityDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#includeEtc "caseDicts/meshQualityDict"
// ************************************************************************* //

42
tutorials/combustion/reactingFoam/RAS/membrane/system/setFieldsDict Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#include "../0.orig/include"
defaultFieldValues
(
volScalarFieldValue CH4 $:sleeve.CH4
volScalarFieldValue N2 $:sleeve.N2
volScalarFieldValue O2 $:sleeve.O2
);
regions
(
zoneToCell
{
name pipe;
fieldValues
(
volScalarFieldValue CH4 $:pipe.CH4
volScalarFieldValue N2 $:pipe.N2
volScalarFieldValue O2 $:pipe.O2
);
}
);
// ************************************************************************* //

168
tutorials/combustion/reactingFoam/RAS/membrane/system/snappyHexMeshDict Normal file
View File

@ -0,0 +1,168 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object snappyHexMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#includeEtc "caseDicts/mesh/generation/snappyHexMeshDict.cfg"
castellatedMesh true;
snap true;
addLayers false;
geometry
{
boundaries
{
type triSurfaceMesh;
file "membrane-boundaries.stl";
regions
{
inletSleeve
{
name inletSleeve;
}
inletPipe
{
name inletPipe;
}
outletSleeve
{
name outletSleeve;
}
outletPipe
{
name outletPipe;
}
wallSleeve
{
name wallSleeve;
}
wallPipe
{
name wallPipe;
}
}
}
membrane
{
type triSurfaceMesh;
file "membrane-membrane.stl";
}
};
castellatedMeshControls
{
features ();
refinementSurfaces
{
boundaries
{
level (0 0);
regions
{
inletSleeve
{
level (0 0);
patchInfo
{
type patch;
inGroups (inlet);
}
}
inletPipe
{
level (0 0);
patchInfo
{
type patch;
inGroups (inlet);
}
}
outletSleeve
{
level (0 0);
patchInfo
{
type patch;
inGroups (outlet);
}
}
outletPipe
{
level (0 0);
patchInfo
{
type patch;
inGroups (outlet);
}
}
wallSleeve
{
level (0 0);
patchInfo
{
type wall;
inGroups (wall);
}
}
wallPipe
{
level (0 0);
patchInfo
{
type wall;
inGroups (wall);
}
}
}
}
membrane
{
level (0 0);
cellZone pipe;
faceZone membrane;
cellZoneInside insidePoint;
insidePoint (0 0 0);
}
}
refinementRegions {}
locationInMesh (0 0 0);
}
snapControls
{
implicitFeatureSnap true;
}
addLayersControls
{
relativeSizes true;
minThickness 0.25;
finalLayerThickness 0.3;
expansionRatio 1.0;
layers {}
}
meshQualityControls
{
#includeEtc "caseDicts/mesh/generation/meshQualityDict.cfg"
}
// ************************************************************************* //

BIN
tutorials/resources/geometry/membrane-boundaries.stl.gz Normal file
View File

Binary file not shown.

BIN
tutorials/resources/geometry/membrane-membrane.stl.gz Normal file
View File

Binary file not shown.