Modeling Turbulent Reactive Flow
 

Hi I am trying to model a multi-species, turbulent reactive flow. From the examples, I understand I need to create a chemkin type format for the reacting species and a thermophysical data file. However, are there any models similar to the Eddy-break-up model in OpenFoam ? If so, where do I find it and how do I change the mixing parameters for this model ?

Thanks in advance.

Sanjib

Hello Sanjib,

search the forum with keyword "reactingFoam" which is a general reacting flow solver in OpenFOAM. You can find a tutorial case here:

http://openfoamwiki.net/index.php/Tu..._firstTutorial

The mixing parameter "Cmix" can be found in "constant/chemistryProperties" dictionary. As you mentioned, the chemical properties are read in ChemKin format.

The chemisty is solved in a separate library and called in "reactingFoam" solver, so the solver code is quite compact. You can find the source code file for turbulence-chemistry interaction "chemistry.H" in "reactingFoam" solver directory. You can find similarities with the Chalmers PaSR model to other eddy-break up models.

Hope this helps,
Ville

hi, I'm working on the similar area. Are there more advanced combustion method like flamelet or even PDF in OpenFOAM?
Thanks a lot!

I haven't seen transported PDF model in OpenFOAM. Someone else can correct me if I'm wrong.

Are you interested in non-premixed or premixed flamelet models? Hannes Kroger at University of Rostock has worked on premixed combustion. He has a SVN repository for all of his stuff (search the forum "hannes repository).

Hannes' work has helped me on my ever-lasting project which is more about non-premixed combustion and deals with flamelet/progress-variable model.

About the more sophisticated models in OpenFOAM, you should check this thread:

http://www.cfd-online.com/Forums/ope...ion-model.html

Hope this helped,
Ville

thanks ville!

I found hannes repository and his work is very helpful to my research.

I'm working on non-premixed combustion with PDF transport model. My supervisor and me are working on a new mixing model and considering implement it in openFOAM. But the previous problem is that no much OPENFOAM usage in my school, university of Queesland, AU.

If that's possible I'd like to know more of your work with OpenFOAM. My email is yipeng.ge@uqconnect.edu.au

Cheers

premixed combustion
 

Hi,

I am working in premixed flame modelling and I have searched for the repository of Hannes Kroger but without success.
Could someone explain what exactly to search for in order to find it or post a link to it?

Thanks

Here's the link for the post:
http://www.cfd-online.com/Forums/ope...tml#post198279

Thank you for the link

Hello Vill, hello Sanjib, hello everyone

I am trying to impliment a turbulent reacting flow. my idea was to use the reactingFoam solver.

My case:
i have zylinder with a fuel (CH4) inlet, an air inlet and a coflow inlet. at the other of the zylinder is an outlet.

first of all i impliment a simpleFoam case just with velocity field (without the reaction). that works fine. so, now i am trying to add the reaction.

i was trying to run the reactingFoam tutorial (http://openfoamwiki.net/index.php/Tu..._firstTutorial). i updated the path of the "chem.inp" and "therm.dat" files as describe and run the case. after the there was a error message.

"keyword psiChemistryModel is undefined in dictionary"

so, i added the keyword as in the dieselFoam tutorial.

"psiChemistryModel ODEChemistryModel<gasThermoPhysics>;"

another error message came up.

Reading chemistry properties


Reading g

Reading thermophysicalProperties
Selecting psiChemistryModel ODEChemistryModel<gasThermoPhysics>
Selecting thermodynamics package hPsiMixtureThermo<reactingMixture<gasThermoPhysics >>
Selecting chemistryReader chemkinReader
#0 Foam::error::printStack(Foam::Ostream&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3 Foam::DimensionedField<double, Foam::volMesh>::operator/=(Foam::DimensionedField<double, Foam::volMesh> const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#4 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>:
perator/=(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#5 Foam::multiComponentMixture<Foam::sutherlandTransp ort<Foam::specieThermo<Foam::janafThermo<Foam::per fectGas> > > >::correctMassFractions() in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#6 Foam::multiComponentMixture<Foam::sutherlandTransp ort<Foam::specieThermo<Foam::janafThermo<Foam::per fectGas> > > >::multiComponentMixture(Foam::dictionary const&, Foam::List<Foam::word> const&, Foam::HashPtrTable<Foam::sutherlandTransport<Foam: :specieThermo<Foam::janafThermo<Foam::perfectGas> > >, Foam::word, Foam::string::hash> const&, Foam::fvMesh const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#7 Foam::reactingMixture<Foam::sutherlandTransport<Fo am::specieThermo<Foam::janafThermo<Foam::perfectGa s> > > >::reactingMixture(Foam::dictionary const&, Foam::fvMesh const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#8 Foam::hPsiMixtureThermo<Foam::reactingMixture<Foam ::sutherlandTransport<Foam::specieThermo<Foam::jan afThermo<Foam::perfectGas> > > > >::hPsiMixtureThermo(Foam::fvMesh const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#9 Foam::hCombustionThermo::addfvMeshConstructorToTab le<Foam::hPsiMixtureThermo<Foam::reactingMixture<F oam::sutherlandTransport<Foam::specieThermo<Foam:: janafThermo<Foam::perfectGas> > > > > >::New(Foam::fvMesh const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#10 Foam::hCombustionThermo::NewType(Foam::fvMesh const&, Foam::word const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#11 Foam:siChemistryModel:siChemistryModel(Foam::fvMes h const&, Foam::word const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libchemistryModel.so"
#12 Foam::ODEChemistryModel<Foam:siChemistryModel, Foam::sutherlandTransport<Foam::specieThermo<Foam: :janafThermo<Foam:erfectGas> > > >::ODEChemistryModel(Foam::fvMesh const&, Foam::word const&, Foam::word const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libchemistryModel.so"
#13 Foam:siChemistryModel::addfvMeshConstructorToTable <Foam::ODEChemistryModel<Foam:siChemistryModel, Foam::sutherlandTransport<Foam::specieThermo<Foam: :janafThermo<Foam:
erfectGas> > > > >::New(Foam::fvMesh const&, Foam::word const&, Foam::word const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libchemistryModel.so"
#14 Foam:siChemistryModel::New(Foam::fvMesh const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libchemistryModel.so"
#15 main in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/reactingFoam"
#16 __libc_start_main in "/lib/libc.so.6"
#17 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/i386/elf/start.S:122
Gleitkomma-Ausnahme

so, i don't know what's mean. has anyone an helpfull advice for me how to fix my problem.

Thanks in advance.

regarts,

Ilja

IIja,

I was able to reproduce a similar error when I either set all the initial mass fractions to 0 or
all the mass fractions were set to 0 at any boundary.

Dave

Hey Dave,

thank you for your advice. i played a bit with the mass fraction and set it like below.

BC T CH4 O2 N2
inlet one 293 0.5 0 0
inlet two 293 0.5 0 0
inlet three 293 0 0.2 0.8
Internal field 293 0 0.2 0.8

the mass fraction in the Ydefault-file are set to all to 0.

but i have still the same error! :(

the mass fraction is the fraction of one substance with there mass to the total mixture mass. where i have to set the total mixture mass of a species?


Regards, Ilja

IIja,

Could you post the text for the "thermophysicalProperties" and "chem.inp" for the case
described above ?

You could also try running with all the inlet mass fractions set to the the mass fractions of the initial condition.

Dave

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format binary;
class dictionary;
location "constant";
object thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType hPsiMixtureThermo<reactingMixture<gasThermoPhysics >>;

CHEMKINFile "$FOAM_CASE/chemkin/chem.inp";

CHEMKINThermoFile "~OpenFOAM/thermoData/therm.dat";

inertSpecie N2;

liquidComponents ( CH4 );

liquidProperties
{
CH4 CH4 defaultCoeffs;
}


// ************************************************** *********************** //

and the cham.inp file...

ELEMENTS
H O C N
END
SPECIE
CH4 O2 N2 CO2 H2O
END
REACTIONS
CH4 + 2O2 => CO2 + 2H2O 6.70091E+12 0.0 4.84149E+04! 1
FORD / CH4 0.2 /
FORD / O2 1.3 /
END

IIja,

I ran the tutorial case with the settings described in the previous posts I was only able to reproduce the error when the sum of the species mass fractions was equal to zero. The code ran OK when the mass fractions did not sum to unity.

I think the location in code where the error occurs is the divide in:
thermophysicalModels/reactionThermo/lnInclude/multiComponentMixture.C
void Foam::multiComponentMixture<ThermoType>::correctMa ssFractions()

Dave

Hey Dave,

thank you for your help. your advice fixed THAT problem.

the problem was: the names of my species-files were ch4, o2 and n2 (instead of CH4, O2 and N2) and the mass fraction in the Ydefault file was set to zero. so FOAM couldn't read the files and set all mass fractions like in the Ydefault to zero.

i ran the case and another error came up...

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading chemistry properties


Reading g

Reading thermophysicalProperties
Selecting psiChemistryModel ODEChemistryModel<gasThermoPhysics>
Selecting thermodynamics package hPsiMixtureThermo<reactingMixture<gasThermoPhysics >>
Selecting chemistryReader chemkinReader
Selecting chemistrySolver ode
Selecting ODE solver SIBS
ODEChemistryModel: Number of species = 5 and reactions = 1
Reading field U

Reading/calculating face flux field phi

Creating turbulence model.

Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon


Different dimensions for =
dimensions : [1 -1 -1 0 0 0 0] = [0 2 -1 0 0 0 0]
#0 Foam::error::printStack(Foam::Ostream&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::dimensionSet::operator=(Foam::dimensionSet const&) const in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#3 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::operator=(Foam::tmp<Foam::Geometri cField<double, Foam::fvPatchField, Foam::volMesh> > const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/reactingFoam"
#4 Foam::compressible::RASModels::kEpsilon::kEpsilon( Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#5 Foam::compressible::RASModel::adddictionaryConstru ctorToTable<Foam::compressible::RASModels::kEpsilo n>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#6 Foam::compressible::RASModel::New(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#7 Foam::compressible::turbulenceModel::addturbulence ModelConstructorToTable<Foam::compressible::RASMod el>::NewturbulenceModel(Foam::GeometricField<doubl e, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#8 Foam::compressible::turbulenceModel::New(Foam::Geo metricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libcompressibleTurbulenceModel.so"
#9 main in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/reactingFoam"
#10 __libc_start_main in "/lib/libc.so.6"
#11 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/i386/elf/start.S:122


From function dimensionSet::operator=(const dimensionSet& ds) const
in file dimensionSet/dimensionSet.C at line 143.

FOAM aborting


Dave, do you have an idea what dimensions are meant?

fixed it so far!
thx Dave

Hello everyone,

i am modelling a reactingFoam case for a CH4-air combustion. i ran the case and it was fine. the problem is, that flame-temperatur was very much lower than expected.

my properties for the pre exponential factor A, temperature exponent b and the activation energy are as below:

ELEMENTS
H O C N
END
SPECIE
CH4 O2 N2 CO2 H2O
END
REACTIONS
CH4 + 2O2 => CO2 + 2H2O 6.70091E+12 0.0 4.84149E+04! 1
FORD / CH4 0.2 /
FORD / O2 1.3 /
END

do anyone has an idea what i could have done wrong and how to increase the flame-temperature?

regards,

Ilja

Ilja,

A number of things may effect the flame temperature (and shape):
- turbulence model
- ode solver and settings
- kinetic model
- mesh resolution

The following paper, among other topics, has comparisons between experimental data and OF flame simulations:
http://www.opensourcecfd.com/confere...haiderRehm.pdf

Dave

Hey Dave,

thanks, you halped me again.

But I have problems to ignite my flame. I would like to simulate a flame with specific bc's so I can compare the flame with the measured one.

My temperature BC's are:

fuel inlet: 291 K
pilot: 1880 K
coflow: 294 K

in addition I chose for the internelField 293 K.

If I run the case with this settings the reaction couldn't start. I was thinking that the fuel-inlet-temperature was to low to ignite. the autoignition temperature of CH4 is 823 K. so, I raised the fuel-inlet-temperature to 900 K to proof, if it would ignite. it did. I ve got a flame temperature of 2500 K. I was expecting 2300 K with the fuel-inlet-temperature of 291 K.

is there another possibility for ignition? maybe to configurate a temperature profile at the fuel-inlet, that the flow would have a temperature of 900 K at the first iteration-steps and change after this to 291 K?

best regards,

Ilja

Ilja,

There is a "timeVaryingFixedValue" boundary condition which would allow you to decrease the inlet temperature over time. Did you try igniting by increase the pilot temperature ? There is also an ignition model on the wiki as well as one use in coalChemistryFoam (1.6.x). Also, "funkySetFields" would alllow you to build a numerical "spark" as an initial condition.

Dave

Thanks Dave,

I think I can work with the timeVaryingFixedValue bc.

I changed the ODESolver from SIBS to KRR4 and the flame temperature increased.

there is one think I don't understand. i am running my case without a combustionProperties fine in the /constant folder. seems like this file arrange the ignition:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.0 |
| \\ / A nd | Web: http://www.openfoam.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/

version 1.0;
format ascii;
root "";
case "example";
instance "constant";
local "";
class dictionary;
form dictionary;
object combustionProperties;

// ************************************************** *********************** //

Cmix Cmix [ 0 0 0 0 0 0 0 ] 1.0 ;

ignitionProperties1
{
ignite on;

ignitionPoint ignitionPoint [ 0 1 0 0 0 0 0 ] ( 0.01 0 0 ) ;

timing timing [ 0 0 1 0 0 0 0 ] 0.0e-1 ;

duration duration [ 0 0 1 0 0 0 0 ] 1.0e-0 ;
}

// ************************************************** *********************** //

So I just copied this file from the reactingFoam tutorial and put it in my \constant folder of my case. but I have the feeling that reactingFoam solver doesn't read this file and solve my case like before without this file. do you know how to integrate this file to my case?

and in general: seems like there are a couple op necessary *properties-files line chemestryProperties. if i want to add some additional files like in my case combustionProperties, do i have to declare them, or do the sover read theam automaticlly?

big thanks for your help Dave!!!

regards,

ilja

Ilja,

You will need re-compile with modifications to the reactingFoam source code for an "igniter". If you are using 1.6.x, coalChemistryFoam provides an example of how to do this. You will need modify createFields.H and hEqn.H (which is borrowed from XiFoam). The syntax for the ignition is in the coalChemistry tutorial "constant" directory "enthalpySourceProperties". You could also run coalChemistryFoam and disable the particles and radiation.

Dave

It is a silly quastion, but where i can find these files "createFields.H" and "hEqn.H", i mean in which diractionary? is it the diractionary "/OpenFOAM-1.6/applications/solvers/combustion/reactingFoam"? as you see, i am not very familiar with OF. how could i create a new solver (or modify a existing one)? with which code (and from which files) is OF running a case, if i am typing "reactingFoam" into the terminal?

Regards,

Ilja

Hey Dave,

thanks again for your help. i allready managed to set up an igniter.

there is one think i would like to know. how to reach the steady state? i not really interested in the time variating distribution, but at the time where the temperature is fixed.

is it possible to modify the reactingFoam solver to bring the simulation to the point of a steady state?

best regards,

Ilja

Access to SpecieThermo data
 

Dear All,

Does any of you know to access to the thermodynamic propertie of species such as hi(T) where hi is enthalpy of ith specie and Ti is temprature of cell?
In openFoam-1.5 you can write

hi = chemistry.specieThermo()[i].h(Ti); and it works. See disealengienfoam solver in openfoam-1.5.

However, in OpenFoam-1.6 if you write the same you get psichemistrymodel has no memebr specieThermo.

How can we use specieThermo in OpenFoam-1.6?

I have the same problem. Did you fixed it? I want to access specieThermo.Hc().

hi, me too... do u figure it out?:)

Unfourtunatly, I am still looking..... :mad:

doh!:o Let me know if u fix it.... I'll do the same

sure, I will do

Turbulent reaction info
 

Hey Guys,

Please through some light on the following questions:

1. For coalChemistryFoam during the setup of chemistryProperties file, there is a switch for turbulentReaction on/off; I am wondering how and which files account for turbulence on the reaction rates. can you please send the link of the files. I am using OpenFoam-1.6

2. What are available combustion models in OpenFoam. Are there tutorails for simulating a sample case with different combustion models?

Many thanks in advance.
NirA

Hi NirA,

There are many combustion models in OpenFOAM. You can run the available tutorials in OpenFOAM.

For Q1, I cannot understand what do you mean?

Hi Hassan,

What I meant was in the sub-directory constant/, there is afile chemistryProperties. In the chemsitryProperties, we specify for example that we can use ODEchemistry whichl will use ODE solver. There is also an option of using turbulentReaction.

So I am trying to figure out which library and which files in the solvers or source code modifies the reaction rate due to turbulence?

My chemistryProperties looks as follow:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object chemistryProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
psiChemistryModel ODEChemistryModel<gasThermoPhysics>;
chemistry on;
turbulentReaction on;
chemistrySolver ode;
initialChemicalTimeStep 1e-07;
sequentialCoeffs
{
cTauChem 0.001;
equilibriumRateLimiter off;
}
EulerImplicitCoeffs
{
cTauChem 0.05;
equilibriumRateLimiter off;
}
odeCoeffs
{
ODESolver SIBS;
eps 0.05;
scale 1;
}
//Cmix Cmix [ 0 0 0 0 0 0 0 ] 0.7;
Cmix Cmix [ 0 0 0 0 0 0 0 ] 1;

Hi NirA,

I guess it is the same as reactingFoam which uses Chalmers turbulent combustion model. It calculates the reaction rate based on the chemical time scale (from ODE solver) and the turbulent time scale (kolomogrov time scale) then it calculates K which is a function of Cmix. You can check the chemistry and readchemistryproperties files in the solver folder.
I hope that will answer your equation.

Hi Hassan,

Thanks. Do you know which .C and .H files are involved to calculate these modified reaction rates. I am trying to locate these files and have hard time tracking it back. partly because still I am a novice in C++ and OpenFoam.

Nir

in the solver folder for example (reactingFoam);

OpenFOAM/ applications/ solvers/combustion/ reactingFoam

you will find reactingFoam.C which is the main solver file contains the C++ main function.
you will find also file called chemistry (where are reaction rate calculation) and readchemistryproperties (where turbulent switch exist)

If anything not clear don't hesitate to ask.

Thanks Hassan,

Now I know where the reaction rates are being modified to account for turbulence.


Thanks,
Nir

You can find more about the model in Chalmers PhD thesis on the following link;

http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/docs/
FabianPengKarrholmPhD2008.pdf
NilssonYokohamaOct2006.pdf

you can see also this paper FLAME LIFTOFF IN DIESEL SPRAYS

combustion flow simulation on liquid rocket thrust chambers
 

HI...
My objective is to simulate the realistic flow involving combustion of propellant(i.e.liquid fuel and liquid oxidiser)with cooling ,Thus exploring the capabilities of CFD tool and demonstrating its usefulness in supporting the design and optimization process of modern rocket engines.
is there a facility in fluent 6.3.26 for liquid-liquid impingement flame jet or limited to "liquid fuel and gaseous oxidiser" only?
can i get all the performance parameters, temperature,pressure,spatial spray distribution, droplet diameter,thrust obtianable.....
i was going through fluent tutorials can i solve this as"EQUILIBRIUM CHEMISTRY MODEL of NON PREMIXED,NON ADIABATIC,UNSTEADY LAMINAR FLEMELET with SINGLE MIXTURE FRACTION COMBUSTION PROBLEM?
Please someone suggest me with some idea to slove this problem...
thank you for spending ur precious time.
regards,
Honey.