thickened flame model
Hi
I came across some previous code on the thickened flame model that uses the following for the source term: Does anyone know what the scalars A, TA, MF etc signify? Thanks, gk namespace Foam { defineTypeNameAndDebug(airmix, 0); addToRunTimeSelectionTable(sourceTerm, airmix, dictionary); airmix::airmix(/*const volScalarField& b*/ const hCombustionThermo& thermo) : sourceTerm(typeName, thermo), A_(readScalar(coeffsDict_.lookup("A"))), TA_(readScalar(coeffsDict_.lookup("TA"))), MF_(readScalar(coeffsDict_.lookup("MF"))), nuF_(readScalar(coeffsDict_.lookup("nuF"))), nuO_(readScalar(coeffsDict_.lookup("nuO"))), phi_(0.0), stOF_(0.0) { dimensionedScalar stof(thermo.lookup("stoichiometricAirFuelMassRatio")); stOF_=stof.value(); if (!thermo_.composition().contains("ft")) { phi_=readScalar(coeffsDict_.lookup("phi")); } } airmix::~airmix() { } void airmix::correct(const volScalarField& T) { const scalar MO2=32; const volScalarField& b_ = thermo_.composition().Y("b"); const volScalarField& rho = //thermo_.rho(); //thermo.rho has uncorrected BC's! Do not use T.db().lookupObject<volScalarField>("rho"); //lookup returns rho field from top level solver if (thermo_.composition().contains("ft")) { const volScalarField& ft=thermo_.composition().Y("ft"); forAll(omega_, I) { scalar maxYF= ft[I]; scalar YF= b_[I]*ft[I] +(1.0  b_[I])*max(thermo_.composition().fres(ft[I], stOF_), 0.0); scalar YO2= 0.233005 * (1.0  ft[I]  (ft[I]  YF)*stOF_); omega_[I]=maxYF>SMALL ? 1e3* // from cgs A_ * nuF_ * MF_ *pow( 1e3*rho[I]*YF / MF_, nuF_ ) // rho is kg/m^3, change to cgs *pow( 1e3*rho[I]*YO2 / MO2, nuO_ ) *exp(TA_/T[I]) /maxYF : 0.0; } forAll(omega_.boundaryField(), bI) forAll(omega_.boundaryField()[bI], fI) { scalar maxYF= ft.boundaryField()[bI][fI]; scalar YF= b_.boundaryField()[bI][fI]*ft.boundaryField()[bI][fI] +(1.0  b_.boundaryField()[bI][fI])* max(thermo_.composition().fres(ft.boundaryField()[bI][fI], stOF_), 0.0); scalar YO2= 0.233005 * (1.0  ft.boundaryField()[bI][fI]  (ft.boundaryField()[bI][fI]  YF)*stOF_); omega_.boundaryField()[bI][fI]=maxYF > SMALL ? 1e3* A_ * nuF_ * MF_ *pow( 1e3*rho.boundaryField()[bI][fI]*YF / MF_, nuF_ ) *pow( 1e3*rho.boundaryField()[bI][fI]*YO2 / MO2, nuO_ ) *exp(TA_/T.boundaryField()[bI][fI]) /maxYF : 0.0; } } else { scalar maxYF=1.0/((stOF_/phi_)+1.0); scalar YLex=1.0  maxYF  stOF_*maxYF; forAll(omega_, I) { scalar YF = maxYF * b_[I]; scalar YO2 = 0.233005 * (1.0  maxYF) * b_[I] + 0.233005 * YLex * (1.0  b_[I]); omega_[I]=1e3* // from cgs A_ * nuF_ * MF_ *pow( 1e3*rho[I]*YF / MF_, nuF_ ) // rho is kg/m^3, change to cgs *pow( 1e3*rho[I]*YO2 / MO2, nuO_ ) *exp(TA_/T[I]) /maxYF; } forAll(omega_.boundaryField(), bI) forAll(omega_.boundaryField()[bI], fI) { scalar YF = maxYF * b_.boundaryField()[bI][fI]; scalar YO2 = 0.233005 * (1.0  maxYF) * b_.boundaryField()[bI][fI] + 0.233005 * YLex * (1.0  b_.boundaryField()[bI][fI]); omega_.boundaryField()[bI][fI]=1e3* A_ * nuF_ * MF_ *pow( 1e3*rho.boundaryField()[bI][fI]*YF / MF_, nuF_ ) *pow( 1e3*rho.boundaryField()[bI][fI]*YO2 / MO2, nuO_ ) *exp(TA_/T.boundaryField()[bI][fI]) /maxYF; } } } } 
Hi,
It seems they refer to this: Wb=−A*[Fuel]^nuF*[O2]^nuO*exp(−TA/T) If so, does anyone know the exact values for propane? Thanks, gk 
Hi,
I know it's been a while, but did you find the answers to your questions? I came across the same code for thickened flame model, and was trying to adapt it to OF2.2 or OF2.3. Any idea on where to start? (XiFoam I thought). Thanks, Remi 
Thought I'd give some feedback on this old post, as I've been working on the TF model recently:
Quote:
The constants refer to: W= A*NuF*MF*[(rho*YF/WF)^NuF]*[(rho*YO/WO)^NuO]*exp(Ta/T) Values for propane are: A=1.65.10^11 cgs Ta=15080K NuF=0.5 NuO=1 WF=44 WO=32 Source: Dynamically thickened flame LES model for premixed and nonpremixed turbulent combustion. By J.P. Legier, T.Poisont and D.Veynante. I have updated the thickened flame model to OF222, and compiled successfully the new solver. However, I encounter a problem when setting NuF to 0.5 : immediate simulation crash: Floating point exception (core dumped) Changing the coefficient to 1 solves the problem, and there seems to be a limit around 0.7. I assume it has to do with the calculation of Omega in airmix.C, but can't find how. Was there any major change from OF16 to OF222 that should be taken care of when adapting an old solver (in mesh, chemistry, units, etc..?). I can send the solver to those interested in this problem. Best, R. 
Hi Remi,
Would you please send me the code on this email (younisengmsu@gmail.com). I'm currently working methane/air combustion in closed channel using TFM in Fluent. Thanks 
1 Attachment(s)
Sure thing Younis.
Little upgrade on the code situation: I located the problem causing the simulation crash, and changed a little the airmix.C file in order to fix it, even though the file itself was well coded originally. I think that at some point, the b field's minimum value might become a negative number ( 1.0e08 or something), thus leading to negative values for species mass fraction, and a NaN value as soon as the term [Fuel]^nuF*[O2]^nuO is calculated, if NuF or NuO are not integers. Thus, to avoid the problem (a real study should be conducted to see where it comes from though..), I added some max functions in the airmix file that has been linked by the original poster, as follow: omega_[I]=maxYF>SMALL ? 1e3* // from cgs A_ * nuF_ * MF_ *pow( max(1e3*rho[I]*YF / MF_,0), nuF_ ) // rho is kg/m^3, change to cgs *pow( max(1e3*rho[I]*YO2 / MO2,0), nuO_ ) *exp(TA_/T[I]) /maxYF : 0.0; Instead of emailing I tried uploading it here, tell me if you got everything. Best, Remi 
Thank you Remi.

TF model
Quote:
I'm also working the premixed methane/air flame propagating in duct using the TF model and flame surface density (FSD) model in Fluent, but it seems that the premixed flame propagating very slow using the TF model, did you meet the same problem? 
Hi Zheng,
Sorry for my late reply. This is due to the turbulent flame speed model which is a function of flow parameters, geometry, initial conditions, and so on. What I know from ANSYS tutorial is the turbulent flame speed has to be set accurately when you work with TFM. Try to use MetghalchiKeck for laminar flame speeds (material>properties>laminar flame speed> MetghalchiKeck>type of fuel you are using. Is the your combustion chamber closed or open/parially open? thanks Y. Najim 
Hi Foamers,
Can someone explain me why in the airmix.C file a 1e+3 conversion is exploited for the preexponential constant A? In my opinion this constant should be proportional to the order of the reaction.. Stefano 
ATF : thermophysicalProperties
Hi All,
I am trying to use ATF model to simulate premixed methane flame. I need to know how to modify the thermophysicalProperties dictionary. I am having some troubles understanding the entry nMoles. Code:
reactants Because I think nMoles has to be 1, considering one mole of reactants is used. Can someone please help me here what is going on with nMoles entry? 
myATF  ftEqn and ft field
Hi remir all,
Does anyone know what exactly is the purpose of ftEqn.H file is. And in the test case that was kindly provided by remir there is a file "ft" What exactly is the purpose of that file? Can someone who has used this solver please help me here. Thanks a lot. 
Hello all,
I will try to address some of the questions above best I can, but I haven't worked on the TFM in a while, so please pardon my lack of memory. The 1e+3 conversion for the preexponential factor is a unit conversion to cgs units. In the original solver when A was defined (user input), the unit was not cgs. In my version of it, it is, so I hardcoded the conversion. Now for ft, it is defined as follow in this portion of the code : if (thermo_.composition().contains("ft")) { const volScalarField& ft=thermo_.composition().Y("ft"); The purpose of the ft file might just be for initialization, have you tried removing it before you run a simulation? ftEqn.H seems to treat the transport equation of a scalar in a turbulent flowfield. The maxYF constant : I don't remember why it's used here, maybe to give some sort of correction depending on the stoecchiometric ratio of air/fuel ? To be investigated further ! The nMoles entry : it is indeed still an unknown for me, have you found a andwer? Now for the values of the TFM coefficients, different choices are possible here, as this is mainly just a curve fitting. I think you can find some of these coeff in Angelberger, C., Veynante, D., Egolfopoulos, F., & Poinsot, T. (1998). Large eddy simulations of combustion instabilities in premixed flames. In Proc. of the Summer Program (pp. 6182).. Also, it is suggested by Westbrook and Dryer (1981) that Ta be kept at the lowest value to assure low stiffness and a thicker reaction zone, hence my choice for a lower Ta = 7048K. For the MF = 1 or 44, have you found any difference in the simulation? Hope it helped a little, good luck. Remi 
Hi remir,
Thanks for your quick response, TA value makes a huge difference, if I use the 15000K value the flame blows off after ignition. But with 7048K value I can get the flame to stay. With 15000K value it is almost impossible to get a stable flame. MF_ , which should be 44 also does not make a huge difference on that backward step flow case. However I need to compare with experimental results. As you said that maxYF term, must be there for some sort of normalization, but not clear what the original author tried to do with it. No i could not find out what nmoles actually does. :( Thanks for the westbrook reference I will look into it. If you understand why they normalize the reaction rate with respect to maxYF please let me know. I ll post the update. Thanks for the westbook reference. 
maxYF and nMoles
Hi Remir,
I think I found the answer to "nMoles" and "maxYF" I explained why nMoles is not equal to one : HTML Code:
http://www.cfdonline.com/Forums/openfoam/175917janafcoefficientgazmixturenmoles.html#post615339 for lean mixtures therefore, so the original code looks to be fine, only problem is fine tuning the Arrehnius coefficients. :mad: 
Hi All
I wanted to use the TFM model (myATF from loaded files by remir) in the recent version of OpenFOAM (v1606+). I am getting below error: Code:
airmix.C: In member function virtual void Foam::airmix::correct(const volScalarField&): I appreciate any suggestion. 
All times are GMT 4. The time now is 00:59. 