Hi,Fluent5.4 User:

Now I have a problem about UDF to simulate the reaction pure oxygen and CH4.

I have two choices.The first choice is to define source terms of energy and all kind of species in fluid pannel.

The other choice is to define reaction rate in UDF. Then I choose user_rate in volume reaction rate function term in User_defined function hooks pannel.

Do you think which choice is better?

I am studying TUT 8.in fluent annul, "Chemical Mixing and Gas Combustion". I don't consider the reaction of air and CH4.I just consider the reaction of pure oxygen and CH4.So I remove the N2 from material pannel.I change the air as to oxygen in the boundary of air-inlet.And I use Cp calcualated by mixing law and put the piecewise-polynomials in for each species. I don't change the other model.

When the solution is converged,I found the temperature rised to 4800K.And this is not true.Theoretical values of combustion temperature can be obtained from industry standard thermochemical codes for pure oxygen and CH4.And the temperature is about 2800K.

I've tried everything I can imagine!!!

Would you give me some advice?

Thanks a lot, in advance......

1. Why are you going to use UDF ? Fluent can solve CH4-O2 reaction without any special source and/or UDF. You can use 'finite-rate/eddy-dissipation' or 'mixture-fraction/PDF/Gibb's-Free-Energy-Minimization(so called PDF model)' for CH4-O2 reaction.

2. Why do you think that 4800K is too high ? You are true that the temperature is not so high in the real combustor. But this is because you do not consider 'dissociation and intermediate species/radicals such as OH, O, H, and so on. Temperature in the your system should be rised to 4000~5000K because I think that you did not include the above mentioned concept(including intermediate species/radicals ......). You only included complete combustion. Without including these effect, it is false output if you obtain the result which represents the maximum temperature as 2800K

3. Simply speaking, your result is correct one within your input(within CFD world or mathematical world). I know that this is not correct for the real world. But CFD is not AI(artificail intelgence). It solves the problem according to your input. In other words, your input is not reasonable for the real world.

4. If you want to obtain the result in which the maximum temperature is lower than your current result(4800K), just use PDF model with Gibb's-Free-Energy-Minimization. I can not bguarantee that the maximum temperature is about 2800K, but I guarantee that the maximum temperature is fairly lower than 4800K. But you should include many many possible intermediate species/radicals. For me, sometimes, I include even solid-carbon(soot), C(s), to model the real world.

I hope that it might be helpful to you.

Sincerely, Jinwook

Thank you for your reply.

I also tried PDF combustion model.

But in my main fluid region,I must define a seperated fluid zone,in which I want to add mass source of only one kind of species.But if I choose PDF combustion model,I can only add source of total mass,momentum,ernergy,turbulence kinetic energy,turbulence dissipation rate,mean mixture fraction and mixture fraction variance.

My problem is that how I can just add mass source of only one kind of species in the seperated fluid zone,just as I can when I choose finite rate model and eddy-dissipation model. Using the mixture fraction method, I conserve two scalars, mixture fraction and variance. With finite rate etc. I conserve each species in turn. That is why I can't add a source term in the pdf for a single species. As far as Fluent is concerned, it has a mixture fraction consisting of various components about which it has little information. It only conserves the bulk. It goes outside the main code to solve the mixture fraction composition in the form of lookup tables. So I cannot use PDF combustion model in my work. Now I am trying such reactions: C2H4+O2->CO+H2+H2O H2+O2->2OH OH+H2->O+H2O CO+0.5O2->CO2 H2+O->OH+O OH+OH->H2O and so on.

I choose eddy-disapation combustion model.But I find the contours of temperature and species are not correct.

Do you think I must use UDF to reduce flame temperature?

Would you like to give me some advice? Thank you.

Mark 2001.8.10

Your problem is very difficult for me. I can say only some aspects.

1. 4800K is not so high temperature with complete combustion modeling(e.g., one-step or two-step reaction model).

2. I have not tried yet, but I think that you can not add mass source of only one species when you use PDF combustion model because each species are not independent variable for PDF combustion model.

3. I think that eddy-dissipation model is fairly good approximation for global reaction. But if you want to add minor species, I think that chemical kinetics(finite-rate) should be considered.

Sincerely, Jinwook

Hi,Mr LEE:

Thank you for your reply.

Now I am trying use UDF to simulate my reaction.I define source terms of energy and all kind of species in fluid pannel. 1> I have a problem about my compiled UDF in fluent5.4.

In fluent UDF mannul,it is said "Copy Makefile.udf from the directory shown above to your library drectory (e.g.,libudf), and name it Makefile",and "Copy makefile.udf from the directory shown above to your /src directory, and name it makefile".

But in my path/Fluent.Inc/fluent5.4 /src/,I have just makefile_nt.udf and user_nt.udf.So I consider makefile_nt.udf as Makefile.udf and user_nt.udf as makefile.udf.So I copy makefile_nt.udf to my library directory (e.g.,libudf), and name it Makefile,and copy user_nt.udf to my /src directory,and name it user_nt.

When I Compile or Link my Compiled UDF, I also type the complete path to the library directory. But I get the following error: Opening library "f:\guochuhybrid\wangyou\libudf\ntx86\2d\libudf.dl l"... Error: open_udf_library: couldn't open library: f:\guochuhybrid\ wangyou\libudf\ntx86\2d\libudf.dll Error Object: ()

2> I have another problem,Do I need to set up 2D or 3D directories in my ultra?

3> The last problem is about the unit of pre-exponential factor in Arrhenius expression.

k=A*exp(-E/RT)

The unit of the forward rate constant for reaction k is m^3/(kmol-S).The unit of activation energy for reaction is J/kmol.The unit of universal gas constant is J/(kmol-K).Then E/RT is dmensionless.So the unit of pre-exponential factor(A) is m^3/(kmol-S).

But in fluent reactions pannel, pre-exponential factor(A) is dimensionless.And in literatures,the unit of pre-exponential factor(A) is 1/S.

Would you give me some advice about these?Any ansewer will be welcome.

Thank you.

[kostis217]

the pre-exponential factor units are (kmol/m^3-s) or (kg/m^3-s) see also fluent manual http://aerojet.engr.ucdavis.edu/flue...ug/node605.htm at defining reactions number 6 paragraph.