CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   Laminar Finite Rate Chemistry - Pre-exponential (

Arun January 20, 2005 15:33

Laminar Finite Rate Chemistry - Pre-exponential
Hello Everyone,

Could someone inform me how to give input for the pre-exponential factor for a complex mechanism in Fluent? Do I need to convert it from gmol/cm3 to kgmol/m3 with the reaction order as powers or do I specify the value which is given in the literature. In the literature the Pre-exponential factor is given as values and all they say is it is consitent with units of concentration (gmol/cm3)^1-m-n where m and n are 1 for an elementary mechanism.

The other problem is that in Fluent when I use the value of Pre-exponential factor as it is in the paper without converting units, it is working. Is this a bug in the code?

Thank you.


cg January 21, 2005 22:22

Re: Laminar Finite Rate Chemistry - Pre-exponentia
Since Fluent uses SI units, you will need to convert pre-exp factors in cgs units. Note also that the pre-exp units depends on the reaction.

The units for molar reaction rate in cgs is mol/cm^3 s. The expression for the reaction rate is

w_dot = A * T^beta * exp(-E/RT) * PROD (conc)^(nu)

In cgs units, the units of concentration is mol/cm^3, which is 1e3 kmol/m^3. So, the formula for the conversion of A is then

A (SI units) = A (cgs units) / 10^(3*(sum_sto-1))

where sum_sto is the sum of the stochiometries of the reactants. In the above example, H+CH3<=>CH4, sum_sto=2, and A (SI units) = 1e-3 A (cgs units). Note that for a reaction 2H+H2O<=>H2+H2O, sum_sto=3, etc.

Fluent will still run without the conversion, but the results will be wrong!

Arun January 24, 2005 11:44

Re: Laminar Finite Rate Chemistry - Pre-exponentia
Hello Cg,

Thanks for your reply. But here is what happens if I implement the conversion.

I do not get the right results. I am studying detonation propagation in a closed tube and I have the CJ conditions (theoritical values) for me to compare with. I get these values only when I use the pre-exponential without the conversion without changing any other parameters. Thats why I am so perplexed. Fluent support is not able to understand my question. Can you throw some light on this matter?

Thanks Arun

cg January 26, 2005 20:49

Re: Laminar Finite Rate Chemistry - Pre-exponentia
Detonations are very tough to model since they are prone to numerical error. You need a lot of resolution behind the shock to resolve the reaction zone, and, if you are using the coupled explicit model you might have numerical errors in the RK integration if your time-step is too large. So, you might have numerical errors which are canceling with your reaction error.

Two things I can think of: 1) Do grid convergence studies on your CJ test 2) Simplify your validation for an ignition problem. You can compare Fluent with say Chemkin to make sure they give identical results on a simpler problem like ignition.

Arun January 27, 2005 13:31

Re: Laminar Finite Rate Chemistry - Pre-exponentia
Hello Cg,

Thanks for your comments. I found out that after doing the conversion for the pre-exponential factor, every different mechanism works for different activation temperature and not by the same temperature and pressure conditions I used for the one-step mechanism. So that was my problem..I could not get the mechanisms going without the correct set of ignition conditions. I am surprised that ignition conditions for 7-step mechanism is different from 19-step mechanism though they all represent the same hydrogen-air fuel mixture. Do you have any comments on this?

And as far as the problem goes, I did a grid convergence check and found minimal variation for dx of 0.25 and 0.5 mm. I also look at my induction length before I start the simulation. I don't know how chemkin works. Do you have an idea what governing equations chemkin solve?

Thanks so much for your inputs and discussions. I really appreciate your responses. Looking forward for your reply. You can also email me at

Regards Arun

vikram June 6, 2010 15:16

Hello Arun,

I was wondering if you could help me with the simulation of detonation in a hydrogen-fueled detonation (pulse) engine using fluent. I am not able to get the required pressure spike for my model. The following are its technical specifications:

The ambient conditions outside the tube are assumed to be 1 bar and 298 K. A high-pressure, high-temperature driver gas (driver pressure, pdriv = 30 p0, and driver temperature, Tdriv = 2500 K) consisting of water vapour is used in a small region next to the closed end of the tube (length of driver gas, Ldriv = 0.005 Lt).

I used Fluent's patch option to patch the driver (H2O) and driven gas (fuel mixture) zones in the cylinder. I am not getting the required pressure spikes for a detonation, though the mixture seems to undergo combustion. I am using a stoichiometric hydrogen-oxygen fuel mixture for simplicity along with inviscid flow conditions. I don't seem to be getting a DDT, though the paper I read guarantees a detonation for the above conditions. Is there something wrong with my species definition? Should I rather use a pressure based solver with a spark ignition system? What reaction mechanism does Fluent use for hydrogen-oxygen combustion? The paper had used a Jachimowski reaction mechanism (23 reactions in all).

I would really appreciate it, if anybody could kindly help me. Thank you for your time.


Vikram. May 3, 2012 02:41

I m modelling cracking reaction in fluent. Basically it is a catalysed reaction. Gas is getting cracked with catalyst. i have taken the laminar finite rate in species transport. In the species transport, when i edit the phases (primary phase) then it shows "number of solid species = zero". But i have one solid species i.e. catalyst. I donot know how to edit this "no of solid species" tab. Could you help me please so that i can get my No. of solid species equal to one

pghoseju August 30, 2012 07:09

I am working on spray combustion. For a particular injection pressure and spray cone angle combustion is happening, but when I reduce the pressure as well as spray cone angle, combustion is happening, but the flame shape is very much unrealistic and the same time particle track lines are also unrealistically haphazard.

Can anybody help me?

All times are GMT -4. The time now is 13:32.