CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   About Patching an "spark" (

Harry Qiu March 16, 2001 04:31

About Patching an "spark"
Hi,Mr or Mrs:

I'm calculating a laminar premixed gas combustion. I have two questions:

(1)I employed the "finite rate reaction model" for simulating gaseous combustion and "DO radiation model" for modeling radiation heat transfer. When I only simulate cold flow, it quite easy to convergence. But it become very difficult(or impossible)to convergence once I add the reaction and radiation, even though I do it according to the FLUENT 5 Documentaton(Two steps cold-flow-->hot-flow simulation, under-relaxation, patching an ignition). Can you tell me whatever other measures I can take for convergence?

(2)When I patch a "spark" in the fluid zone, the position(location) of reaction front is not the same as I expected preveously. So, does the position of the reaction front(laminar premixed combustion) vary with where the "spark" is patched?

Looking forward to your answer! Thank you very much!

Sincerely yours, Harry Qiu.

Dmitriy Makarov March 16, 2001 09:32

Re: About Patching an "spark"
Hi Harry,

Just a couple of suggestions.

1)What kind of problem do you solve - steady-state or transient? If it is steady state, I would prefer lower relaxation coefficients than FLUENT's default (something like 0.125 0.25 for velocity and 0.5 for non-reacting scalars) and for pressure 0.8 (which doesn't play too big role from my experience).

2) Also, if it is pure Arrhenius reaction rate model, it is supposed to have very bad convergence due to its exponential dependence on temperature. And your mesh, probably, needs to resolve laminar flame front thickness with this reaction model (which is of order of 1 mm or less).

Probably, other people can suggest something more.



Harry Qiu March 16, 2001 22:15

Re: About Patching an "spark"
Hi,Dmitriy: Thank you for your answer and help. But is the position of the ignition a key factor for modeling the premixed combustion? Thank you very much. Sincerely yours,Harry Qiu

Dmitriy Makarov March 17, 2001 11:00

Re: About Patching an "spark"

Sorry, I can not describe this question. I didn't model "spark" itself. I believed that part of calculation domain is already filled with hot combustion products (in initial conditions), which generated further reaction and flame front propagation. It is interesting to know how you model spark.



Harry Qiu March 17, 2001 21:55

Re: About Patching an "spark"
Hi,Dmitriy the steps of modeling a spark are as follows: (1)register(or select) some cells in the fluid zone (2)patching hot temperature, certain reactant and productant spices concentration on those selected cells (3)iterate Sincerely, Q

Dmitriy Makarov March 18, 2001 11:03

Re: About Patching an "spark"
Well, I did almost the same. Thanks.



Volker Pawlik March 19, 2001 07:53

Re: About Patching an "spark"

did you use the coupled solver?

Further the correct definition of the diffusion coefficients is very important for laminar flames.


Harry Qiu March 20, 2001 06:08

Re: About Patching an "spark"

Thank you for your help and answer. I guess from your answer that you are expert in the combustion simulation field.

I still have four questions: (1)Whose diffusion coefficients shoud I define?

(2)Where and how to define diffusion coefficients? In DEFINE-->MATERIAL?

(3)There are two DO radiation models(Gry-Discrete-Ordinate and Nongray -Discrete-Ordinate). Which one is applicable(suitable) for flue gas(flame)radiation?

(4)I have tried only to model radiation between the walls, which means radiation of the flue gas is not taken into consideration(disable it in DEFINE-->boudary condition-->fluid zone-->not selecting radiation check-box). But the residual of the DO equation is always zero when the computer started iterating. It seems that the DO equation is not being calculated, Can you tell me why?

looking forward to your answer. Thank you a lot!! Sincerely yours,Harry.

Volker Pawlik March 20, 2001 11:47

Re: About Patching an "spark"
Hi Harry,

I am not the expert you expect me to be. Unfortunately...

But due to a similar problem which I solved together with the Fluent staff I know a little bit about the difficulties which can occur.

My answers:

(1) The diffusion coeff. of your components.

(2) Define them e.g. by kinetic gas theory (see Bird, Stuart, Lightfoot, Transport Phenomena) inside the material panel; Most kin. theory coeff. fortunately are inside the fluent database

(3) if you have co2 and h2o as components you should use the gray gas gas model (wsgm). It calculates the absorption coeff. for you. Otherwise you have to provide one for your domain

(4) use the non-gray gas model (if posible together with a mixture) and define the absorption coeff to be zero.

Harry Qiu March 20, 2001 23:27

Re: About Patching an "spark"
Hi, Volker: Thank you very much. Your answer greatly helps me. For laminar flame, is the coupled solver formulation more appropriate than the segregated solver formulation? Thank you! Sincerely yours, Harry.

Volker Pawlik March 21, 2001 03:16

Re: About Patching an "spark"
Hi Harry,

Yes. Have a look to the cfd-online archive referring to the topic "combustion" to find the explanation why.

Harry Qiu March 21, 2001 04:17

Re: About Patching an "spark"
Hi,Volker: Thank you very much. Sincerely yours,Harry.

Harry Qiu March 21, 2001 07:11

Re: About Patching an "spark"
Hi, Volker: How are you. I find the topic you posted "laminar combustion/methane-air" in the cfd-online archive. Were you simulating the combustion in a porous burner(acttually in one flame pore)at that time? If so, I'm doing the same job as yours now. Untill now, I have get a result only with segregated solver formulation after iterating more than 10,000 times. It is quite difficult to testify if my result is correct or not because the geometry model of the pore is very small(Diameter=1.2mm;Length=12mm),which results in the experimental difficulty. So I'm not sure that the flame(reaction front) is correctly located. But, Anyway the plot of the flame temperature is similar to most papers. If you are interested in it and you don't mind my directly contacting you, I can email you the relevant "Graghic result". Thank you a lot! Sincerely yours, Harry.

Harry Qiu March 26, 2001 22:20

Re: About Patching an "spark"

How are you. I'm modeling the laminar premixed flame of methane/air. I meet the same difficulty(flame extinct) as yours. During the iteration, although it seems that the reaction front might be formed at a certain iteration time, the flame must be extinct if the computer continue to iterate from then on. So personally I think, some heat transfer factors result in flame extinct.

I do have seen the archive of cfd-online and read the "laminar flame-methane/air" in detail and do something(coupled solver, small mesh, grid adaption) suggested by others, but it does't work.

So, could you tell me (1)how did you solve that flame extinct problem? (2)What are key factors to solve this problem? (3)Did you consider the radiation of the flue gas(flame) and the wall? (4)How to define "internal emissivity"( 1 by default) for mixture inlet and outlet?

I'm writing the paper for PH.D.,and very anxius about no applicable result. Can you give me a hand? please.

Thank you very much. Sincerely yours, Harry.

Volker Pawlik March 28, 2001 06:09

Re: About Patching an "spark"
Hello Harry,

excuse me for not answering at once. Yes it would be nice to get an image of a cut through the flame. Please send it to my e-mail address. Where are you doing your Ph.D?

As I already told you, I am also still learning how to model laminar flames and how to produce reasonable results. The way I ,respectively the fluent staff got one result with the one-step mechanism (coeff. from the fluent database) without radiation was

1. to generate a cold flow solution of the laminar flow field of the 2D-slot

2. patch temperature (about the adiabatic flame temp), and mass-fractions for products and educts (=0) to the expected flame zone

3. start with CFL=1 and increase it after some it up to 200

4. maybe you have to use the double precision solver. I had some difficulties in getting the same result as others on a Sun or respectively on NT with IBM-AIX and the single-precision solver

5. For mechanisms with more steps I have yet no experience. I will inform you, when I know new.

6. As I mentioned: Diff. coeff. seem to be very important, since the main problems disappeared after having them defined by kinetic theory. I want to mention that even viscosity and thermal conductivity were defined by kinetic theory. But I don't think that kinetic theory property def. will have succeess over piecewise def. for those two.

Harry Qiu March 28, 2001 07:07

Re: About Patching an "spark"

I'm studying in China(main land), and you? I will email you my modeling result(poor in my mind) as soon as possible. But one more question:

which equation is more apropriate for the laminar premixed combustion of methane-air, the steady equation or unsteady equation? If the unsteady one is better, then what time step(how long) should be specified?

Thank you. Sincerely yours, Harry.

All times are GMT -4. The time now is 21:28.