
[Sponsors] 
March 16, 2001, 04:31 
About Patching an "spark"

#1 
Guest
Posts: n/a

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 coldflow>hotflow simulation, underrelaxation, 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. 

March 16, 2001, 09:32 
Re: About Patching an "spark"

#2 
Guest
Posts: n/a

Hi Harry,
Just a couple of suggestions. 1)What kind of problem do you solve  steadystate 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 nonreacting 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. Cheers, Dmitriy 

March 16, 2001, 22:15 
Re: About Patching an "spark"

#3 
Guest
Posts: n/a

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


March 17, 2001, 11:00 
Re: About Patching an "spark"

#4 
Guest
Posts: n/a

Hi,
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. Regards, Dmitriy 

March 17, 2001, 21:55 
Re: About Patching an "spark"

#5 
Guest
Posts: n/a

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


March 18, 2001, 11:03 
Re: About Patching an "spark"

#6 
Guest
Posts: n/a

Well, I did almost the same. Thanks.
Regards, Dmitriy 

March 19, 2001, 07:53 
Re: About Patching an "spark"

#7 
Guest
Posts: n/a

Hi,
did you use the coupled solver? Further the correct definition of the diffusion coefficients is very important for laminar flames. Volker 

March 20, 2001, 06:08 
Re: About Patching an "spark"

#8 
Guest
Posts: n/a

Hi,Volker:
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(GryDiscreteOrdinate and Nongray DiscreteOrdinate). 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 checkbox). 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. 

March 20, 2001, 11:47 
Re: About Patching an "spark"

#9 
Guest
Posts: n/a

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 nongray gas model (if posible together with a mixture) and define the absorption coeff to be zero. 

March 20, 2001, 23:27 
Re: About Patching an "spark"

#10 
Guest
Posts: n/a

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.


March 21, 2001, 03:16 
Re: About Patching an "spark"

#11 
Guest
Posts: n/a

Hi Harry,
Yes. Have a look to the cfdonline archive referring to the topic "combustion" to find the explanation why. 

March 21, 2001, 04:17 
Re: About Patching an "spark"

#12 
Guest
Posts: n/a

Hi,Volker: Thank you very much. Sincerely yours,Harry.


March 21, 2001, 07:11 
Re: About Patching an "spark"

#13 
Guest
Posts: n/a

Hi, Volker: How are you. I find the topic you posted "laminar combustion/methaneair" in the cfdonline 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.


March 26, 2001, 22:20 
Re: About Patching an "spark"

#14 
Guest
Posts: n/a

Hi,Volker:
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 cfdonline and read the "laminar flamemethane/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. 

March 28, 2001, 06:09 
Re: About Patching an "spark"

#15 
Guest
Posts: n/a

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 email 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 onestep mechanism (coeff. from the fluent database) without radiation was 1. to generate a cold flow solution of the laminar flow field of the 2Dslot 2. patch temperature (about the adiabatic flame temp), and massfractions 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 IBMAIX and the singleprecision solver 5. For mechanisms with more steps I have yet no experience. I will inform you, when I know s.th. 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. 

March 28, 2001, 07:07 
Re: About Patching an "spark"

#16 
Guest
Posts: n/a

Hi,Volker:
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 methaneair, 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. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
2.0.x on Mac OSX  niklas  OpenFOAM Installation on Windows, Mac and other Unsupported Platforms  74  March 28, 2012 16:46 
VOF  Patching  friends.sk  FLUENT  6  April 2, 2010 01:56 
OpenFOAM on MinGW crosscompiler hosted on Linux  allenzhao  OpenFOAM Installation  127  January 30, 2009 20:08 
patching in fluent  P.R.Naren  FLUENT  1  May 14, 2005 01:00 
time dependant patching??  Glenn  FLUENT  0  November 7, 2002 09:59 