Hi,

I am currently trying to model the premixed laminar combustion of methane in air over a ceramic plaque burner using the finite rate model in Fluent. Apart from poor convergence, I have the problem that the combustion takes place at the inlet on the upstream side of the burner (and not on the downstream side as it should be). The cold flow simulation without reaction shows good results and converges quite quickly, but as soon as I introduce the reaction I get rubbish. Any suggestions would be welcome.

Volker

are you using segregated or coupled solver ? coupled is required for this kind of analisys. I did lot of simulation with premixed laminar combustion with poor results.

Let me know how you fare. Marc

Thanks for the response!

I have used mainly the segregated solver so far. I have just started trying the coupled solver but I am limited to the over simplified 2d case because our computer system cannot cope with the 3d case for the coupled solver. The 2D case I have tried with the coupled solver produced poor results as well. I have started by calculating the flow field without combustion using the segregated solver and then moved to the coupled solver for the reaction (1 step methane-air), patched a zone where I would expect the flame with a high temperature (2500 K) and started with a small Courand number of 0.05. This did not produce a flame and the residuals are very high. Do you have any idea what I could do to improve it.

Volker Schaika

Yes , you have the same problems I had. First : the first-cold then reaction approach is not always useful, I talked with users that reached good convergence starting with reactions from the beginning

Second, it is important to set kinetic theory for all species ( in the material panel, under FLUID ) for viscosity and thermal conductivity, and set ideal-gas-mixing-law for the MIXTURE viscosity and thermal conductivity ( yes, the same properties !! ) .

Thirdth : set mass diffusivity = kinetic theory set density = incompressible-ideal-gas set thermal diff. coeff. = kinetic theory in the material panel for the MIXTURE properties. Remember CP = mixing law

Try this and let me know, maybe still with first cold then reaction.

Beware that the results will be sligtly over-heated and generally not locally precise. ( low-re simulation are not good with fluent in laminar combustion ). Bye Marc

Marc,

Thanks for the advice. I am finally getting reasonable results. My approach was: As recommended by my university supervisor, I changed the frequency factor and / or the activation energy in the chemical kinetics to see the effects on the combustion using the segregated solver. This produced reasonable reaction zone shapes (A = 1E+9, Ea = 2E+8), but unrealistic values for temperature and species concentrations. Therefore I used these results as an initial solution in the coupled solver. The aforementioned case lifted off the burner, but with A = 1E+10 (instead of the default 2.119E+11) and Ea = 2E+8 (instead of default 2.027E+8), the case converged very slowly (2-d domain with ca. 1000 elements, increasing the Courant number from 0.05 initially gradually to 3)to produce realistic values (species concentration as in complete combustion, flame temperatures around 2000 K). The material settings were as you recommended in your last message. It might not be the best way to tune the reaction mechanism to suit the case, but on the other hand the 1-step mechanism is only a rough approximation to the 'real' kinetics anyway, i.e. it seems quite possible that a different temperature distribution through the flame (likely in a ceramic burner) would produce different overall 1-step kinetics. I'm grateful for any comments on that.

Regards,

Volker

dear sir I am not sure that your approach is correct. Changing the activation energy ( or the arrehnius parameters ) trying to achieve a good flame shape is not guarantee to a phisically correct result. First: note that using a single reaction, whatever parameter you use, FLUENT accomplish the reaction completely ( if you have an air ratio e.g. 0.7 you will have CO2 and H2O according to the complete trasformation of all the methane present) but where and with what heat release this occurs depends on the parameter choosen. My advice is NOT change the parameters of a single reaction mechanism. You can try to use multi-reaction mechanism, and achieve different ( by my experience sliglty different ) behaviour. High temperature in the one reaction mechanism (ORM) is due to the lack of radicals, if you had them, you would have almost right temperature, and a more diffuse flame too as is in the reality. As I checked, the ORM adiabatic flame is around 200 degree higher the real flame temperature, the shape really less diffuse but roughly right. An advice: try fine mesh where you expect the flame front , no cold starting simulation (!!!), patch 2000 K in that zone, courant 1 from the beginning, and stay to that until 500 - 1000 it, then try to rise. Another advice, try to find a reduced mechanism with more reactions. With more reaction I achieved almost perfect results. Let me know if you do not agree with me best wishes

Dear Marc,

I would not claim that my approach guarantees physical correct results but it produces realistic results over a range of equivalence ratios and heat inputs under the conditions of my system.

I certainly agree that using a more detailed mechanism would be preferable. Unfortunately, this is no realistic option for me, as our computer system is struggling with the ORM already. This means that I have to try to achieve some result with the ORM (to a quickly approaching dead-line). The modification of the frequency factor described in my last message was the only way it would work (the default parameters produced a very thin reaction zone directly at the inlet, independent of the grid size).

I think this approach can be justified: The ORM itself is only a very rough approximation of the real chemistry behind methane combustion (e.g GRI use 325 elementary reactions involving 53 species), i.e. the ORM parameters can only be valid for certain conditions or can be the average over a number of conditions (which can be rather diverse). In this case a porous ceramic plaque is used as a burner with some of the combustion taking place inside the pores, i.e. the flame is in contact with a relatively large area of a solid surface. As this can reduce the collision frequency (see also Nakamura et. al, J. of Chem. Eng. of Japan, 26/2, 1993), it seems reasonable that the frequency factor in the reaction mechanism is reduced.

I don't think the kinetic parameters influence the heat release (that is a function of the thermodynamic properties, i.e. the enthalpies) as long as complete combustion is achieved.

Let me know what you think.

Regards,

Volker

hello people !

having switched to the 2 step mechanism for methane combustion in FLUENT, I am forced to come back to this forum again !

the single step with the segregated solver did work for me for a laminar Rijke tube combustion simulation. the current work needs multi-step mechanisms, so I decided to start off with the 2 step model. unlike the 1 step model, I haven't been able to ignite the flame ... even with a 3000 K patch. I must mention that the segregated solver did give me fairly decent solutions (as compared with expermental results).

any suggestions from combustion veterans ?

prateep