Does someone has experience with laminar flame modelling in Fluent? Maybe also concerning a methane-air reaction problem?

I tried to simulate the combustion of a houshold burner with a laminar flame. The fluent database reaction parameters for a one-step methane-air reaction modelled by the Arrhenius equation were employed. The solving process was started basing on a converged cold flow solution, with high temperature values (about 2000K) patched, where the flame was supposed to be situated. After an initial starting of the reaction the flame "extinguished" during the iterative solving process, when the temperature was limited to the adiabatic flame temperature. With higher temperature limits the reaction zone moved to the inlet of the model keeping the solution process unconverged.

Neither the patching of products nor the use of a two-step reaction scheme brought success.

I have similar experience with turbulent combustion, not laminar. I have two suggestions which might be helpful for you.

1. Increase wall temperature, e.g., 2000K. If you can get converged solution, decrease wall temperature step by step and finaly set wall boundary condition such as low temperature or given heat flux ......

2. Increase inlet temperature, e.g., 1800K, If you can get converged solution, decrease inlet temperature step by step till your real inlet temperature.

Sincerely, Jinwook

Have you tried FLUENT 5 with coupled solver?

You must use the coupled solver. The segregated solver cannot solve stiff chemistry (unless you solve it unsteady with time steps near the chemical time scale). Recall that the segregated solver solves each equation to convergence in sequence. In chemical reactions, the reaction rate increases exponentially with temperature, and is only limited when the fuel or oxidizer gets depleted. During the (segregated) solution of the temperature equation, the species are held constant, so the temperature either goes to the high limit, or does not ignite if there is insufficient fuel or oxid. Using the coupled solver, one can obtain good solutions with full chemical mechanisms (trick: start with a very small mesh, get a solution, then adapt, and so on until sufficient resolution is obtained). If you use the one or two step chemistry, you should use some modified Cp polynomials to account for the temperature over-prediction due to the neglect of radicals.

Someone else did try it for me but with the same bad result. Have you had positive experience with the coupled solver in a laminar combustion case?

Volker

Thanks for your answer. I think that you are the one who gave the same advice to the German fluent staff? So we (that means Fluent Germany an I) did not try yet the way with the small mesh, we only used the coupled solver on the same mesh where we used the segregated before. As far as I know the procedure was as I described in my first mail (converged cold solution, patching of an ignition zone, starting the solution with small a courant number). The result was unfortunately poor.

Concerning the trick with the small mesh I have some questions: 1. Due to the very thin slit I have to model the mesh is bound to be "big" in the pre-flame zone and if it should be consistent, it is big in the whole domain. If I understood you right, it would be sufficient so have a small mesh in the zone where I expect the flame to be. This may be carried out by a nonconformal interface. But what is the advantage of the small mesh in fact? because 2. what I forgot to mention in my first mail is that fuel and oxidizer are premixed. Does this have an impact on your way of solution? 3. What about the kinetic parameters for methane-air in the fluent database? Do you know the origin and the range of validity?

The advantage of starting on a small mesh is much more rapid solution time. Yes, there will (initially) be large numerical diffusion, but the basic flame shape will be established. Further, you can identify where to adapt the flame. Once a coarse solution is obtained, the adapted (fine) solution converges relatively quickly. I use region adaption. I would recommend starting with a VERY coarse mesh (say 1000 cells - one cell in a nozzle), then continually adapt this. The Chemistry in the Fluent database was gradually accumulated from a number of references, but mostly from the Westbrook-Dryer paper. Note that premixed (laminar) flames are much trickier to solve than non-premixed because you have to resolve the internal flame structure. However, I have obtained a number of good results. Try to use the coupled-implicit solver if you have the memory.

I tried the coupled solver for a turbulent flow with finite-rate kinetics (13 species, multiple steps). It works out fine, but it takes a lot of fine-tune and mesh refinement. Try to start the case with small courant number then gradually increase the speed of time steping. Refine your mesh where the solution needs it (e.g. check temperature gradient, etc.). Good luck.

Does someone has experience with turbulent flame, in chambre combustion in gas turbines

[divyatman]

Hi Volker,

I am trying to simulate interaction of laminar premixed flame with constant temperature wall. I am also facing the same problem of flame extinction with iterations. can you help me out from your experience.