CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

laminar combustion / methane-air

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   January 10, 2000, 13:16
Default laminar combustion / methane-air
  #1
Volker Pawlik
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   January 10, 2000, 20:19
Default Re: laminar combustion / methane-air
  #2
Jin-Wook LEE
Guest
 
Posts: n/a
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
  Reply With Quote

Old   January 12, 2000, 14:34
Default Re: laminar combustion / methane-air
  #3
Kuochen Tsai
Guest
 
Posts: n/a
Have you tried FLUENT 5 with coupled solver?
  Reply With Quote

Old   January 12, 2000, 17:06
Default Re: laminar combustion / methane-air
  #4
Graham Goldin
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   January 13, 2000, 04:06
Default Re: laminar combustion / methane-air
  #5
Volker Pawlik
Guest
 
Posts: n/a
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
  Reply With Quote

Old   January 13, 2000, 04:36
Default Re: laminar combustion / methane-air
  #6
Volker Pawlik
Guest
 
Posts: n/a
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?
  Reply With Quote

Old   January 13, 2000, 10:15
Default Re: laminar combustion / methane-air
  #7
Graham Goldin
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   January 13, 2000, 10:22
Default Re: laminar combustion / methane-air
  #8
Kuochen Tsai
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   January 24, 2000, 07:33
Default Re: turbulent combustion / methane-air
  #9
karim
Guest
 
Posts: n/a
Does someone has experience with turbulent flame, in chambre combustion in gas turbines
  Reply With Quote

Old   June 29, 2009, 07:47
Default
  #10
New Member
 
divyam
Join Date: Jun 2009
Posts: 7
Rep Power: 8
divyatman is on a distinguished road
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.
divyatman is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Temperature drops in Methane combustion CPRL CD-adapco 0 July 24, 2007 12:56
Methane combustion using PPDF CPRL CD-adapco 0 July 19, 2007 13:28
Boundary Conditions and solver for low Mach laminar air jet fbisetti OpenFOAM Running, Solving & CFD 1 September 13, 2006 12:49
kinetic data for methane air global reaction James FLUENT 0 March 11, 2006 16:33
Pre-heat combustion air Eric FLUENT 1 November 17, 2003 12:36


All times are GMT -4. The time now is 01:25.