CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   combustion study (

L. Li August 9, 2000 13:19

combustion study
Dear all:

Now I am taking the research related combustion using Fluent5.3. I used the eddy-break-up model and PDF model to simulate the combustion of

CH4 and O2, When I finished, I found there are some tolerence between simulation and experiment data, esp. temperature result. I want to know the

critiae of tolerence. Can I correct the simulation data by correction coeffience? Do you know which documents to introduce the comparison the both

result? Thanks.

Maurizio Barbato August 11, 2000 06:15

Re: combustion study
Dear Fluent user,

the test case you are simulationg is a premixed or non premixed combustion case. Dealing with what you say (using PDFs) you are dealing with non premixed combustion. Anyway please let me know more. I have just few comments on your concerns. To reproduce the temperature profiles in a combustion simulation is a very diffcult objective. Many variables play a role. For example, if you are assuming a one step chemistry o fast chemistry , no intermediate products are accounted for (e.g. CO) and you temperature will be higher than in reality.

A further point is that for diffusion flames mixing is the leading process. Therefore if you approach fails in well reproducing the mixing (for example a wrong evaluation of swirl) the temperature distribution will easily go wrong.

Another point is that some of the non-premixed combustion flows are not really steady and an approach based on reynolds averaged equations can fail in reproduce some behaviour reported by experiments (I had this experience more than once due to periodic motion of eddies which where completely "smmothed" by the averaged approach).

Let me know.



L. Li August 11, 2000 07:15

Re: combustion study
Dear Mr. Barbato:

Thank you for your advice.

1)My case is non-premixed combustion and swirl=0. The two inlets are coxial located in symmetry. Yes, I got the result from simulation that is higher than the experiment-- about 1000k in EBU model and about 200k in PDF model. I took the one-step and two-step reaction also. But the result is similar.

2)In experiment, there are some cooling pipes around the furnace to reduce the heat. About 50% heat was released. I don't how to use this condition in simulation.

Please advise for me. Thanks.

Yours, Li

Maurizio Barbato August 11, 2000 10:53

Re: combustion study
Dear Li,

Being a diffusion combustion case I would advise you to use the PDF approach and put apart the Eddy Break Up which, by the its fundations, is intended for premixed flames. The results you have already obtained with the PDF method is not bad. Work on refining the physics representation and modeling. What I mean is, play attention to: - grid refinment: if necessary operate a refinement in the region of strong mixing, - boundary conditions: are they flat profiles or you have already given shaped profiles for the inlet variables? - turbulence model: which model have you chosed (if there are zones of recilculations I would suggest you to use RNG k-epsilon, but may be this is not the case of your geometry) - pdf: I suggest to use beta shaped PDFs.

Concerning the heat release, you can use a non adiabatic approach and set boundary conditions to account for the heat exchange at boundaries. The most simple approach is to set isothermal walls at the temperature you can obtain from your experimental data. This is at lest a first simple way to do it. Furthermore being a furnace,, large part of heat exchange occurs via radiation, therefore to include radiation modeling can help your results to become more representative of the real flow.

Hi hope this helps.



P.S. I will stay at work two hours more, then my holidays start and I will be away all next week.

L. Li August 14, 2000 04:09

Re: combustion study
Dear Barbato:

Thank you for your useful suggestion. I think I get it with your advice. Wish to communicate for further research.



All times are GMT -4. The time now is 16:09.