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

combustion problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 30, 2000, 15:17
Default combustion problem
  #1
cindy
Guest
 
Posts: n/a
Hi, I am using fluent5 to simulate a combustion process. The fuel is propane and another chemical material. I just tried to use the propane 2 step model to simulate the rich combustion, but the solution wouldn't converge.

For the initial condition, outlet boundary condition, I don't know how to set them. Can you give me any suggestion?

Also, I checked some literature for Westbrook's 2 step kinetic model of propane combustion, the Arrehnius parameters seem different from what are provided by Fluent model. I don't know whether I need to modify the Fluent number or not.

Thank you. Cindy
  Reply With Quote

Old   August 31, 2000, 00:16
Default Re: combustion problem
  #2
Jin-Wook LEE
Guest
 
Posts: n/a
Dear Cindy

1. Convergence : For combustion analysis, I have met convergence problem, like you, for every case. However, I have overcomed the problem for most case, by re-generating grid-net, by adjusting under-relaxation parameters and so on. For example, under-relaxation parameters for species are set to be 1.0 by Fluent 5.x as default values. However, I could have good convergence by using default value ONLY for some case. I usually set lower values and increase slightly after couple of hundreds iterations and eventually to near 1.0. Poor grid-net is also one of source of convergence difficulty. If there is a region where (delx)i/(delx)i-1 >> 1. or <<1, it is very difficult to reduce residual values, especially for pressure residual. In addition, there might be many factors which cause convergence problem. As you might guess, convergence of higher order discretization scheme is more difficult than lower order scheme. RSM is more difficult than k-epsilon. Strong swirl which is generally accompanied to the combustion makes difficulty. So, I start from k-e to RSM(if required), from lower order to higher order, from weak swirl flow to higher swirl, sometimes from lower carlorific value to eventually higher(real) value and so on. You may need couple of try but I guess you should have fairly useful results.

2. Initial condition : I think that it's too difficult question. Unfortunately, I only rely on 'trial & error'.

3. Arrehnius parameters : Most codes, including Fluent, adopt slower rate among chemical kinetics controlled rate(Arrehnius type) and turbulent mixing controlled rate(eddy breakup type). As far as my numerical experience is concerned, sensitivity of Arrehnius parameters is fairly weak than eddy break-up parameters, especially for high temperature application. And, considering that Arrhenius parameters are determined by a kind of curve fitting from experiment of fuel, sometimes two(or more) euuations of a type, A*EXP(-E/RT), suggested by different researchers, are fairly similar even though A and E are different each other. So I recommend that, at first, compare the ploting of two curves, A1*EXP(-E1/RT) and A2*EXP(-E2/RT) by spread sheet calculation. Next, compare CFD results by using two different Arrehinus equations, while maintaining the law, R=min(R1,R2), where R1=rate of chemical kinectics controlled reaction and R2 is that of turbulent mixing controlled reaction. You might have similar results for many combustion application.

Sincerely, Jinwook

  Reply With Quote

Old   August 31, 2000, 07:40
Default Re: combustion problem
  #3
Henrik
Guest
 
Posts: n/a
Regarding Westbrook & Dryer's constants vs. FLUENT values: As far as I recall, Westbrook & Dryer used units of cm and mol, while FLUENT uses m and kmol - if exponents of fuel and oxygen concentration do not add up to 1, constants will be different, because pre-exponential factor is no longer dimensionless. I also think W & D used kcal/mol for activation energies instead of J/kmol - again there will be a difference in numerical values due to use of different units.

Regards,

Henrik
  Reply With Quote

Old   September 1, 2000, 04:14
Default Re: combustion problem
  #4
L. Li
Guest
 
Posts: n/a
i think you will overcome this if you don't use 2 step model. you can initialize the suitable value first. then iterate it.

when i use 2 step model in my combustion case, i still get the divergence result. i think fluent5.x is different with fluent4.x. maybe this is false.

good luck Li
  Reply With Quote

Old   September 4, 2000, 18:54
Default Re: combustion problem
  #5
Maurizio Barbato
Guest
 
Posts: n/a
Hallo,

what Henrik says is correct. Units used by W-D for the source depletion terms: d[C_3H_8]/dt = -A exp(-E/RT)[C_3H_8]^m [O_2]^n are gmole/(cm^3 s). Therefore the units for the preexponential term are:

A = (gmole/cm^3)^(1-m-n) 1/s and for the activation energy (the exponent has to be non dimensional) E = Kcal/gmole

Which can be easily converted to SI units then.

As far as I know A and E values implemented in Fluent for the one step chemistry are coherent with the W-D model. This is not the case for the two steps model.

Cheers

Maurizio
  Reply With Quote

Old   September 4, 2000, 19:00
Default Re: combustion problem
  #6
Maurizio Barbato
Guest
 
Posts: n/a
Hello again,

just a suggestion for the outlet boundary condition: set them as pressure boundary with gauge pressure value equal zero.

Cheers

Maurizio
  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
hel (turbulent viscosity ratio limited) for supersonic combustion problem omar.2002bh FLUENT 2 September 5, 2012 11:04
Problem using EDM for combustion nakul FLUENT 1 August 11, 2011 05:01
A problem with combustion Luk Main CFD Forum 1 April 28, 2008 09:55
Combustion problem rupal CFX 0 April 21, 2008 05:29
problem in incomplete nonpremixed combustion muro FLUENT 0 September 28, 2007 06:54


All times are GMT -4. The time now is 01:20.