|
[Sponsors] |
How come... the fuel is still igniting at 300K? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
February 18, 2013, 12:17 |
How come... the fuel is still igniting at 300K?
|
#1 |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 28 |
Hello there,
I have started a couple of days ago to work on combustion simulation. i have done recently the tutorial with the liquid fuel combustion using the non-premixed model and pdf table generation. where liquid droplet of c5h12 are injected in an air stream flowing at 650K. until now everything seems ok. Next i wanted to play more with it, so i decided to change both the fuel and the air's temperature and make it 300K. In reality it can happen. no ignition should happen there... just fuel being injected... but when i ran my simulation, i ended up with a flame ! i don't know why , cane someone please explain to me what I've done wrong ... Thanks a lot |
|
February 19, 2013, 10:21 |
|
#2 |
Senior Member
Stuart Buckingham
Join Date: May 2010
Location: United Kingdom
Posts: 267
Rep Power: 25 |
Hey Ali, because you're not a CFD beginner, this may be a stupid question; but did you reinitialise the domain with a constant temp? Or just change the temps of the inlets?
Stu |
|
February 19, 2013, 10:25 |
|
#3 |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 28 |
thanks stuarts for answering,
I didn't patch any region with a specific temperature, also temperature inlet of both fluid is 300 K. Long time no see btw, have you been on vacation ? |
|
February 20, 2013, 09:05 |
Hi dimond
|
#4 |
Senior Member
shoeb khan
Join Date: Nov 2011
Posts: 179
Rep Power: 14 |
Basically what you are saying is not digestive as no reaction should happen at that temperature.
But still i think you should check the equation that you are using in excel or matlab . Plot k(k=k0*e6(-E/R*T) v/s T and see after what temperature the reaction starts . May be something wrong with the equation. Let me know the results. Regards shk |
|
February 20, 2013, 10:49 |
|
#5 |
Member
Jenny
Join Date: Apr 2011
Posts: 34
Rep Power: 15 |
Hi,
Just wondering, did you regenerate your PDF table? It may be because the PDF that is used in the simulation is still from the old temperatures. Good luck, Jenny |
|
February 20, 2013, 11:13 |
|
#6 |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 28 |
Thanks guys for you answer, i made sure it's the new pdf table. both the air and the c5h12 enters at 300K. i didn't use any patch for ignition. could it be that the turbulence brought suffiant energy, or the result are wrong ?
And here is the temperature profile with a maximum of 1560 K: A screenshot at the droplet: Thanks a lot |
|
February 20, 2013, 11:27 |
|
#7 |
Member
Jenny
Join Date: Apr 2011
Posts: 34
Rep Power: 15 |
Hi Ali,
One reason I can think of is that non-premixed combustion model assumes "mix is burnt", that is, reaction occurs once the fuel and oxidiser mix. That is why you don't have to patch a region of high temperature (ignition point not required). You may want to try species transport model (eg. laminar finite-rate chemistry) and compare the results with your non-premixed combustion results to see if they are the same. Good luck, Jenny |
|
February 21, 2013, 23:14 |
|
#9 | |
Senior Member
SSL
Join Date: Oct 2012
Posts: 226
Rep Power: 14 |
Quote:
|
||
February 22, 2013, 08:59 |
|
#10 |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 28 |
My injection setting:
i'm running steady injection . Cone (droplets) with 60 degrees, and a velocity of (20 m/s) about the velocity, i don't know if it's enough. the velocity of the air where the injection starts is 10 m/s. there is also some circulation there. (the magnitude of the velocity in the tutorial is about 80) The mass flow rate is 0.00249 kg/s. i gave it 60 particles. i also set the number of tries to 10. Something i don't understand, it writes in the console that 600 injection are tracked, but 600 escaped. if they escaped, it means they didn't have the time to evaporate, so why is there a flame !!! i could have solved the problem of evaporation by reducing the diameter or increasing the max number of time step. these setting represent a mix of tutorials and my own decision as i just started. i'm not trying to replicate any experiments because simply i don't have any data. if somebody have some realistic setting applicable to combustion chamber please let me know... In general i don't understand why there is a fire at first place. Sorry for asking too much. Thanks a lot |
|
February 22, 2013, 09:15 |
|
#11 |
Senior Member
SSL
Join Date: Oct 2012
Posts: 226
Rep Power: 14 |
Just change injection angle to 30 degree (half angle should be set).
|
|
February 22, 2013, 10:10 |
|
#12 | |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 28 |
Quote:
that has to be applied to start angle and stop angle(air blast atomizer), where you use only half. but i think in my case the angle i gave it is really the one i see in particle plot. (from 0 degres to 90 from x axis to y axis, while the symmetry is along z) |
||
February 22, 2013, 10:26 |
|
#13 |
Senior Member
SSL
Join Date: Oct 2012
Posts: 226
Rep Power: 14 |
I really didn't understand. I have confronted with this problem before. The only problem is with your injection settings. Just change them to see their parameters effects.
|
|
April 27, 2015, 16:38 |
|
#15 |
Member
sanjeet Limbu
Join Date: Mar 2015
Posts: 91
Rep Power: 11 |
Hi
I am trying to do auto ignition for nheptane/Ar/O2/N2 mixture... with adiabatic wall Can anyone suggest how to do ..ignition 1. I tried the laminer - species transport: It shows no rise in temp / pressure (I did the cold flow calculation + patch temp 1400K and species reactant), as there is no combustion even after patch temp... just increase in temperature as in attached snapshot 2. I tried the flame let model in Partially premixed but that show error in the unsteady initialisation that the mixture fraction limit is grater than the largest domain fraction even as I entered 0 in it I tried using the cold flow+ patch at 1400K the body -part in mesh , but no combustion observed , only the temp raised.... I tried then 2900K/40atm patch but no raise observed in products _ CO2 or H20 in mole fraction... In both cases the temperature just climbs to the patch value and there is no temp /pressure raise after than |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
To put fuel mixture initialy for closed vessel combustion | sanjeetlimbu | Fluent Multiphase | 0 | March 27, 2015 16:55 |
modeling empirical fuel in liquid fuel combustion | Hayder Mohammed | FLUENT | 0 | August 7, 2013 03:06 |
burning of solid fuel | lizihujx | FLUENT | 8 | September 19, 2012 08:50 |
How to include new fuel in KIVA4 itape5? | fahdme | OpenFOAM | 0 | August 24, 2011 13:32 |
injection of fuel into tank filled with fuel | mujahid | FLUENT | 1 | February 19, 2004 06:36 |