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

Discrete Phase Modeling (DPM) for Liquid Fuel Combustion

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

Like Tree5Likes
  • 1 Post By juzer_700
  • 1 Post By Roberto Meloni
  • 1 Post By Roberto Meloni
  • 1 Post By msaeedsadeghi
  • 1 Post By msaeedsadeghi

Reply
 
LinkBack Thread Tools Display Modes
Old   January 17, 2013, 05:14
Default Discrete Phase Modeling (DPM) for Liquid Fuel Combustion
  #1
Member
 
Join Date: Apr 2012
Location: Heidenheim
Posts: 51
Rep Power: 5
juzer_700 is on a distinguished road
Hello everyone,

I need some guidance on how to go about modeling liquid fuel (diesel c10h22<df>) in Fluent. I have a gas turbine combustor and I have finished with cold flow analysis with swirler at the inlet.

Now, with non-premixed combustion option, I am generating a PDF table with fuel as c10h22<df>.

I am a bit confused on how to give input parameters in DPM tab.

I am carrying out steady state analysis.

How to estimate or calculate parameters such as:--
1) Number of Continous Phase Iterations per DPM Iteration ???
2) Should be Particle Treatment be unsteady??

Also, I am using a air assisted atomizer.
1) How to estimate number of particle streams??

Any help would be appreciated. Thanks.
pravin zinzala likes this.
juzer_700 is offline   Reply With Quote

Old   January 17, 2013, 10:54
Default
  #2
New Member
 
Roberto Meloni
Join Date: Dec 2012
Posts: 14
Rep Power: 4
Roberto Meloni is on a distinguished road
Hi man.
Few months ago I finished a very similar study on a gas turbine fueled with biodiesel, and I had the same doubts !!! So, I can suggest you somethingh.
First of all, you have to adopt an unsteady analisys to study a spray phenomena; keep attention about the time step size.

As Regards the number of particle streams, more elevated is its number more accourated the analysis of the atomization; usually, I adopted 200/300 particle streams.

As Regards, the DPM sources I always retain the default setting.

By the way, there is a very complete tutorial in Ansys about spray injection.
I hope I helped you.

Best regards.
Rob.
Hayder Mohammed likes this.
Roberto Meloni is offline   Reply With Quote

Old   January 18, 2013, 02:36
Default
  #3
Member
 
Join Date: Apr 2012
Location: Heidenheim
Posts: 51
Rep Power: 5
juzer_700 is on a distinguished road
Thanks Roberto.

I am solving using steady state equations for the continous phase.

For DPM, I am going for unsteady particle tracking.

I wanted to ask in my case, how should I set in the injection panel, the start time and the stop time of injection.

Also, how do I set up,
1) The particle time step size
2) Number of time step

Thanks again.
juzer_700 is offline   Reply With Quote

Old   January 18, 2013, 06:16
Default
  #4
New Member
 
Roberto Meloni
Join Date: Dec 2012
Posts: 14
Rep Power: 4
Roberto Meloni is on a distinguished road
Hi Juzer.
You can set the start time to 0s and the end time 100 s for example: this ensures that the injection never stops during the simulation.

Usually, I set the particle time step size to 0.0001 s and 1 time step.

See you.

R.
Hayder Mohammed likes this.
Roberto Meloni is offline   Reply With Quote

Old   January 18, 2013, 06:57
Default
  #5
Member
 
Yanlong Li
Join Date: Jan 2013
Location: BeiJing
Posts: 47
Rep Power: 4
Yanlong Li is on a distinguished road
I think the particle time step is depend on the mass flow rate of your fule.
Yanlong Li is offline   Reply With Quote

Old   January 18, 2013, 07:12
Default
  #6
Member
 
Join Date: Apr 2012
Location: Heidenheim
Posts: 51
Rep Power: 5
juzer_700 is on a distinguished road
Hi,

My mass flow rate of fuel is 0.00596 kg/s. I am using air assisted atomizer option in FLUENT. How do I determine the particle time step??

Thanks.
juzer_700 is offline   Reply With Quote

Old   January 18, 2013, 07:15
Default
  #7
Member
 
Join Date: Apr 2012
Location: Heidenheim
Posts: 51
Rep Power: 5
juzer_700 is on a distinguished road
Thanks Roberto for the reply.

Yes, when I used stop time as zero, the paricles were injected only during the start of calculation. After that, the temperature field was updated with no further injection of particles.

Later, I used stop time as 100s. Now, for every iteration, particles were injected and I was able to achieve combustion.

Thanks again.
juzer_700 is offline   Reply With Quote

Old   January 18, 2013, 07:49
Default
  #8
Member
 
Join Date: Apr 2012
Location: Heidenheim
Posts: 51
Rep Power: 5
juzer_700 is on a distinguished road
Hi,

I have one more doubt.

Since I am using diesel, it requires a high temperature for the mixture to ignite.

In my experimental setup, I am using a spark ignition source to ignite a local flame and then the main fuel supply is turned on which catches the local flame and then a swirl stabilized flame is achieved.

Now, for my simulation I implemented two methods.

1) While intializing, I selected 'all zones', and under that I set the temperature to 2500K. The mixture did ignite after 80 iterations.

2) During my second simulation, I gave a patch of 2500K under entire zone. The mixutre ignited here as well.

My question is which approach is numerically correct. Am I making a mistake here??

For simulation, air inlet and fuel are both at 300K (same in experiment)

Thanks in advance.
juzer_700 is offline   Reply With Quote

Old   January 18, 2013, 08:43
Default
  #9
Member
 
Yanlong Li
Join Date: Jan 2013
Location: BeiJing
Posts: 47
Rep Power: 4
Yanlong Li is on a distinguished road
Sure,
Particle Time Step = (Q/(4/3*Pi*(d/2)^3)/N)^(-1)
where Pi = 3.14;d is diameter of particle;N is the number of mesh face of your inlet face if you used "surface" type. this is my personal experience.
Yanlong Li is offline   Reply With Quote

Old   January 18, 2013, 11:14
Default
  #10
Member
 
Join Date: Apr 2012
Location: Heidenheim
Posts: 51
Rep Power: 5
juzer_700 is on a distinguished road
@Yanlong Li: I am using a Air-blast atomizer. Also, how do you set the Parameter for 'Number of DPM iterations per Continous Phase'??
juzer_700 is offline   Reply With Quote

Old   January 18, 2013, 21:43
Default
  #11
Member
 
Yanlong Li
Join Date: Jan 2013
Location: BeiJing
Posts: 47
Rep Power: 4
Yanlong Li is on a distinguished road
Quote:
Originally Posted by Yanlong Li View Post
Sure,
Particle Time Step = (Q/(4/3*Pi*(d/2)^3)/N)^(-1)
where Pi = 3.14;d is diameter of particle;N is the number of mesh face of your inlet face if you used "surface" type. this is my personal experience.
first of all, I made a mistake, Particle Time Step = (Q/(4/3*Pi*(d/2)^3)/density/N)^(-1)
where density is bubble's

secondary, You do not have to set it, It is 10 times of the "Max Iterations/Time Step".
Yanlong Li is offline   Reply With Quote

Old   January 19, 2013, 02:52
Default
  #12
Member
 
Join Date: Apr 2012
Location: Heidenheim
Posts: 51
Rep Power: 5
juzer_700 is on a distinguished road
My solution is not converging. The residuals go down and then increase and remain constant. Any help would be appreciated.
juzer_700 is offline   Reply With Quote

Old   January 19, 2013, 05:26
Default
  #13
Senior Member
 
SSL
Join Date: Oct 2012
Posts: 227
Rep Power: 5
msaeedsadeghi is on a distinguished road
I have modeled liquid fuel spray combustion so many times (Gasoil, HFO).
It is better to start your simulation with the simplest ones.
If you have enabled breakup, set injection start time=0 and stop time=10000 (high, not important).
Increase continous phase iteration per DPM to 100, if continous phase is complex and is not converging well.
Decrease URF of continuity, turbulence and energy.
Which combustion model are you using? I do prefer Non-Premixed combustion.
Also P1 radiation model is the best at the start up.
Hayder Mohammed likes this.
msaeedsadeghi is offline   Reply With Quote

Old   January 19, 2013, 09:19
Default
  #14
Member
 
Join Date: Apr 2012
Location: Heidenheim
Posts: 51
Rep Power: 5
juzer_700 is on a distinguished road
Quote:
Originally Posted by msaeedsadeghi View Post
I have modeled liquid fuel spray combustion so many times (Gasoil, HFO).
It is better to start your simulation with the simplest ones.
If you have enabled breakup, set injection start time=0 and stop time=10000 (high, not important).
Increase continous phase iteration per DPM to 100, if continous phase is complex and is not converging well.
Decrease URF of continuity, turbulence and energy.
Which combustion model are you using? I do prefer Non-Premixed combustion.
Also P1 radiation model is the best at the start up.
First of all, thanks for replying.

My geometry consists of a combustor with a swirler (Swirl No. 0.56).
I am using non-premix combustion with equilibrium method. I am generating PDF taking c10h22<df> (diesel) as fuel with mole fraction 1 and in oxidizer (Mole fraction of O2 as 0.21 and of N2 as 0.79).

During my initial simulations do I need to consider heat loss from walls. I am giving default values for combustor wall. Am I correct??

Also, what should be the value of rich flammability limit?

Thanks
juzer_700 is offline   Reply With Quote

Old   January 19, 2013, 09:24
Default
  #15
Senior Member
 
SSL
Join Date: Oct 2012
Posts: 227
Rep Power: 5
msaeedsadeghi is on a distinguished road
Wall condition should be real. Try convection.
Forget flameability limit. It should just be at the range, fluent will show an error message if was not in the range.
Hayder Mohammed likes this.
msaeedsadeghi is offline   Reply With Quote

Old   April 27, 2013, 05:36
Default
  #16
Member
 
sajeesh
Join Date: Feb 2013
Posts: 52
Rep Power: 4
sajeesh is on a distinguished road
Quote:
Originally Posted by Yanlong Li View Post
first of all, I made a mistake, Particle Time Step = (Q/(4/3*Pi*(d/2)^3)/density/N)^(-1)
where density is bubble's

secondary, You do not have to set it, It is 10 times of the "Max Iterations/Time Step".

The equation is dimensionally wrong
i think
sajeesh is offline   Reply With Quote

Old   April 27, 2013, 06:22
Default
  #17
Member
 
Yanlong Li
Join Date: Jan 2013
Location: BeiJing
Posts: 47
Rep Power: 4
Yanlong Li is on a distinguished road
Quote:
Originally Posted by sajeesh View Post
the equation is dimensionally wrong
i think
关你鸟事!!!!!!!!!!!!!!
Yanlong Li is offline   Reply With Quote

Old   April 27, 2013, 22:33
Default
  #18
Member
 
sajeesh
Join Date: Feb 2013
Posts: 52
Rep Power: 4
sajeesh is on a distinguished road
i didint get you sir
sajeesh is offline   Reply With Quote

Old   August 7, 2013, 03:17
Default
  #19
New Member
 
jieyu
Join Date: Jul 2013
Posts: 18
Rep Power: 4
onlylno is on a distinguished road
Quote:
Originally Posted by Yanlong Li View Post
关你鸟事!!!!!!!!!!!!!!
Be shame of your self?
顺便说一句你TM真是傻B一个。
onlylno 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
Discrete phase modeling on porous media magnounibo FLUENT 0 April 9, 2009 08:18
uncoupled discrete phase calculations AMV FLUENT 0 December 3, 2003 08:21
Discrete Phase Modeling revanth FLUENT 8 July 18, 2002 05:30
Discrete Phase Modeling Chris FLUENT 0 November 20, 2000 14:08
Discrete Phase Modeling Fred Kang FLUENT 3 October 18, 2000 10:23


All times are GMT -4. The time now is 14:07.