CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Discrete Phase Modeling (DPM) for Liquid Fuel Combustion (http://www.cfd-online.com/Forums/fluent/111880-discrete-phase-modeling-dpm-liquid-fuel-combustion.html)

juzer_700 January 17, 2013 05:14

Discrete Phase Modeling (DPM) for Liquid Fuel Combustion
 
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.

Roberto Meloni January 17, 2013 10:54

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.

juzer_700 January 18, 2013 02:36

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.

Roberto Meloni January 18, 2013 06:16

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.

Yanlong Li January 18, 2013 06:57

I think the particle time step is depend on the mass flow rate of your fule.

juzer_700 January 18, 2013 07:12

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 January 18, 2013 07:15

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 January 18, 2013 07:49

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.

Yanlong Li January 18, 2013 08:43

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.

juzer_700 January 18, 2013 11:14

@Yanlong Li: I am using a Air-blast atomizer. Also, how do you set the Parameter for 'Number of DPM iterations per Continous Phase'??

Yanlong Li January 18, 2013 21:43

Quote:

Originally Posted by Yanlong Li (Post 402648)
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".

juzer_700 January 19, 2013 02:52

My solution is not converging. The residuals go down and then increase and remain constant. Any help would be appreciated.

msaeedsadeghi January 19, 2013 05:26

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.

juzer_700 January 19, 2013 09:19

Quote:

Originally Posted by msaeedsadeghi (Post 402814)
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

msaeedsadeghi January 19, 2013 09:24

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.

sajeesh April 27, 2013 05:36

Quote:

Originally Posted by Yanlong Li (Post 402781)
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

Yanlong Li April 27, 2013 06:22

Quote:

Originally Posted by sajeesh (Post 423485)
the equation is dimensionally wrong
i think

关你鸟事!!!!!!!!!!!!!!

sajeesh April 27, 2013 22:33

i didint get you sir

onlylno August 7, 2013 03:17

Quote:

Originally Posted by Yanlong Li (Post 423492)
关你鸟事!!!!!!!!!!!!!!

Be shame of your self?
顺便说一句你TM真是傻B一个。


All times are GMT -4. The time now is 00:26.