CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   particle time step size, number of time steps in DPMPM (http://www.cfd-online.com/Forums/fluent/101494-particle-time-step-size-number-time-steps-dpmpm.html)

lili May 5, 2012 04:55

particle time step size, number of time steps in DPMPM
 
hi
i want to solve a DPM problem with unsteady particle tracking. in discrete phase model panel what is the "particle time step size (s)" and "number of time steps"?
is "particle time step size" related to length scale/step length factor? I have been confused because I dont know how fluent track particles unsteady in an steady contineous flow field:(
please help.

Amir May 5, 2012 08:31

Dear Leila,

The particle trajectories are computed with lagrangian approach; i.e., particle paths are computed via unsteady integration here which obviously needs time step size and number of them but there is a restriction here that a particle cannot jump over a cell in its path. you can implicitly set time step with specifying length scale or step length factor which is a successive number of iteration that particles remain in one cell; you can also deactivate automation and provide time step size explicitly which suggested in specific goals.

Bests,

lili May 6, 2012 03:05

Dear Amir
As I understand from the help the "length scale" is the distance that the particle will travel before its motion equations are solved again and its trajectory is updated and the "step length factor" is the number of time steps required to traverse the current continuous phase control volume. So why you say "cell"?
And I want to know in discrete phase model panel what is the difference between length scale/step length factor (bellow the tracking parameters) which control time step size and "particle time step size" (bellow particle treatment) which appears when unsteady particle tracking is ticked.
Also in particle treatment field what does "number of time steps" means? In help said "When you increase the Number of Time Steps, the droplets penetrate the domain faster"???


Amir May 6, 2012 07:07

Quote:

Originally Posted by lili (Post 359527)

As I understand from the help the "length scale" is the distance that the particle will travel before its motion equations are solved again and its trajectory is updated and the "step length factor" is the number of time steps required to traverse the current continuous phase control volume. So why you say "cell"?


yes, that's right! the current cell (computational cell) is the current control volume the particle is there.
Quote:

Originally Posted by lili (Post 359527)
And I want to know in discrete phase model panel what is the difference between length scale/step length factor (bellow the tracking parameters) which control time step size and "particle time step size" (bellow particle treatment) which appears when unsteady particle tracking is ticked.

These are 3 different ways for setting particle time step in steady/unsteady tracking. (refer to the unsteady particle tracking section of manual)
Quote:

Originally Posted by lili (Post 359527)
Also in particle treatment field what does "number of time steps" means? In help said "When you increase the Number of Time Steps, the droplets penetrate the domain faster"???

yep, that's the number of particle advancement in the domain. (number of integration)

Bests,

lili May 8, 2012 02:10

Dear Amir
Thanks for your helpful guide. but I cant fully understand the procedure fluent uses to solve a coupled problem in which contineous phase is steady and particle tracking is unsteady. I think fluent first solves the contineous flow field and then in t=0 injection and particle tracking occurs then depend on "Number of contineous phase iteration per DPM iteration" some iteration for contineous phase are done and then again injection. but how long is each injection? I think it is "particle time step size"*"number of time steps" am I right?and another question: what happens if "update DPM sources every flow iteration" is ticked?

Amir May 8, 2012 15:06

Quote:

Originally Posted by lili (Post 359848)
how long is each injection? I think it is "particle time step size"*"number of time steps" am I right?

Exactly, but note that these are not necessarily new injections! these can be advancements of previously injected particles.
Quote:

Originally Posted by lili (Post 359848)
what happens if "update DPM sources every flow iteration" is ticked?

The effects of particles on flow field are computed more realistically in each time step but in steady flow fields it can just affect the required time for convergency.

Bests,

lili May 9, 2012 01:03

hi
yani age "update DPM sources every flow iteration" tick bekhore convegence behtar mishe? ye soale dige: shoma az openfoam chizi midunid? nesbate be fluent che mazaya va eibhaee dare?
thanks

Amir May 9, 2012 10:01

Dear Leila,
Quote:

Originally Posted by lili (Post 360028)
yani age "update DPM sources every flow iteration" tick bekhore convegence behtar mishe?

Generally, It can reduce convergence time but it may cause other issues.
Quote:

Originally Posted by lili (Post 360028)
ye soale dige: shoma az openfoam chizi midunid? nesbate be fluent che mazaya va eibhaee dare?

yes, I've done few projects with it specially in viscoelastic field. it's not very user friendly but you'll like it at last. It's not fair to compare openFOAM with FLUENT :D. OpenFOAM is much more powerful that FLUENT in all aspects and it's also open source.

Bests,

kingpots November 21, 2012 14:27

Dear Amir and Leila ,
The above mentioned clarifications helped me a lot in understanding lots of issues related to the DPM , however i still have some concerns , kindly bear with the following :
- If my injection flow rate is 1.5 g/s and particle time size is 0.001 (unsteady tracking ) No. of time size =1 i.e. the pulse of the injection will be short (1*0.001 ) the start and stop time of the injection was set to 0 -300 sec. and the no. of particles is 60 droplets

1) Fluent at each DPM injection is injecting the 1.5E-3 which is 1.5 *0.001 and this no. is not increasing , why ???

2) As you said (Amir ) the Update DPM option is really affecting the convergence time , but what i don't understand is the relation btw that option and the famous graph of URF interphase exchange terms

3) in the best practice guide : they are saying to reduce the URF of DPM and increase the no of continous iterations per DPM iterations , which is totally contradictory with the 2 way couple strategy and to the above mentioned graph . i.e for the results to take effects URF of DPM should be increased and the no. of iterations to be reduced

Can you please advise , since i can tell that you are seniors in the DPM sub-model
Thanks in advance

ruturaj171 January 24, 2014 08:42

aamir sir can you please tell me what is exact meaning of stop time in the set injection properties in the fluent? for micron size water droplet what should be its value? is it really affecting the simulation results?

Amir January 24, 2014 09:51

Quote:

Originally Posted by ruturaj171 (Post 471604)
aamir sir can you please tell me what is exact meaning of stop time in the set injection properties in the fluent? for micron size water droplet what should be its value? is it really affecting the simulation results?

Hi,

Actually these variables are described in the manual if you can take a look. You can set how the particles are injected in your domain. This happens between "start time" and "stop time"; this is a physical BC regardless of the particle type!

Bests,

ruturaj171 January 24, 2014 13:34

Thank you sir for your quick reply.
Sir my problem is evaporation of 10 micrometer droplet in air (continuous phase). So i did "injection type" as a 'surface' with injection from velocity inlet BC. "the particle type" I have taken as 'inert' and "material" as 'water liquid' then i set point properties. Have set problem correctly? In theory guide of fluent about 'start' and 'stop times' they gven Injections with start and stop times set to
zero will be injected only at the start of the calculation ( t=0).
' still not clear the meaning.
Thank you sir

Amir January 24, 2014 15:51

Quote:

Originally Posted by ruturaj171 (Post 471649)
Thank you sir for your quick reply.
Sir my problem is evaporation of 10 micrometer droplet in air (continuous phase). So i did "injection type" as a 'surface' with injection from velocity inlet BC. "the particle type" I have taken as 'inert' and "material" as 'water liquid' then i set point properties. Have set problem correctly? In theory guide of fluent about 'start' and 'stop times' they gven Injections with start and stop times set to zero will be injected only at the start of the calculation ( t=0).' still not clear the meaning.
Thank you sir

I don't have any idea regarding the evaporating particles. I guess you need to change the type to droplet not inert.
In an unsteady flow, the particles can inject over time with a specified time step. For instance, if you set "start time=5" and "stop time=10", injection of particles starts at t=5 s and continues until t=10 s with specified particle time step.

Bests,

ruturaj171 February 27, 2014 07:43

Amir sir, from your previous posts I understood the exact meaning of 'particle time step size' and 'number of time steps'. About maximum number of steps under tracking parameters I know is 'step length factor * number of control volumes (elements)=maximum number of time steps. Which are these steps? Is there any relationship between particle time step size and maximum number of time steps?
Also suppose in set injection properties we set 'start time=0 sec' and 'stop time =10sec' and if 'particle time step size is 0.1 s' then does it mean 100 iterations per control volume.
In fluent DPM, (for 10 micron droplet case) during iterations , after certain number of continuous phase iterations, there will be 'advancing DPM injections' , so injecting suppose 570 particles with certain mass, is it mean by mass of 570 droplets?

Thank you sir.

Amir February 27, 2014 11:39

Quote:

Originally Posted by ruturaj171 (Post 477091)
Amir sir, from your previous posts I understood the exact meaning of 'particle time step size' and 'number of time steps'. About maximum number of steps under tracking parameters I know is 'step length factor * number of control volumes (elements)=maximum number of time steps. Which are these steps? Is there any relationship between particle time step size and maximum number of time steps?

Actually, what we need in tracking particles are step size and number of steps. When you're setting the particle time step, the step size is specified and the number of steps would be set by considering the current flow field time. However, the time step can be changed if you have decreased the max number of steps as a controlling criterion.
Quote:

Originally Posted by ruturaj171 (Post 477091)
Also suppose in set injection properties we set 'start time=0 sec' and 'stop time =10sec' and if 'particle time step size is 0.1 s' then does it mean 100 iterations per control volume.

Of course not! Injecting and tracking are completely 2 different concepts!
Quote:

Originally Posted by ruturaj171 (Post 477091)
In fluent DPM, (for 10 micron droplet case) during iterations , after certain number of continuous phase iterations, there will be 'advancing DPM injections' , so injecting suppose 570 particles with certain mass, is it mean by mass of 570 droplets?

Depends on the particle properties. If they are droplets, the mass of 570 droplets will be added.

I guess it would be better to take a look at the manual sec. 22.

Bests,

ruturaj171 March 1, 2014 02:41

Thank you sir,
Can you please tell me which manual ? I have 3 guides, user, theory and tutorial of ansys fluent 14.0 but any of these sec.22 is not related with DPM.

Regards

Amir March 1, 2014 04:34

Quote:

Originally Posted by ruturaj171 (Post 477377)
Thank you sir,
Can you please tell me which manual ? I have 3 guides, user, theory and tutorial of ansys fluent 14.0 but any of these sec.22 is not related with DPM.

Regards

I mean the user guide, DPM section. In the manual of FLUENT 6.3, it's sec. 22.

Bests,

ruturaj171 March 17, 2014 03:53

Hi Amir Sir

Sir, if I treat the particles in steady fashion, then does it mean that discrete phase equations which are ODEs with time as independent variable will not be solved?

Also in my cooling of heat sink model with water droplets of 10 micrometer, if I reduce the number of continuous phase iterations then domain is overcooled if I increase those it will not happen, so can say that this particular number will directly proportional to certain region of domian (CV) where evaporation will happen because of particle tracking.....
Sir can you suggest me some books or material regarding DPM as from manual I could not clear totally the processes happening in DPM

Regards

Amir March 17, 2014 06:00

Quote:

Originally Posted by ruturaj171 (Post 480395)
Hi Amir Sir

Sir, if I treat the particles in steady fashion, then does it mean that discrete phase equations which are ODEs with time as independent variable will not be solved?

No! The DPM equations are solved in unsteady fashion, but they can be considered in steady or unsteady flow fields. These two are different.
Quote:

Originally Posted by ruturaj171 (Post 480395)
Also in my cooling of heat sink model with water droplets of 10 micrometer, if I reduce the number of continuous phase iterations then domain is overcooled if I increase those it will not happen, so can say that this particular number will directly proportional to certain region of domian (CV) where evaporation will happen because of particle tracking.....
Sir can you suggest me some books or material regarding DPM as from manual I could not clear totally the processes happening in DPM
Regards

Nope. In each numerical analysis, you should assure the iterations are quite enough and increasing them any further wouldn't change the results. I don't see any proportion ....
You can take a look at any text book in this field; aerosols. For instance, this one:
"Aerosol Technology, William C. Hinds"

Bests,

ruturaj171 April 14, 2014 09:31

Hi sir

In my heat sink cooling problem actually I want relative humidity of 15% at the exit of the sink but I am getting it 7.42% , I tried with different combinitions of particle time step size and number of time steps. In this particular process I have given mass flow rate of 4.22e-7 and stop time of injection as 100s for every combinition, But still my rate of evaporation and hence RH is not increasing. (In my problem the relative reynolds number is 0, air velocity is 1 m/s). Can you suggest me a way to resolve the problem?

Regards
Ruturaj


All times are GMT -4. The time now is 17:31.