# Number of positions in particle tracking

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

 July 29, 2011, 07:33 Number of positions in particle tracking #1 Member   Sujay Join Date: Apr 2010 Location: Karnataka, India Posts: 41 Rep Power: 9 Sponsored Links I am modeling inert solid particle injection in water. I had specified particle size distribution viz. min, max,mean, std deviation. At the injection area velocity and mass flow rate is specified. It is supposed to calculate number of particle on basis of density provided in material properties and size distribution. What is need to specify number of positions and how to specify ? Sujay

 August 8, 2011, 15:30 #2 New Member   Przemek Join Date: Feb 2010 Location: Warsaw Poland Posts: 25 Rep Power: 9 Hi, CFX computes number of real particles based on mass flow rate, density and sizes distribution. Solving the motion equations for each particle is highly CPU costed so you need to provide number of artificial (let's say numerical) particles which each of them represent a group of real particles going by the same trajectory. The bigger number you provide the more statistically representative solution you get. To find appropriate number of numerical particles you should make a parameter independent study. Regards, Przemek srinidhi4u likes this.

August 9, 2011, 00:19
#3
Member

Sujay
Join Date: Apr 2010
Location: Karnataka, India
Posts: 41
Rep Power: 9
Then why it ask information like mass flow rate and size distribution ? Numbers can be calculated on basis of this information

Please guide me to do parameter independent study for this case

Particle Injection

In present case domain is rectangular tank with inlet at top and outlet at bottom. Particles are injected at inlet. Few particles float to top and leave domain while few are carried away by fluid through outlet.
Attached Files
 Doc1.doc (24.5 KB, 150 views)

Last edited by sujay; August 9, 2011 at 00:41.

 August 9, 2011, 15:05 #4 New Member   Przemek Join Date: Feb 2010 Location: Warsaw Poland Posts: 25 Rep Power: 9 Hi, CFX ask for mass flow and particle size to calculate real (physical) number of particles. Parameter 'Number of Positions' is just a numerical reprezentation. CFX assumes that each numerical particle is a group of real particles bahaving in the same way. But to know how many particles is hiding behind numerical particle you need to provide mass flow and sizes. For example, if from your mass flow and sizes you calculate that you should get 100,000 particles per unit of time and you provide Number of Positions as 100. It means that each numerical paricle is representing 1000 real particles (per unit of time). To make parameter independent study you have to decide what kind of results you would like to get. Then run few cases with different values in Number of Position parameter, and then look when your results are not changing with icrease in this parameter. In other words choose value big enough to not affect your results. Regards, Przemek Julian K. and rockzh like this.

 August 10, 2011, 04:03 #5 New Member   Join Date: Jun 2010 Posts: 21 Rep Power: 9 Sujay, If l the ratio of flow mass flow rate of particles to the to the mass flow rate of fluid is low. Or if you believe that your particles have negligible influence on continous phase, you may choose one way coupled particles on fluid pairs tab. Mass flow definition for one way coupled particles does not effects the solution. You can define any value, out flow mass rate for particles will calculate from ratio between number of particles left domain and entered domain at the post process..

December 5, 2011, 17:58
#6
Member

Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 10
Quote:
 Originally Posted by Batis For example, if from your mass flow and sizes you calculate that you should get 100,000 particles per unit of time and you provide Number of Positions as 100. It means that each numerical paricle is representing 1000 real particles (per unit of time).
Let's assume the following case: the mass of one particles m_p = 1e-9 kg (calculated from diameter and density of the particle). The mass flow rate show be F_m = 1e-3 kg/s. Thus, the particle flow rate would be F_p = F_m/m_p = 1e+6 1/s. If we set the 'Number of Positions' to nop = 100, one numerical particle will represent F_p/nop = 10,000 real particles (per unit of time). Thus, if of nop = 1e+6 1/s, one numerical particle will represent F_p/nop = 1 real particle. In this case, all real particles are actually simulated.

Is this correct? What happens, if nop > 100,000?
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0

Last edited by Julian K.; December 7, 2011 at 09:52.

 December 6, 2011, 18:34 #7 New Member   Przemek Join Date: Feb 2010 Location: Warsaw Poland Posts: 25 Rep Power: 9 Julian, your proceedings is correct but you made a mistake in calculations. Your number of real particles will be 1e6 [1/s], so if you set Number of Positions to 100, each numerical particle will represent 10,000 real particles (per unit of time). In that case if you set 'nop' to 1e6 [1/s] then yes, one numerical particle will represent one real particle but it will have very high CPU cost and it is almost for sure not needed from statistical point of view. Best Regards, Przemek Julian K. and srinidhi4u like this.

December 7, 2011, 09:53
#8
Member

Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 10
Quote:
 Originally Posted by Batis Julian, your proceedings is correct but you made a mistake in calculations. Your number of real particles will be 1e6 [1/s], so if you set Number of Positions to 100, each numerical particle will represent 10,000 real particles (per unit of time). In that case if you set 'nop' to 1e6 [1/s] then yes, one numerical particle will represent one real particle but it will have very high CPU cost and it is almost for sure not needed from statistical point of view. Best Regards, Przemek
Thank you Przemek, I corrected it.
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0

June 4, 2015, 05:55
#9
New Member

GPJ
Join Date: Feb 2015
Posts: 27
Rep Power: 4
Quote:
 Originally Posted by Julian K. Let's assume the following case: the mass of one particles m_p = 1e-9 kg (calculated from diameter and density of the particle). The mass flow rate show be F_m = 1e-3 kg/s. Thus, the particle flow rate would be F_p = F_m/m_p = 1e+6 1/s. If we set the 'Number of Positions' to nop = 100, one numerical particle will represent F_p/nop = 10,000 real particles (per unit of time). Thus, if of nop = 1e+6 1/s, one numerical particle will represent F_p/nop = 1 real particle. In this case, all real particles are actually simulated. Is this correct? What happens, if nop > 100,000?
Hi I am also doing a particle tracking in combustion..I know my total flow rate is 4g/s....Then in particle behaviour is the particle mass flow rate is also 4g/s??
My dia is 400microns...What should be my nop based on your experience The cfx pre i have set is shown in pic
Attached Images
 lox particle.jpg (62.5 KB, 46 views)

 February 8, 2016, 04:48 Particle Transport #10 New Member   Join Date: Feb 2016 Posts: 4 Rep Power: 3 Hello everyone. I am trying to calculate heat transfer from a tube with nano fluid. I set my setup according to your suggestions. However, my particles cant exit from domain. do you have any suggestion for it. Thank you. Mustafa.

 February 8, 2016, 05:38 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,735 Rep Power: 106 To answer your direct question: You will have to post an image of what you are modelling and your CCL for us to help you. And now the bigger question: Why are you modelling nanoparticles with a particle tracking model? Nanoparticles usually have no slip relative to the fluid phase and have problems modelling the huge numbers of particles nanoparticles usually contain, so a lagrangian particle model is not often a good choice. Additional variable and multicomponent fluid models are usually more appropriate.

 February 8, 2016, 08:11 #12 New Member   Join Date: Feb 2016 Posts: 4 Rep Power: 3 Thank you for your quick reply. My geometry is pretty simple, so i want to investigate particle tracking method for nano-fluids. But as you can see in the pic, particles didnt leave domain from the outlet. https://drive.google.com/file/d/0B34...hxcGNTbVE/view

 February 8, 2016, 18:10 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,735 Rep Power: 106 The link does not work. Particle tracking models should go out outlets just fine, so something is weird with your model. Did you consider the bigger question I asked in the previous post?

February 10, 2016, 04:05
#14
New Member

Join Date: Feb 2016
Posts: 4
Rep Power: 3
Yes you are right, multi-phase modelling is a better option. But i want to compare results of particle transport and multi-phase methods. as you can see the pic, although water go out outlets, aluminium particles cant. i tried to add cll files, but system didnt allow. So i attached it as .docx. Thank you.

http://www.cfd-online.com/Forums/att...1&d=1455090463

http://www.cfd-online.com/Forums/att...1&d=1455091005
Attached Images
 particles.JPG (18.7 KB, 42 views) fluid.JPG (28.9 KB, 33 views)
Attached Files
 Re6972_1971404elm_Pn_100000.docx (22.9 KB, 14 views)

 February 10, 2016, 07:06 #15 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,735 Rep Power: 106 I said a multi-component mixture, not a multi-phase flow. Have you looked at how much relative slip your particles are going to have? You will find it is almost zero. Have you looked at the temperature difference between your particles and the fluid? Again, it will be almost nothing. A full-blown multiphase model is not an appropriate model for this type of flow. Regardless - why do you say the particles don't exit the domain? They look like they are exiting the domain to me.

 February 10, 2016, 10:31 #16 New Member   Join Date: Feb 2016 Posts: 4 Rep Power: 3 Thank you. left pic belongs to particles. gray lines represent particles. Because gray lines dont reach to outlet, I doubt. And i computed particle volume fraction at the outlet. it is zero.

 February 10, 2016, 18:21 #17 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,735 Rep Power: 106 Have you looked at the maximum integration time parameters for the particle tracking model? They are probably being stopped due to a termination criteria.

 February 28, 2016, 19:00 particulate flow #18 New Member   demir Join Date: Feb 2016 Posts: 1 Rep Power: 0 I simulate a cyclone with cfx how can I find out how much particulate flow at the outlet

 February 29, 2016, 01:20 #19 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,735 Rep Power: 106 Have a look at the outlet file or use the post processor.

January 10, 2017, 14:09
#20
New Member

cfd_guy
Join Date: Apr 2014
Location: Munich, Germany
Posts: 21
Rep Power: 5
Quote:
 Originally Posted by ghorrocks Have you looked at the maximum integration time parameters for the particle tracking model? They are probably being stopped due to a termination criteria.
Hi Ghorrocks,

Could you please throw some light as to how I could estimate maximum integration time parameters?

I am trying to simulate particles in an inert atmosphere. Image attached.

Thanks.
Attached Images
 2017-01-10_18h20_51.png (58.9 KB, 11 views)

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post parisa- FLUENT 1 August 7, 2012 12:03 parisa- Main CFD Forum 2 June 15, 2011 05:12 scatman CFX 5 May 5, 2011 07:23 DPD CFX 1 February 18, 2011 02:28 Renold FLUENT 0 January 26, 2011 15:23