[sujay]

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

[Batis]

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

[sujay]

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.

[Batis]

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

[altano]

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..

[Julian K.]

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?

[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

[Julian K.]

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.

[Onig]

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

[mkisman]

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.

[ghorrocks]

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.

[mkisman]

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

[ghorrocks]

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?

[mkisman]

I updated link.
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

[ghorrocks]

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.

[mkisman]

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.

[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.

[nihat]

I simulate a cyclone with cfx how can I find out how much particulate flow at the outlet

[ghorrocks]

Have a look at the outlet file or use the post processor.

[krishna13j]

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.