[usamaperwez]

I am trying to insert massless particle in my model but i am not getting any information how to insert massless particle properties. Can anyone help in this regard.

[usamaperwez]

The problem i am facing is following:
1. how to define the material properties for massless particle.
2. When i try to setup particle tracking in CFX, it requires particle diameter, particle mass flow rate, particle injection properties. Since i am modeling it as massless, how can i define these.

[usamaperwez]

Can anybody help in this regard.

[Gert-Jan]

Massless means that the particles behave like the continuous phase. In fact, their tracks represent the molecules of the continuous phase. So, the density of the particles is equal to the density of the continuous phase. Since the drag must be very smal, pick a very small diameter (1mu) and low weight. And of you go. Don't switch on turbulent dispersion.

[usamaperwez]

what you mean by density of continuous phase?
I am using water as fluid and i will be inserting 5000 massless particle.

what should be particles mass flow rate?
Basically, water is moving at 1.5 mm/s. So how can i define that?

[usamaperwez]

So far following is being setup for massless particle injection:
1. Fluid Pair Model:
Particle coupling: One-way coupling
Drag force: None
Non-drag forces: None

2. Particle Injection Regions
a. Injection vel magnitude: 1.5 mm/s (as per my fluid velocity)
b. Number of Positions
Option: Direct Specification
Number Rateneed to defined)
Particle diameter distribution: specified diameter: 1e-39 micron (due to massless particle)

In material properties of massless particles:
molar mass: 1e-10 kg k/mol
density: 1e-39 kg/m3

At inlet:
it requires particle mass flow rate. what should i specify at that (water inlet velocity is 1.5 mm/s).

Can you advice on improving this model for massless particle

[Gert-Jan]

For velocity you should use zero slip velocity.
You shouldn't take massless literally. Better is "no density difference with continuous phase", i.e. water. So for density particles, you should use the denstiy of water.

[usamaperwez]

Thanks alot for the help.

The model so far is as follow now:

1. Material Properties
Particle density is same as water density.
Will all other material properties of massless particle will be same too?

2. Fluid Basic Settings:
Water as continuous fluid
Massless particle as Particle transport fluid

3. Fluid Pair model:
Particle coupling: one way coupling
Drag Force: None
Non-Drag Force: None

4. At inlet BC (Fluid Value Tab):
Particle Behaviour: on
Mass and Momentum: Zero Slip Velocity
Particle Position: Uniform injection
Particle locations: Random
Number of Positions: Direct Specifications
Number Rate: 50000 [s^-1]
Particle mass flow rate: 0 [kg/s]
Particle Specified Diameter: 0.000001 m

Upto this point, i have model this. Can you specify any mistake in it?

[usamaperwez]

I have following questions:
1. I have set particle mass flow rate as 0 Kg/s. Based on following discussion on old forums:
"In this light, a particle mass flow rate of zero should reduce the source term on the fluid to zero (no particle loading at all)."

Link: https://www.google.com.pk/url?sa=t&r...rT6fF6CM4A7GUL

2. I want to inject 5000 massless particles but with above settings, it is injecting 930 per timestep (timestep is 0.1 s). I have idea of Number of Positions which is also given in older forum as:
"Let's assume the following case: the mass of one particles m_p = 5.23e-16 kg (calculated from diameter= 1 um and density of the particle= 1000 Kg/m3). The fluid mass flow rate be F_m = 2.25e-8 kg/s (inlet vel is 1.5 mm/s). Thus, the particle flow rate would be F_p = F_m/m_p = 4.3e+7 1/s. If we set the 'Number of Positions' to nop = 50000, one numerical particle will represent F_p/nop = 860 real particles (per unit of time). Thus, if of nop = 4.3e+7 1/s, one numerical particle will represent F_p/nop = 1 real particle."

Link: Number of positions in particle tracking

Is this approach correct?

[Gert-Jan]

I don't know if it possible to inject 0 kg/s. Never tried. Looks unrealistic to me.
The number of particles depends on how you specify them. You mention per time step. Do you run transient?

[usamaperwez]

Yes i am running transient case.

In this case, it seems that either it is 0 kg/s or following observation obtained from ANSYS CFX 14.5 Lagrangian Particle Tracking PDF:

Particle number rate = Particle mass flow rate/Particle mass
mass of particle is based on particle density and particle volume (V=4/3*3.14*(r/2)^3). In my case, it is 5.22e-16 Kg.

Now i want to inject 5000 particles/sec, so multiply 5000*5.22e-16=2.61e-12 Kg/s=particle mass flow rate.

Particle number rate=5.22e-16/2.61e-12=5000 1/s.

When i set time step as 0.1, it injects 500 particles per timestep, which totally agree with this calculation.

I have also tried steady state run and yes, it requires only number of injections which is straight forward.
By the way, i have also studied in old CFD-online forum (2001) that to model massless particle take 1e-9 m as particle diameter.

[usamaperwez]

Can you guide me about how to obtain Residence Time Distribution from either "Particle Histogram in Output Control" or CFD Post.

[Gert-Jan]

Is your flow really transient? Or do you think you need a transient simulation in order to obtain a RTD?

[usamaperwez]

It is basically steady state problem but i was just learning the transient particle tracking. Due to your help, it seems that lot of people will benefit from above discussion since i have seen lot of forums in which people have asked this question and noone has given complete answer to this massless particle problem.

Now i am looking for obtaining RTD from particle tracking simulation. Can you guide in that?

[Gert-Jan]

Not for transient. But that is asking for troubles since a transient particle track is a hassle.

For steady state is not so difficult since you can define your histogram in CFX-Pre.

For steady state, it won't be easy to do it afterwards in Post, since you are not able to export solely the time of the particle when leaving the domain through an outlet which is what you need when want to generate a histogram in a speadsheet. Unfortunately, Post can only export ALL timedata on a track. Then using a spreadsheet or home-made-tool you have to look up the end data in the long list of time data.

I have been asking ANSYS for more than 10 years to improve the export capabilities from particles tracks in CFD-Post,. For example, I want CFD-Post to export the particle track number. But that is not possible. Why? Don't ask. Unfortunately, they do not respond on all my request. Maybe we all should demand it.

[Lance]

Originally Posted by Gert-Jan

I have been asking ANSYS for more than 10 years to improve the export capabilities from particles tracks in CFD-Post,. For example, I want CFD-Post to export the particle track number. But that is not possible. Why? Don't ask. Unfortunately, they do not respond on all my request. Maybe we all should demand it.

I have also requested that feature, without any response. It should not be that difficult for ansys to implement.

[usamaperwez]

I have so far created Particle Histogram using Output control:

Histogram Type: Raw
x variable: massless.Particle Time
y variable: massless.Particle Number Rate
Sample location: Outlet

Is it fine to get RTD?

[Gert-Jan]

You just need a list of the end time of all your particles. And from that, create a histogram in e.g. Excel. That would be the most flexible situation. Then you should convince yourself, if the histogram that you obtain makes sense, and if it is realistic. You should ask yourself if the RTD is what you would expect.......

Regarding your setting......I think your Y variable is inappropriate, since this is a constant. I think you don't need a Y variable anyway, but I don't really know. I do not do this on a regular basis. You are the researcher in this respect.

[Gert-Jan]

I looked it up from an old steady state calculation. It reads:

EXPORT RESULTS: Export Results 1
Option = Particle Track Data
EXPORT FORMAT:
Option = CFX CSV
END
EXPORT FREQUENCY:
Option = End of Run
END
EXPORT TRACK DATA:
Option = Selected Variables
Output Boundary = outlet
Output Variables List = particle1.Particle Time
Particle Definition = particle1
END
END


This gave me a list of particle end time.

[usamaperwez]

i have setup my export tab like this but i am not getting CSV file in my directory.
Is there any other way to get that file?