[pietro_lopo]

Hi guys, i need some help to derive this curve.
I've already simulated the gas flow in my cyclone, then i added the discrete phase (ash-solid, using a Rosin-Rammler distribution). Can someone help me for plotting this curve :
- x-axis: Particle diameter
-y-axis: separation efficiency

[vinerm]

For this, you need to sample the particles at the outlet boundary. Efficiency is not defined within Fluent but it is rather easy. Once you have sampled the data at the outlet boundary, you can load it back, and plot it. To do that, you have to use Reports > Discrete Phase > Sample and for loading and plotting use Reports > Discrete Phase > Histogram. Histogram will display number of particles against their diameter for the boundary that you selected during sampling. Using this data, you can define efficiency.

[pietro_lopo]

Thank you for your prompt reply! but...
I've already tried this but when i plot the histogram the x-axis is full of zeros..
I put in 'variable' : 'diameter', and what am i supposed to chose in weight?
And what i've to chose in options?
i was thinking to calculate my curve using this distributions and this formulas (see the images i attached).
Thank you for your attention to this matter. Best regards!GradeEfficiencyCurve.png

GradeEfficiencyCurve_2.png

[vinerm]

The values displayed are in m. Most likely the diameter is quite small, of the order of microns. Therefore, you will have to either use scientific notation or increase the number of significant digits.

You do not need to select any weight. You can disable weight and percent from options on the left.

[pietro_lopo]

You're a GENIUS! Thanks!
Last questions, i've succesfly plotted the histogram , you can see it in the image, but there is a way to see exactly the values on the y-axis?
I'm so grateful to you!

[vinerm]

Either use a bigger screen or reduce number of significant digits to 0 for x-axis. Another option is to use some external plotting tool, such as Gnuplot or Excel. .dpm file written by Fluent is just a text file. You can load it and plot it outside Fluent as well.

[pietro_lopo]

Understood.
Scuse me if i'm asking you so many things but do you know if is possible to visualize in the same way the inlet particle distribution?

[vinerm]

You can do sampling at any boundary, including inlet, as well as at planes. So, you can create a plane a little downstream of particle injection location and then do a sampling at that plane.

[pietro_lopo]

Sorry i haven't fully understood what youre saying.. the only thing i've been able to do Is to list the injections particles, and the program show in the console all the particles, reporting diameters and other proprieties which are not specified.

[vinerm]

The procedure to be followed is similar to what you did for outlet sampling, except, now you should create a plane using Surface > Plane and this plane should be slightly downstream of the injection location. If you are using surface injection, then you do not need to create any plane. You may directly do sampling using Reports > Sample at the boundary being used for surface injection. This will given you details of all the particles being injected.

[pietro_lopo]

I tried that, i'm using surface injections, but when i try to create the histogram then he gives me an histogram with all zeros values. Like no particles pass from there. Maybe becuase i set reflect in the injections surfaces?

[vinerm]

Yes, that's the reason I suggested creating a plane slightly downstream of the surface being used for injection. Then you will be able to observe all the particles. While sampling, you have to select plane and none of the boundary.

[pietro_lopo]

I have to inserti this new Plane in the initial cad? And so run again the calculation? My simulation Is so heavy, and It tooks much time to iterate. There s a way to do so without run calculation agai?
Thanks, again😂

[vinerm]

Surfaces for post-processing are created within Fluent and do not affect the simulation. You have to use option Surfaces > Plane to create plane and not in the CAD. You won't have to rerun the simulation.

[pietro_lopo]

You've been so helpful to me, i appreciate that but i need some others hint if you can..
I've been able to create a plane for the injections particles, but i'm not sure if it is correct. There's a way to see this plane i created? My geometry isn't so simply and i have to be sure that my particles in inlet crosses this plane only once. (i attached an image of my inlet geometry seen from the above).
However i've another problem, fluent tracked 18210 particles, in wich 12912 are escaped and 5298 incomplete. Running the calculation for a longer time will decrease the incomplete particles?
Thanks again, you're saving me!
Best regards.

[vinerm]

Lagrangian equations have only one independent variable, time, i.e., these equations are always unsteady and solved in that manner. If the particles are not tracked for enough time, then Fluent does not know about their fate and are considered as incomplete. You need to increase the number of steps in the DPM Panel. In steady-state simulation, you would have 50000 as default. You may double it.

If there are a significant number of particles even after increasing number of steps, then it could be due to multiple reasons. One, the continuous flow is not converged. Second, there are recirculation zones in your case and particles are stuck there. There could be more reasons. But the first step you can do is to increase the number of steps.

[pietro_lopo]

Thanks Vinerm! I'll try that!
And for the First question i made? A way to see the plane i created?

[vinerm]

You can display the plane using Mesh Display or any other graphical method, such as, contours.

[pietro_lopo]

Why i have this kind of distribution in the inlet despite i use a rosin-rammler distribution? inlet1particles.jpg

[vinerm]

RR Distribution only specifies the mass fraction held by a certain size. It does not affect the number of particles. That is decided by the number of faces on the surface that is used to inject particles.