'Cyclone separator' simulation project by Steelduines


#1

I created a new simulation project called 'Cyclone separator':

Cyclone separator


More of my public projects can be found here.


#2

Hi @Steelduines, if you need any assistance, feel free to tag me or @psosnowski to continue our discussions from yesterday. Cheers!


#3

Hi @Steelduines,

I took a quick look at your simulation setup and maybe my hints help to run this sim successfully:

  • The medium is air at room temperature and you expect 23m/s at the outlet, so this seems to me that we’ll be far below Mach 0.3, right? So I’d assume that you can model application incompressible, which will be much simpler and faster to simulate
  • Is there a specific reason why you’re using a fixed velocity outlet boundary condition?

Looking forward to see that separator separating :smile:!

Best,

David


#4

@Steelduines,

I gave your model a quick spin, check it out here: https://www.simscale.com/projects/dheiny/cyclone_separator_1

I switched the analysis type to an incompressible turbulent one and drove the flow via an inlet flow BC, hope that makes sense:

I checked a bit on your mesh - great work! One thing to improve would be that you also added layered cells at inlet and outlet faces, where they are actually rather disadvantageous, so working on the mesh, you could remove those faces from the layer refinement but for the first tests, this should be fine.

Hope that helps,

Best,

David


#5

Hi @dheiny,

Thanks for looking at my project.

  • I used a fixed velocity at the outlet because that is how the cyclone works in our machine, a compressor is sucking air from the top tube instead blowing it into the inlet.

  • I want to model the separation of the particles within the cyclone that’s why I want to use a discrete phase model. Can this also be done with an in compressible model?

Best,

Mathijs


#6

Hi Mathijs @Steelduines,

ah I see - sucking the air out of the outlet will work as well, but in general it might be a bit more unstable. And yes, using the discrete phase model should work incompressible as well but my colleague @gholami is the expert on this. Babak, could you take a look here and advice?

In general, I’d definitely start with a simulation without the particles, only a single phase flow to make sure mesh density etc. are all good to go. Then I’d duplicate the sim setup and start one with the discrete phase model.

Looking forward to see the discrete phase sim!

Best,

David


#7

Hi @Steelduines,

cyclone simulation is a fantastic example for using discrete phase model. I’m glad you are planning to use it in your simulation. You already have made good progress with your simulation. However, as DPM might be a little challenging to make stable, I should agree with David’s approach; DPM assumes incompressible flow. Since this is valid for your simulation, once the single phase incompressible simulation is successfully finished, you can focus on the particles only!

We have two cyclone projects, with and without DPM, in our public library. I strongly recommend that you have a look at them to save time on setting up the details. I hope it helps.

Babak


#8

Hi @Steelduines ,

I see that in your latest run “23ms Cyclone” for ‘simulation3’ you got an error shown below:

The ‘Simulation Run Event Log’ states what happened. It says “Maximum execution time exceeded” , which means that your actual simulation “Runtime” of 121 minutes exceeded the “Maximum runtime ( of 7200sec)” set by you under ‘Simulation Control’ ( that is used for capping run times).

So, what you can do is just increase the value from 7200 to a sufficient time for your simulation to finish. Lets say about 18,000 sec. With this value your simulation will finish successfully.

Best,
Ali.


#9

Hi @Steelduines

Also, I see that you are interested in flow simulation with particles. Just follow the sample project that you have imported and setup your case accordingly. I would recommend two things to change compared to the sample project for the particle case:

  1. To optimize the mesh to make it a bit less fine. This would help in reducing compute times for transient case with particles.

  2. To use standard K-Epsilon model ( 3rd option ) instead of the more expensive LES k-Eqn .

This will not change the setup much with respect to the sample project.

If you encounter problems just let me know by tagging me using @Ali_Arafat in the reply.

Best,
Ali.


#10

Hi @Ali_Arafat

I made a setup for the direct phase model. Could you take a quick look at the settings before I run it?
I based the settings on the other direct phase model that you suggested.

Best regards,
Mathijs


#11

Hi @Steelduines

I have taken a look at the setup. The setup seems ok but I would recommend you 2 things to change for a “First Run”.

1- As this is a transient simulation it would be appropriate to use a Coarse mesh instead of a fine one. This would keep the overall run times to feasible limits. For this you may have to use the “SnappyHexMesh” manual setup. Try to keep the mesh around 200,000 cells to 300,000 cells. ( you may also use just 1-2 layers with a finalLayerThickness of 0.5-0.7)

2- Use a low inlet velocity for starting e.g about 5m/s to see that all goes well. Then later we can use Ramping to achieve your goal of 20-23m/s.

The above mentioned suggestions will help keep the auto calculated time step size to feasible value for the simulation. You can use a “Maximal Courant number [-]” of upto 0.7 in “simulation control” under ‘Adjustable timestep’ to further speed things up.

I hope this helps.

Best,
Ali.


#12

Hi @Ali_Arafat

I used a coarser mesh for the direct phase model, but I keep getting an error that courant number exceeded the limit of 1. I tried decreasing the time step but that didn’t help. Do you have any tips to make this model work?

Best regards,

Mathijs


#13

Hi @Steelduines

I will be trying some simulations myself. I will get back to you soon with some updates.

Best,
Ali.


#14

Hi @Steelduines

I have done some test simulations with the standard K-Epsilon and the LES-K model. I modded the geometry a bit to get rid of a sharp face edge on the top casing. The mesh used was of moderate fineness with the “Tetrahedral with prism layers”. ( used only 2 layers to keep it less in size )
I managed to get both the simulations running up till a significant runtime, but the standard K-Epsilon later runs into an error that we are investigating.

I was able to get a Finished simulation run with the LES-K model, which also ran more stably for the moderate mesh. So for now, I suggest you to use LES-K model with a moderate mesh to keep the compute times low ( untill the issue with standard K-Epsilon is fully investigated ).

Also, the solver for the particle analysis involves a " Multiphase Particle-in-Cell (MP-PIC) method for collisional exchange " approach (see ‘Collision Handling and MP-PIC’ in the link). For this approach, it is generally advisable Not to use a very fine mesh and rather a moderate one.

The test simulation parameters are summarized below:

  • Total simulated time 0.6 sec
  • Particle injection duration 0.05 - 0.5 sec
  • Inlet velocity of 5 m/s ( to speed things up via larger time steps )
  • particle size of 0.0001 m and a closed bottom for simplicity.

Below are some snapshots:

.

The project is public and so you can take a look or copy it : https://www.simscale.com/projects/Ali_Arafat/copy_-_particle_flow_analysis_of_a_cyclone_separator

Please try to follow this to get a finished test case yourself. After that you can use the working setup for the full case.

I hope this helps.

Best,
Ali.