Cyclone separators are characterized by low power usage and great flexibility when compared to other technologies. This is mainly due to the lack of moving parts and geometrical simplicity.

In this tutorial, you will learn how to perform an analysis of a cyclone separator. In particular, how to set up parameters of the discrete phase boundary injection, how to set up Multiphase Particle-in-Cell (MP-PIC) solver and which models to use in your simulation. You will also learn how to post-process results using ParaView.

## Loading Cyclone Geometry

Before you begin, download the cyclone geometry file:

- Click Load STL button
- Select geometry file
`cyclone.stl`

- Click Open

## Scale Geometry

The downloaded geometry was created in milimeters. Scale it to meters:

- Click Option button next to
`cyclone`

STL geometry - Select
**Scale**from the list

- Select uniform scaling
- Set scaling factor
- Click Scale button

## Cyclone Geometry

When loaded, the geometry will appear in the graphics window.

- Click Fit View button to scale the model

## Enable Meshing

Now set meshing parameters for `cyclone`

geometry:

- Go to
**Hex Meshing**panel - Enable meshing on the
`cyclone`

geometry

## Base Mesh Geometry and Boundaries

You will define base mesh and boundaries names and types now:

- Go to
**Base**tab - Define minimum and maximum dimensions of the base box, so that inlet, bottom and top faces of the geometry fall slightly outside the box
- Define number of divisions
- Rename
`X+`

boundary to`inlet`

- Rename
`Z-`

boundary to`bottom`

- Rename
`Z+`

boundary to`top`

- Click on the patch button next to any
`boundary`

and change type to`wall`

- Click on the patch button next to
`top`

and change type to`wall`

## Meshing

Make sure the material point is located inside the geometry:

- Go to
**Point**tab to verify material point location

Everything is set up now for the meshing:

- Go to Mesh tab
- Press Mesh button to start meshing process

## Mesh

The mesh will be displayed in the graphics window.

## Setup Solver

You will use `MPPICFoam`

solver. This is a Lagrangian solver based on Discrete Particle Modelling(DPM) method with Multiphase Particle-in-Cell(MPPIC) collision handling.

- Go to
**SETUP**panel - Select
`Transient`

filter - Select
`Lagrangian`

model - Pick
`MMPICFoam`

from the list of available solvers - Select solver

## Discrete Phase Properties

You will now define properties of the discrete phase:

- Go to
**Discrete Phase**panel - Go to
**Properties**tab - Set density of the discrete phase
- Set packing factor

## Discrete Phase Injection

You will now define injection of discrete phase through `inlet`

boundary. We assume an initial velocity of particles to be 3 m/s. Mass flow rate of the particles is equal to the mass flow rate of the air that will be defined later in the **Boundary Conditions** panel.

- Go to
**Injection**tab - Click Create Boundary Injector
- Set
`Total Mass`

of particles for assumed injection duration to match desired flow rate - Set
`Start Of Injection`

time - Set injection duration longer than expected simulation time
- Select boundary of injection
- Define initial particle velocity

## Discrete Phase Distribution

You will now define a normal distribution of the discrete phase size.

- Go to
**Distribution**tab - Select
`Normal`

distribution - Set minimum particle diameter
- Set maximum particle diameter
- Set variance of the particle diameter
- Set expected value of the particle diameter

## Discrete Phase Models

You will now define particle drag model:

- Go to
**Models**tab - Select
`Sphere drag`

model

## Discrete Phase Solution

You will now define methods of computing and interpolating an average of the Lagrangian phase:

- Go to
**Solution**tab - Select
`Dual`

averaging method - Expand
**Source Terms** - Set
`Semi-Implicit`

discretization of the`U`

term

## Turbulence

For turbulence modeling you will use anisotropic LES model:

- Go to
**Turbulence**panel - Select
`LES`

turbulence modeling - Select
`k Equation`

model - Select
`Anisotropic`

filter

## Transport Properties of Fluid

You will define transport properties of fluid material now:

- Go to
**Transport Propertis**panel - Click Material Database button
- Select
`air`

material - Click Apply

## Boundary Conditions (I)

You will now set bottom boundary to be transmissive for particles:

- Go to
**Boundary Conditions**panel - Select
`bottom`

boundary - Select
**Particles**tab - Change particle interaction to
`Escape`

## Boundary Conditions (II)

You will now set boundary conditions on inlet boundary:

- Select
`inlet`

boundary - Change particle interaction to
`Rebound`

- Change boundary condition for
`inlet`

to`Velocity Inlet`

- Switch to
**Flow**tab - Set velocity at inlet

## Controls

You will now adjust write interval:

- Go to
**Controls**panel - Set write control to
`Run Time`

- Set write interval

## Start Simulation

The case is set up. To run the simulation:

- Go to
**Run**panel - Set
**time step** - Set
**end time** - Run simulation

**End time** in *steady state* simulation represents the number of iterations.

**End time** in *transient* simulation (such as this one) is expressed in seconds.

## Start ParaView

Start ParaView software to display results:

- Go to
**Postprocessing**panel - Start ParaView
- Click Last Frame to select the latest result set
- Uncheck
`lagrangian/kinematicCloud`

region - Click Apply to load results

## Display Stream Lines

You will now plot stream lines:

- Click on Stream Tracer button to add stream lines
- Click Apply

- change coloring variable to
`U.bulk`

## Load geometry (I)

In order to display geometry you can load the same case again into ParaView:

- Select Open from menu File

- Select
`cyclone.foam`

from file selection dialog - Click OK

## Load geometry (II)

You will now select outer surfaces only:

- Check
`Mesh regions`

- Uncheck
`internalMesh`

- Uncheck
`lagrangian/kinematicCloud`

- Click Apply

## Clip geometry

You will clip the geometry:

- Click Clip button
- Select Y Normal
- Click Apply
- Select coloring variable of the clip to
`Solid Color`

## Streamtraces

Results are displayed in the graphics window.

## Display particles (I)

In order to display particles you can load the same case into ParaView once again:

- Select
**Open**from menu**File**

- Select
`cyclone.foam`

from file selection dialog - Click OK

## Display particles (II)

You will now select to display particles only:

- Click
`Mesh regions`

twice to uncheck all boxes - Click Apply

Note that after applying,`lagrangian/kinematicCloud`

will appear on the list of mesh regions. It is checked by default. - Scroll down
**Properties**view - Check file format specification
- Click Apply

- Select particle age as a particle coloring variable
- Click to adjust scale for selected variable

## Display particles (III)

You will now disable stream traces and reduce the opacity of the cyclone geometry:

- Click visibility icon next to
`StreamTracer1`

to hide stream traces - Select
`Clip1`

- Adjust opacity of the geometry

## Results

Results are displayed in the graphics window.

*This concludes this tutorial.*

Note that this tutorial is meant only to demonstrate capabilities of the software and not to solve the problem in the best possible way. Therefore, some assumptions are taken to keep case setup time and computational time low. In particular, to refine the model, one could in first place consider refining the grid and choosing more suitable drag model for the particles (e.g. Ergun-Wen-Yu model). Subsequently, it is worth considering enabling isotropic particle packing, isotropic particle time scale and stochastic isotropy model.