Back to all tutorials

# Cyclone Seprator - CFD Simulation SimFlow Tutorial

## 1. Create Case

After opening SimFlow, we will now create a new case cyclone_separator

1. Go to panel

2. Provide name cyclone_separator

3. Click

## 2. Import Geometry

1. Click

2. Select geometry file cyclone.stl

3. Click

## 3. Imported Geometry Units

The STL format does not contain the unit information which are defined during the geometry export. If we do not know the exported unit, we can estimate it based on the total size of the model. It is displayed next to Geometry size label. In our case, the model was created in millimeters.

1. Select mm unit

2. Click button

## 4. Display Geometry

After importing geometry, it will appear in the 3D window

1. Click to zoom out the geometry

## 5. Meshing Parameters - Cyclone

Now we will set meshing parameters for cyclone geometry

1. Go to Hex Meshing panel

2. Enable meshing on the cyclone geometry

## 6. Base Mesh

We will define the base mesh now

1. Go to Base tab

2. Define initial mesh extends
Min $${\sf [m]}$$-0.1-0.1-0.4499
Max $${\sf [m]}$$0.14990.1010.5499
(these dimensions have been set, so that inlet, bottom and top faces of the geometry fall slightly outside the box)

3. Define the number of divisions
Division2520100

## 7. Base Mesh Boundaries

To be able to define different conditions on each boundary of the domain we need to assign an individual name to each side of the base mesh

1. Change the following boundary names accordingly
X+ inlet
Z- bottom
Z+ top

2. Define boundary types accordingly
X- wall
X+ patch
Y- wall
Y+ wall
Z- wall
Z+ patch

## 8. Material Point

Make sure the material point is located inside the geometry

1. Go to Point tab

2. Make sure that the material point is set accordingly
Material Point000

## 9. Start Meshing

Now everything is set up, we can begin the meshing process

1. Go to Mesh tab

2. Click to start the meshing process

## 10. Mesh

After meshing process is finished the mesh should appear in the 3D graphics window

1. Click

## 11. Setup Solver - MPPIC

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

1. Go to Setup panel

2. Select filter

3. Select Lagrangian model

4. Pick MPPIC (MMPICFoam) solver

5. solver

## 12. Discrete Phase - Properties

We will now define properties of the discrete phase

1. Go to Discrete Phase panel

2. Set density of the discrete phase
$$\rho_0$$ $${\sf [\frac{kg}{m^2}]}$$2500

3. Set packing factor
$$\alpha_{packed}$$ $${\sf [-]}$$0.6

## 13. Discrete Phase - Injection

We will now define the injection of the discrete phase through the inlet boundary. 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.

1. Go to Injection tab

2. Create Boundary Injector

3. 45 Set following parameters accordingly
Total Mass $${\sf [kg]}$$1.225
SOI $${\sf [s]}$$1
Duration $${\sf [s]}$$10
Parcels Per Second10000
Boundaryinlet
$$U_0$$ $${\sf [m/s]}$$-300

## 14. Discrete Phase - Distribution

We will now define a normal distribution of the discrete phase size

1. Go to Distribution tab

2. Set Distribution to Normal

3. Set distribution parameters accordingly
Min $${\sf [m]}$$4e-05
Max $${\sf [m]}$$3.6e-04
$$\mu$$ $${\sf [m]}$$5e-05
$$\sigma$$ $${\sf [m]}$$2e-04

## 15. Discrete Phase - Models

We will now define the particle drag model

1. Go to Models tab

2. Select Ergun-Wen-Yu model

## 16. Discrete Phase - Solution

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

1. Go to Solution tab

2. Set Averaging method to Dual

3. Expand Source Terms options

4. Set Semi-Implicit discretization of the U term

## 17. Turbulence

For turbulence modeling, we will use the LES model

1. Go to Turbulence panel

2. Select LES turbulence modeling

3. Select $$k \; Equation$$ model

## 18. Transport Properties - Fluid

Now we will define the transport properties of fluid material

1. Go to Transport Properties panel

2. Click

3. Select air material

4. Click

## 19. Solution - PIMPLE

To increase the stability of the simulation we will increase the number of pressure corrector iterations

1. Go to Solution panel

2. Select the PIMPLE tab

3. Increase the number of Correctors to 2

## 20. Boundary Conditions - Bottom (Particles)

Now we will set a bottom boundary to be transmissive for particles

1. Go to Boundary Conditions panel

2. Select bottom boundary

3. Select Particles tab

4. Change particle interaction to Escape

## 21. Boundary Conditions - Cyclone (Particles)

1. Select cyclone boundary

2. Set following values accordingly
e $${\sf [-]}$$0.97
$$\mu$$ $${\sf [-]}$$0.09

## 22. Boundary Conditions - Inlet (Particles)

We will now set boundary conditions on inlet boundary

1. Select inlet boundary

2. Change boundary condition for inlet to Velocity Inlet

3. Change particle interaction to Rebound

## 23. Boundary Conditions - Inlet (Flow)

1. Switch to Flow tab

2. Set velocity at inlet
Reference Value $${\sf [m/s]}$$20

## 24. Run - Time Controls

1. Go to Run panel

2. Set Simulation Time [s] to 5

3. Set time step $$\Delta t [s]$$ to 1e-04

## 25. Run - Output

1. Go to Output tab

2. Set Write Control Interval [s] to 0.1 seconds
(it will force solver to write results on the hard drive every 0.1 seconds of the simulation)

## 26. Run - CPU

This simulation will require high CPU usage and might take several hours to finish the calculation depending on the machine used. To speed up the calculation process increase the number of CPUs basing on your PC capability. We recommend using at least 4 cores for this tutorial. The free version allows you to use only 2 processors in parallel mode. To get the full version, you can use the contact form to Request 30-day Trial

Estimated computation time for 2 processors: 4 hours

1. Switch to CPU tab

2. Use parallel mode

3. Increase the Number of processors

4. Click button

## 27. Postprocessing - Open ParaView

Open ParaView software to display results

1. Go to Postprocessing panel

2. Start ParaView

## 28. ParaView - Import Results

After opening the ParaView we will import result from the simulation. We will import fluid region and parcels cloud separately to be able to assign them different display properties.

1. Select cyclone_separator.foam

2. Click to import results

3. Click Last Frame to select the latest result set

4. Refresh the results

5. Uncheck lagrangian/kinematicCloud region

6. Click

## 29. ParaView - Streamlines

We will now plot streamlines for the fluid region and set the coloring variable to velocity

1. Select cyclone_separator.foam

2. Click Stream Tracer button to add streamlines

3. Click

4. Change the coloring variable to U.bulk

## 30. ParaView - Display Geometry

To show the transparent geometry together with the streamlines we will follow below steps:

1. Select cyclone_separator_foam

2. Click on the eye next to cyclone_separator_foam

3. Select Solid Color from the list

4. Change the opacity in a properties tab to 0.3

## 31. ParaView - Display Particles (I)

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

1. Select Open from the top menu

2. Make sure you are in folder with cyclone_separator_foam case

3. Select cyclone_separator.foam from file

4. Click

## 32. ParaView - Display Particles (II)

Now we will select to display particles only

1. Click

2. Go to Mesh regions, uncheck all regions and check only lagrangian/kinematicCloud

3. Click once again to confirm

4. Change the coloring variable to the age

 Note that after first applying, lagrangian/kinematicCloud will appear on the list of mesh regions.

## 33. ParaView - Results

The results are displayed in the graphics window.

1. Play with an animation buttons to track the results of analysis

 Note that this tutorial is meant only to demonstrate the 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 the first place consider refining the grid and choosing a more suitable drag model for the particles (e.g. Ergun-Wen-Yu model). Subsequently, it is worth considering enabling isotropic particle packing, isotropic particle timescale, and stochastic isotropy model.