2. Create Case
Open SimFlow and create a new case named cyclone_separator
Go to New panel
Provide name cyclone_separator
Click Create Case
3. Import Geometry
After creating case Download GeometryCyclone
Click Import Geometry
Select geometry file cyclone.stl
Click Open
4. 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.
Select mm unit
Click OK button
5. Display Geometry
After importing geometry, it will appear in the 3D window
Click Fit View to zoom out the geometry
6. Meshing Parameters - Cyclone
Now we will set meshing parameters for cyclone geometry
Go to Hex Meshing panel
Enable meshing on the cyclone geometry
7. Base Mesh
We will define the base mesh now
Go to Base tab
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)Define the number of divisions
Division2520100
8. 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
Change the following boundary names accordingly
X+ inlet
Z- bottom
Z+ topDefine boundary types accordingly
X- wall
X+ patch
Y- wall
Y+ wall
Z- wall
Z+ patch
9. Material Point
Make sure the material point is located inside the geometry
Go to Point tab
Make sure that the material point is set accordingly
Material Point000
10. Start Meshing
Now everything is set up, we can begin the meshing process
Go to Mesh tab
Click Mesh to start the meshing process
11. Mesh
After meshing process is finished the mesh should appear in the 3D graphics window
Click Fit View
12. 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.
Go to Setup panel
Select Transient filter
Select Lagrangian model
Pick MPPIC (MMPICFoam) solver
Select solver
13. Discrete Phase - Properties
We will now define properties of the discrete phase
Go to Discrete Phase panel
Set density of the discrete phase
\(\rho_0\) \({\sf [\frac{kg}{m^2}]}\)2500Set packing factor
\(\alpha_{packed}\) \({\sf [-]}\)0.6
14. 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.
Go to Injection tab
Create Boundary Injector
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
15. Discrete Phase - Distribution
We will now define a normal distribution of the discrete phase size
Go to Distribution tab
Set Distribution to Normal
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
16. Discrete Phase - Models
We will now define the particle drag model
Go to Models tab
Select Ergun-Wen-Yu model
17. Discrete Phase - Solution
We will now define methods of computing and interpolating an average of the Lagrangian phase
Go to Solution tab
Set Averaging method to Dual
Expand Source Terms options
Set Semi-Implicit discretization of the U term
18. Turbulence
For turbulence modeling, we will use the LES model
Go to Turbulence panel
Select LES turbulence modeling
Select \(k \; Equation\) model
19. Transport Properties - Fluid
Now we will define the transport properties of fluid material
Go to Transport Properties panel
Click Material Database
Select air material
Click Apply
20. Solution - PIMPLE
To increase the stability of the simulation we will increase the number of pressure corrector iterations
Go to Solution panel
Select the PIMPLE tab
Increase the number of Correctors to 2
21. Boundary Conditions - Bottom (Particles)
Now we will set a bottom boundary to be transmissive for particles
Go to Boundary Conditions panel
Select bottom boundary
Select Particles tab
Change particle interaction to Escape
22. Boundary Conditions - Cyclone (Particles)
Select cyclone boundary
Set following values accordingly
e \({\sf [-]}\)0.97
\(\mu\) \({\sf [-]}\)0.09
23. Boundary Conditions - Inlet (Particles)
We will now set boundary conditions on inlet boundary
Select inlet boundary
Change boundary condition for inlet to Velocity Inlet
Change particle interaction to Rebound
24. Boundary Conditions - Inlet (Flow)
Switch to Flow tab
Set velocity at inlet
Reference Value \({\sf [m/s]}\)20
25. Run - Time Controls
Go to Run panel
Set Simulation Time [s] to 5
Set time step \(\Delta t [s]\) to 1e-04
26. Run - Output
Go to Output tab
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)
27. 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
Switch to CPU tab
Use parallel mode
Increase the Number of processors
Click Run Simulation button
28. Postprocessing - Open ParaView
Open ParaView software to display results
Go to Postprocessing panel
Start ParaView
29. 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.
Select cyclone_separator.foam
Click Apply to import results
Click Last Frame to select the latest result set
Refresh the results
Uncheck lagrangian/kinematicCloud region
Click Apply
30. ParaView - Streamlines
We will now plot streamlines for the fluid region and set the coloring variable to velocity
Select cyclone_separator.foam
Click Stream Tracer button to add streamlines
Click Apply
Change the coloring variable to U.bulk
31. ParaView - Display Geometry
To show the transparent geometry together with the streamlines we will follow below steps:
Select cyclone_separator_foam
Click on the eye next to cyclone_separator_foam
Select Solid Color from the list
Change the opacity in a properties tab to 0.3
32. ParaView - Display Particles (I)
In order to display particles you can import the same case into ParaView once again
Select Open from the top menu
Make sure you are in folder with cyclone_separator_foam case
Select cyclone_separator.foam from file
Click OK
33. ParaView - Display Particles (II)
Now we will select to display particles only
Click Apply
Go to Mesh regions, uncheck all regions and check only lagrangian/kinematicCloud
Click once again Apply to confirm
Change the coloring variable to the age
| Note that after first applying, lagrangian/kinematicCloud will appear on the list of mesh regions. |
34. ParaView - Results
The results are displayed in the graphics window.
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. |
