3.5. Three-dimensional fluidized bed¶
This tutorial shows how to create a three dimensional fluidized bed simulation using the two-fluid model (TFM) and the discrete element model (DEM). The model setup is:
Property |
Value |
---|---|
geometry |
10 cm diameter x 40 cm |
mesh |
20 x 60 x 20 |
solid diameter |
200 microns (\(200 \times 10^{-6}\) m) |
solid density |
2500 kg/m2 |
gas velocity |
0.25 m/s |
temperature |
298 K |
pressure |
101325 Pa |
3.5.1. Create a new project¶
On the main menu, select
New project
Create a new project by double-clicking on “Blank” template.
Enter a project name and browse to a location for the new project.
When prompted to enable SMS workflow, answer No, we will use the standard workflow for this tutorial.
3.5.2. Select model parameters¶
On the Model
pane:
Enter a descriptive text in the
Description
fieldSelect “Two-Fluid Model (MFiX-TFM)” in the
Solver
drop-down menu.
3.5.3. Enter the geometry¶
On the Geometry
pane:
Create the cylindrical geometry by pressing the
Add Geometry
button ->Primitives
->cylinder
Enter
40/100
meters for the cylinder heightEnter
10/2/100
meters for the cylinder radiusEnter
30
for the cylinder resolutionPress the autosize button to fit the domain extents to the geometry
Extend the height of the cylinder by adding
0.1
meters. This will hang the stl file outside of the domain, allowing for a sharp and clean cut.Flip the normals by clicking the button and selecting the
flip normals
filter
3.5.4. Enter the mesh¶
On the Mesh
pane:
On the
Background
sub-pane
Enter
20
for the x cell valueEnter
60
for the y cell valueEnter
20
for the z cell value
Note
This is a fairly coarse grid for a TFM simulation. After completing this tutorial, try increasing the grid resolution to better resolve the bubbles.
3.5.5. Create regions for initial and boundary condition specification¶
Select the Regions
pane. By default, a region that covers the entire domain
is already defined. This is typically used to initialize the flow field and
visualize the results.
Click the (all) button to create a new region to be used for the bed initial condition.
Enter a name for the region in the
Name
field (“bed”)Change the color by pressing the
Color
buttonEnter
0
in theTo Y
field
Click the (bottom) button to create a new region to be used by the gas inlet boundary condition.
Enter a name for the region in the
Name
field (“inlet”)
Click the (top) button to create a new region to be used by the pressure outlet boundary condition.
Enter a name for the region in the
Name
field (“outlet”)
Click the (all) button to create a new region to be used to select the walls.
Enter a name for the region in the
Name
field (“walls”)Click the
Select facets
box. The region type should change from “box” to “STL”.
All the facets of the cylinder should now be selected. Since the cylinder is outside the domain extents, normal cells (i.e. not cut-cells) will be placed at the outlet and inlet. This allows for the standard boundary conditions to be applied.
3.5.6. Create a solid¶
On the Solids
pane:
3.5.7. Create Initial Conditions¶
On the Initial conditions
pane:
Select the already populated “Background IC” from the region list. This will initialize the entire flow field with air.
Enter
101325
Pa in thePressure (optional)
fieldSelect the region created previously for the bed Initial Condition (“bed” region) and click the
OK
button.Select the solid (named previously as “glass beads”) sub-pane and enter a volume fraction of
0.4
in theVolume Fraction
field. This will fill the bottom half of the domain with glass beads.
3.5.8. Create Boundary Conditions¶
On the Boundary conditions
pane:
On the
Select region
dialog, select “Mass Inflow” from theBoundary type
drop-down menuSelect the “inlet” region and click
OK
On the
Fluid
sub-pane, enter a velocity in theY-axial velocity
field of0.25
m/sOn the
Select region
dialog, select “Pressure outflow” from theBoundary type
combo-boxSelect the “outlet” region and click
OK
Note
The default pressure is already set to 101325 Pa, no changes need to be made to the outlet boundary condition.
3.5.9. Change numeric parameters¶
On the Numerics
pane, Residuals
sub-pane:
Enter
0
in theFluid Normalization
field.
3.5.10. Select output options¶
On the Output
pane:
On the
Basic
sub-pane, check theWrite VTK output files (VTU/VTP)
checkboxSelect the
VTK
sub-paneSelect the “Background IC” region from the list to save all the cell data
Click
OK
to create the outputEnter a base name for the
*.vtu
files in theFilename base
fieldChange the
Write interval
to0.01
secondsSelect the
Volume fraction
,Pressure
, andVelocity vector
checkboxes on theFluid
tabSelect the “Slice” region from the list to save all the cell data
Click
OK
to create the outputEnter a base name for the
*.vtu
files in theFilename base
fieldChange the
Write interval
to0.01
secondsSelect the
Volume fraction
,Pressure
, andVelocity vector
checkboxes on theFluid
tab
3.5.11. Change run parameters¶
On the Run
pane:
Change the
Stop time
to1.0
secondsChange the
Time step
to1e-3
secondsChange the
Maximum time step
to1e-2
seconds
3.5.12. Run the project¶
3.5.13. View results¶
Results can be viewed, and plotted, while the simulation is running.
Create a new visualization tab by pressing the next to the Model tab
Select an item to view, such as plotting the time step (dt) or click the
3D view
button to view the vtk output files.On the
VTK
results tab, the visibility and representation of the*.vtk
files can be controlled with the menu on the side.
3.5.14. Convert this project into a 3D DEM simulation¶
Close the VTK window
On the
Model
pane, change the solver toMFiX-DEM
On the
Mesh
pane, coarsen the grid to 15, 45, and 15 cells in the in the x, y, and z direction, respectfully.
Note
The grid resolution needs to be coarser because we are drastically increasing the particle diameter below. The fluid grid cell size has to be bigger than the particle size.
On the
Solids
pane, change that particle diameter to5.0000e-03
to get a more reasonable particle count for tutorial purposes.On the
Solids
pane,DEM
sub-pane: - check theEnable automatic particle generation
- enter a value of15
in theSearch grid partitions
,KMAX
field.On the
Boundary Conditions
pane, change theinlet
Y-axial velocity
to0.6
m/sOn the
Boundary Conditions
pane, delete thewalls
boundary condition and re-add it to write the correct wall parameters for the DEM simulation.On the
Output
pane,VTK
sub-pane:Delete the
all
orBackground_IC
outputCreate a new output, change the
Output type
toParticle data
and select theBackground_IC
region.Change the write frequency to
0.01
Select the
Diameter
andTranslational Velocity
data
Run the simulation
Create a VTK window to visualize the data. It will automatically show the slice (cell data) and the particles.