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.

create project

3.5.2. Select model parameters

On the Model pane:

  • Enter a descriptive text in the Description field

  • Select “Two-Fluid Model (MFiX-TFM)” in the Solver drop-down menu.

select model parameters

3.5.3. Enter the geometry

On the Geometry pane:

  • Create the cylindrical geometry by pressing the Add Geometry button -> Primitives -> cylinder

add cylinder
  • Enter 40/100 meters for the cylinder height

  • Enter 10/2/100 meters for the cylinder radius

  • Enter 30 for the cylinder resolution

  • Press 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 filter button and selecting the flip normals filter

enter cylinder input

3.5.4. Enter the mesh

On the Mesh pane:

  • On the Background sub-pane

  • Enter 20 for the x cell value

  • Enter 60 for the y cell value

  • Enter 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.

enter mesh

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_region (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 button

  • Enter 0 in the To Y field

create region 1
  • Click the bottom_region (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”)

create region 2
  • Click the top_region (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”)

create region 3
  • Click the all_region (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.

create region 4
  • Click the left_region (left) button to create a new region to be used to save a slice of cells at the center of the domain.

  • Enter a name for the region in the Name field (“slice”)

  • Enter 0 in the From X and To X fields

create region 5

3.5.6. Create a solid

On the Solids pane:

  • Click the add button to create a new solid

  • Enter a descriptive name in the Name field (“glass beads”)

  • Accept the radial distribution setting (Carnahan-Starling)

  • Enter the particle diameter of 200e-6 m in the Diameter field

  • Enter the particle density of 2500 kg/m2 in the Density field

create a solid

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 the Pressure (optional) field

  • Create a new Initial Condition by pressing the add button

  • Select 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 the Volume Fraction field. This will fill the bottom half of the domain with glass beads.

initial conditions

3.5.8. Create Boundary Conditions

On the Boundary conditions pane:

  • Create a new Boundary condition by clicking the add button

  • On the Select region dialog, select “Mass Inflow” from the Boundary type drop-down menu

  • Select the “inlet” region and click OK

  • On the Fluid sub-pane, enter a velocity in the Y-axial velocity field of 0.25 m/s

  • Create another Boundary condition by clicking the add button

  • On the Select region dialog, select “Pressure outflow” from the Boundary type combo-box

  • Select 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.

  • Create another Boundary condition by clicking the add button

  • On the Select region dialog, select “No Slip Wall” from the Boundary type combo-box

  • Select the “wall” region and click OK

3.5.9. Change numeric parameters

On the Numerics pane, Residuals sub-pane:

  • Enter 0 in the Fluid Normalization field.

3.5.10. Select output options

On the Output pane:

  • On the Basic sub-pane, check the Write VTK output files (VTU/VTP) checkbox

  • Select the VTK sub-pane

  • Create a new output by clicking the add button

  • Select the “Background IC” region from the list to save all the cell data

  • Click OK to create the output

  • Enter a base name for the *.vtu files in the Filename base field

  • Change the Write interval to 0.01 seconds

  • Select the Volume fraction, Pressure, and Velocity vector checkboxes on the Fluid tab

  • Create another output by clicking the add button

  • Select the “Slice” region from the list to save all the cell data

  • Click OK to create the output

  • Enter a base name for the *.vtu files in the Filename base field

  • Change the Write interval to 0.01 seconds

  • Select the Volume fraction, Pressure, and Velocity vector checkboxes on the Fluid tab

initial conditions

3.5.11. Change run parameters

On the Run pane:

  • Change the Stop time to 1.0 seconds

  • Change the Time step to 1e-3 seconds

  • Change the Maximum time step to 1e-2 seconds

new boundary condition

3.5.12. Run the project

  • Save project by clicking save button

  • Run the project by clicking the play button

  • On the Run dialog, select the default executable from the list

  • Click the Run button to actually start the simulation

3.5.13. View results

Results can be viewed, and plotted, while the simulation is running.

  • Create a new visualization tab by pressing the add 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.

new boundary condition

3.5.14. Convert this project into a 3D DEM simulation

  • Click the reset button and delete all simulation files.

  • Close the VTK window

  • On the Model pane, change the solver to MFiX-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 to 5.0000e-03 to get a more reasonable particle count for tutorial purposes.

  • On the Solids pane, DEM sub-pane: - check the Enable automatic particle generation - enter a value of 15 in the Search grid partitions, KMAX field.

  • On the Boundary Conditions pane, change the inlet Y-axial velocity to 0.6 m/s

  • On the Boundary Conditions pane, delete the walls 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 or Background_IC output

    • Create a new output, change the Output type to Particle data and select the Background_IC region.

    • Change the write frequency to 0.01

    • Select the Diameter and Translational Velocity data

  • Run the simulation

  • Create a VTK window to visualize the data. It will automatically show the slice (cell data) and the particles.

new boundary condition