3.3. Two-dimensional fluidized bed, Discrete Element Model (DEM)

This tutorial shows how to create a two dimensional fluidized bed simulation using the Discrete Element Model. The model setup is:

Property

Value

geometry

15 cm x 90 cm x 0.4 cm

mesh

15 x 45 x 1

solid diameter

4000 microns (\(4000 \times 10^{-6}\) m)

solid density

2700 kg/m2

gas velocity

42.0 m/s

temperature

298 K

pressure

101325 Pa

3.3.1. 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

3.3.2. Select model parameters

  • On the Model pane, enter a descriptive text in the Description field

  • Select “Discrete Element Model (MFiX-DEM)” in the Solver drop-down menu.

model parameters

3.3.3. Enter the geometry

On the Geometry pane:

  • Enter 0.15 meters for the maximum x value

  • Enter 0.90 meters for the maximum y value

  • Enter 0.004 meters for the maximum z value

enter geometry

3.3.4. Enter the mesh

On the Mesh pane, Background sub-pane:

  • Enter 15 for the x cell value

  • Enter 45 for the y cell value

  • Enter 1 for the z cell value

Note

Since there is only one cell in the Z direction, this model is effectively a 2D simulation.

enter mesh

3.3.5. Create regions for initial and boundary condition specification

On the Regions pane:

  • Click the All (all) button to create a new region that covers the entire domain to be used for the bed initial condition.

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

  • Change the To Y field to be “ymax/2”

  • Click the Bottom (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”)

  • Enter 0.07 in the From X field and 0.08 in the To X field.

  • Click the Top (top) button to create a new region to be used by pressure outlet boundary condition.

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

create regions

3.3.6. Create a solid

On the Solids pane, Materials sub-pane:

  • Click the Add button to create a new solid

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

  • Enter the particle diameter of 0.004 m in the Diameter field

  • Enter the particle density of 2700 kg/m2 in the Density field

new boundary condition
  • Select the Solids pane, DEM sub-pane

  • Check the Enable automatic particle generation checkbox, so that the bed Initial Condition, defined later, will be filled with solids

new boundary condition

3.3.7. 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

new boundary condition
  • Create a new Initial Condition by pressing the Add button

  • Select the bed region created previously for the bed Initial Condition (“bed” region) and click the OK button.

new boundary condition
  • Select the solid (named previously as “solid”) 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 solids.

  • Note the estimated number of particles and inventory (around 3,200 particles or 0.3 kg). When running DEM simulations on a single core machine, it is recommended to stay below 100,000 particles to get reasonable run times.

new boundary condition

3.3.8. 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

new boundary condition
  • On the “Fluid” sub-pane, enter a velocity in the Y-axial velocity field of “42” m/s

new boundary condition
  • 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.

new boundary condition

Note

By default, boundaries that are left undefined (here the left, right, front, and back planes) will behave as No-Slip walls.

3.3.9. Select output options

On the Output pane:

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

new boundary condition
  • Select the VTK sub-pane

  • Create a new output by clicking the Add button

  • Select “Particle Data” from the ‘Output type’ drop-down menu.

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

  • Click OK to create the output

new boundary condition
  • Enter a base name for the *.vtu files in the Filename base field (“particles”)

  • Change the Write interval to 0.01 seconds

  • Select the Diameter and Translational Velocity checkboxes

new boundary condition

3.3.10. Change run parameters

On the Run pane:

  • Change Stop time to 1.0 seconds

  • Change Time step to 1e-2 seconds

  • Change Maximum time step to 1e-2 seconds

3.3.11. Run the project

  • Save project by clicking the Save button

  • Run the project by clicking the Play button

  • On the Run dialog, select the executable from the combo-box

  • Click the Run button to actually start the simulation

new boundary condition

3.3.12. 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
  • Change frames with the First, Back, Next, and Last buttons

  • Click the Play button to play the available vtk files.

  • Change the playback speed under the Speed section on the sidebar.

vtk view