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.

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.

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

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.

3.3.5. Create regions for initial and boundary condition specification¶

On the Regions pane:

Click the (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) 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) 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”)

3.3.6. Create a solid¶

On the Solids pane, Materials sub-pane:

Click the 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

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

3.3.7. Create Initial conditions¶

On the Initial conditions pane:

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

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.

3.3.8. Create Boundary conditions¶

On the Boundary conditions pane:

Create a new Boundary condition by clicking the 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 “42” m/s

Create another Boundary condition by clicking the 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.

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

Select the VTK sub-pane
Create a new output by clicking the button
Select “Particle Data” from the ‘Output type’ drop-down menu.
Select the “Background” region from the list to save all the particle data
Click OK to create the output

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

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 button
Run the project by clicking the button
On the Run dialog, select the executable from the combo-box
Click the Run button to actually start the simulation

3.3.12. 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.

Change frames with the , , , and buttons
Click the button to play the available vtk files.
Change the playback speed under the section on the sidebar.