3.2. Two-dimensional fluidized bed, Two-fluid Model (TFM)

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

Property

Value

Geometry

10 cm x 30 cm

Mesh

20 x 60

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

3.2.1. 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.

Note

A new project directory will be created in the location directory, with the name being the project name.

create project

3.2.2. 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

3.2.3. Enter the geometry

On the Geometry pane:

  • Select the 2 Dimensional checkbox

  • Enter 10/100 meters for the maximum x value

  • Enter 30/100 meters for the maximum y value

Note

We could have entered 0.1 and 0.3 to define the domain extents, but this example shows that simple mathematical expressions (+,-,*,/) are allowed.

enter geometry

3.2.4. Enter the mesh

On the Mesh pane, Background sub-pane:

  • Enter 20 for the x cell value

  • Enter 60 for the y cell value

enter mesh

3.2.5. 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 add (add) 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 xmin or min in the From X field

  • Enter xmax or max in the To X field

  • Enter ymin or min in the From Y field

  • Enter ymax/2 or max/2 in the To Y field

  • Enter zmin or min in the From Z field

  • Enter zmax or max in the To Z field

Note

Here we could have entered numerical values for the coordinates, but it is recommended to use parameters (xmin, xmax etc.) when possible. These parameters will update automatically if the “Domain Extents” change.

create region 1
  • Click the bottom_region (bottom) button to create a new region with the From and To fields already filled out for a region at the bottom of the domain, to be used by the gas inlet boundary condition. From Y and To Y should equal ymin, defining an XZ-plane.

  • 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 with the From and To fields already filled out for a region at the top of the domain, to be used by the pressure outlet boundary condition. From Y and To Y should equal ymax, defining an XZ-plane.

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

create region 3

3.2.6. Create a solid

On the Solids pane:

  • Click the add button to create a new solid

  • Accept the radial distribution setting (Carnahan-Starling)

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

  • Keep the model as “Two-Fluid Model (MFiX-TFM)”)

  • 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

3.2.7. 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

initial condition pane
  • 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.

create new initial condition
  • 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 condition pane2

3.2.8. 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 “0.25” 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 and right planes) will behave as No-Slip walls.

3.2.9. Change numeric parameters

On the Numerics pane, Residuals sub-pane:

  • Enter 0 in the Fluid Normalization field.

3.2.10. 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 the “Background IC” region from the list to save all the cell data

  • Click OK to create the output

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

  • Change the Write interval to 0.1 seconds

  • Select the Volume fraction, Pressure, and Velocity vector checkboxes on the Fluid sub-sub-pane

new boundary condition

3.2.11. Change run parameters

On the Run pane:

  • Change the Time step to 1e-3 seconds

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

new boundary condition

3.2.12. Run the project

  • Save project by clicking the save button

  • Run the project by clicking the play button

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

  • Click the Run button to actually start the simulation

new boundary condition

3.2.13. 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.

new output
  • 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.

new boundary condition

3.2.14. Increase grid resolution

For this simulation, increasing the grid resolution will better resolve the bubbles (at the expense of a slower simulation time). To do this:

  • Click the reset button and delete all simulation files.

  • On the Mesh pane, change the X Cells to 80 and the Y Cells to 180

  • On the Output pane, VTK sub-pane, change the write interval to 0.01

  • Save and run the project.