3.20. DEM granular flow chutes

This tutorial shows how to create a three dimensional pure granular flow simulation from a series of cylindrical chutes. The model setup is:

Property	Value
geometry	1.75 m x 0.94 m x 0.2 m
mesh	20 x 20 x 10
solid diameter	12.5 mm (0.0125 m)
solid density	2500 kg/m2
temperature	298 K
pressure	101325 Pa

3.20.1. 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.

3.20.2. 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.

• Check the Disable Fluid Solver checkbox.

3.20.3. Enter the geometry

On the Geometry pane:

• Create the cylindrical geometry by pressing -> primitives -> cylinder

  • Enter 0.1 meters for the cylinder radius

  • Enter 30 for the cylinder resolution

• Create another cylindrical geometry by pressing -> primitives -> cylinder

  • Enter 1.2 meters for the cylinder height

  • Enter 0.08 meters for the cylinder radius

  • Enter 30 for the cylinder resolution

• Subtract the smaller radius cylinder from the larger radius cylinder

  • Select the larger radius cylinder (named cylinder)

  • While holding the ctrl key, select the smaller radius cylinder (named cylinder1)

  • Press the (difference) button

• Slice the tube in half:

  • Add a box: -> primitives -> box

  • Change the Center X value to 0.5 m

  • Change the Y Length to 1.2 m

  • Select the tube (named difference)

  • While holding the ctrl key, select the box (named box)

  • Press the button

• Rotate the chute:

  • Select the chute (named difference1)

  • Add a filter: -> transform

  • Enter a value of 0.8 m in the Translate Y field.

  • Enter a value of 70 in the Rotation Z field.

• Copy the chute by pressing the button with the chute selected (named transform)

  • Enter a value of 0.8 in the Translate X field

  • Enter a value of 0.6 in the Translate Y field

  • Enter a value of 120 in the Rotation Z field

• Copy the chute again by pressing the button with the chute selected (named transform1)

  • Enter a value of 0.0 in the Translate X field

  • Enter a value of 0.3 in the Translate Y field

  • Enter a value of 70 in the Rotation Z field

• Press the Autosize button to fit the domain extents to the geometry

3.20.4. Enter the mesh

On the Mesh pane:

• On the Background sub-pane

• Enter 20 for the x cell value

• Enter 20 for the y cell value

• Enter 10 for the z cell value

3.20.5. Create regions for initial and boundary condition specification

Select the Regions pane.

• Create a region to be used for the wall boundary condition

  • Click the (all) button to create a new region

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

  • Change the color by pressing the Color button

  • Check the Select facets (STL) checkbox

• Create a region to be used as the mass inflow boundary condition

  • Click the (top) button to create a new region

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

  • Enter a value of -0.4 m in the From X field

  • Enter a value of -0.2 m in the To X field

3.20.6. Create a solid

On the Solids pane:

• Click the button to create a new solid

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

• Enter the particle diameter of 1/80 m in the Diameter field

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

On the DEM sub pane:

• check the Enable automatic particle generation checkbox and keep defaults values for all other settings.

3.20.7. Create Initial Conditions

On the Initial conditions pane leave the default initial condition.

3.20.8. 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 glass beads sub-pane:

  • Enter a value of 0.1 in the volume fraction field.

  • Enter a velocity in the Y-axial velocity field of -0.1 m/s

• Create another Boundary condition by clicking the button

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

• Select the “walls” region and click OK

3.20.9. Select output options

On the Output pane:

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

• Select the VTK sub-pane

• Create a new output by clicking the button

• Select Particle Data in the Output type combo box.

• 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 *.vtp files in the Filename base field

• Change the Write interval to 0.1 seconds

• Select the Diameter and Translational Velocity check boxes.

3.20.10. Run the project

• Save project by clicking button

• Run the project by clicking the button

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

• Click the Run button to actually start the simulation

3.20.11. View results

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

• Create a new visualization tab by pressing the in the upper right hand corner.

• Select an item to view, such as plotting the time step (dt) or click the VTK button to view the vtk output files.