3.6. Three Dimensional DEM Hopper¶

This tutorial shows how to create a three dimensional granular flow DEM simulation. The model setup is:

Property	Value
geometry	5 cm diameter hopper
mesh	10 x 25 x 10
solid diameter	0.003 m
solid density	2500 kg/m²
gas velocity	NA
temperature	298 K
pressure	NA

3.6.1. 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.

3.6.2. 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 (Pure Granular Flow) check-box.

3.6.3. Enter the geometry¶

On the Geometry pane:

Select the wizard menu and select the hopper wizard
Select apply to build the hopper stl file
Press the Autosize button to fit the domain extents to the geometry
Press the Reset View icon on the top-left corner of the Model window

3.6.4. Enter the mesh¶

On the Mesh pane, Background sub-pane:

Enter 10 for the x cell value
Enter 25 for the y cell value
Enter 10 for the z cell value

On the Mesh pane, Mesher sub-pane:

Enter 0.0 in the Facet Angle Tolerance

3.6.5. Create regions for initial and boundary condition specification¶

Select the Regions pane. By default, a region that covers the entire domain is already defined.

A region for the hopper walls (STL) is needed to apply a wall boundary condition to:

Click the button to create a region that encompasses the entire domain
change the name of the region to a descriptive name such as “walls”
Check the Select Facets (STL) check-box to turn the region into a STL region. The facets of the hopper should now be selected.

In order to allow the particles to leave the domain through the bottom, the facets at the bottom of the hopper need to be deselected. There are three ways to accomplish this:

Change the Y Min domain extent value on the geometry pane by a small amount so that those facets fall outside the simulation domain (for example, change the value to -0.0974).
Change the Y From region extent value on the regions pane for this STL region by a small amount so that those facets fall outside the region (for example, change the value to ymin+0.0001)
Or, use the Filter facets based on normals option on the region pane.

For this example, use option 3 to filter the facets that have normals pointed in the Y direction by:

Select box from the Selection method drop-down.
Uncheck Slice facets.
Check the Filter facets based on normals check-box
Enter a vector pointed in the positive Y direction by entering 0, 1, and 0 in the x, y, z fields, respectively
Check the Include equilibrant vector to include facets with normals in the opposite direction of the vector (-x, -y, -z)
Enter an angle of 10 in the angle field to include facets with normals within 10 degrees of the filter vector
Check the Invert Selection check box to de-select facets that fall along the filter vector and select all the other facets

All the facets, except for the facets at the top and bottom, of the hopper should now be selected.

Create a region to apply a pressure outlet boundary condition to allow particles to leave the domain:

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

Finally, create a region to initialize the solids:

Click the
Enter a name for the region in the Name field (“solids”)
Enter ymin/3 in the From Y field
Enter 0 in the To Y field

3.6.6. Create a solid¶

On the Solids pane

Click the button to create a new solid
Enter a descriptive name in the Name field (“solids”)
Keep the model as “Discrete Element Model (MFiX-DEM)”)
Enter the particle diameter of 0.003 m in the Diameter field
Enter the particle density of 2500 kg/m² in the Density field

In the DEM sub-pane, check Enable automatic particle generation check-box

3.6.7. Create Initial Conditions¶

On the Initial conditions pane

Click the button to create a new initial condition
On the Select Region dialog, select the “solids” region and click OK
On the solids sub-pane, enter 0.4 in the Volume fraction field

3.6.8. Create Boundary Conditions¶

Select the Boundary conditions pane and create a wall boundary condition for the hopper by:

clicking the button
On the Select Region dialog, select “No Slip Wall” from the Boundary type drop-down menu
Select the “walls” region and click OK

Finally, create a pressure outlet 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

3.6.9. Select output options¶

Select 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
On the “select region” dialog, select “particle data” from the output type drop-down menu
Select the “Background IC” region from the list to save particle data over the entire domain
Click OK to create the output
Change the Write interval to 0.01 seconds
Select the Diameter and Translational velocity check-boxes

3.6.10. Change run parameters¶

On the Run pane:

Change Stop time to 2.0 seconds
Change Time step to 1e-3 seconds
Change Maximum time step to 1e-2 seconds

3.6.11. Run the project¶

Save project by clicking button
Run the project by clicking the button
On the Run dialog, select the default solver
Click the Run button to actually start the simulation

3.6.12. 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.