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 worflow for this tutorial.

create project

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.

select model parameters

3.6.3. Enter the geometry

On the Geometry pane:

  • Select the wand 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 overscan Reset View icon on the top-left corner of the Model window

hopper wizard

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

enter mesh

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 all_region 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:

  1. 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).

  2. 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)

  3. 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 region 1

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

  • Click the bottom_region

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

Finally, create a region to initialize the solids:

  • Click the all_region

  • 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 add 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 add 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 add 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 add 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

new boundary condition
  • Select the VTK sub-pane

  • Create a new output by clicking the add 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 the Stop Time to 2.0 seconds

  • Change the Time step to 1e-3 seconds

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

3.6.11. Run the project

  • Save project by clicking save button

  • Run the project by clicking the play button

  • On the Run dialog, select the default solver

  • Click the Run button to actually start the simulation

run

3.6.12. View results

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

  • Create a new visualization tab by pressing the add 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.

results