# ACU-T: 6104 AcuSolve - EDEM Bidirectional Coupling with Non-Spherical Particles

This tutorial introduces you to the workflow for setting up and running a basic bidirectional coupling (two-way) simulation with non-spherical particles using AcuSolve and EDEM. Prior to starting this tutorial, you should have already run through the introductory HyperWorks tutorial, ACU-T: 1000 HyperWorks UI Introduction, and have a basic understanding of HyperWorks CFD, AcuSolve, and EDEM. To run this simulation, you will need access to a licensed version of HyperWorks CFD, AcuSolve, and EDEM.

Prior to running through this tutorial, copy HyperWorksCFD_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract ACU-T6104_sieve.hm and sieve.dem from HyperWorksCFD_tutorial_inputs.zip.

## Problem Description

The problem to be solved is shown schematically in the figure below. The model consists of a simple sieve which oscillates at a frequency of 5 Hz and has an amplitude of 0.02 m. Particles are introduced into the system from the top at a velocity of 1 m/s. The particles fall through the openings in the sieve and as air is blown from the inlet at the bottom, the lighter bar-shaped particles get separated from the heavier spherical particles. An average velocity of 6 m/s is applied on the inlet face and the Arbitrary Lagrangian Eulerian approach is used for the mesh motion.
A sinusoidal motion along the z-axis is assigned to the sieve. The motion profile is shown below:

AcuSolve-EDEM bidirectional coupling is used to model the interaction between the fluid and particles. In this tutorial, non-spherical drag force models are used to accurately predict the drag forces on the particles by taking the shape of particles into consideration. The length scale used for factoring in the shape of the particles is the aspect ratio. Bar shaped particles with an aspect ratio of 2.75 and spherical particles with aspect ratio 1 are used for this simulation. The Rong drag model is used in conjunction with the Holzer-Sommerfeld non-spherical drag coefficient model.

The particle properties used for this simulation are listed in the table below:

L - length, D - diameter
Particle Type Density (kg/m3) Size (m) Number of particles
Bar 200 0.022/0.008 (L/D) 100
Sphere 1500 0.008 (D) 200

## Part 1 - EDEM Simulation

Start Altair EDEM from the Windows start menu by clicking Start > Altair 2021.2 > EDEM 2021.2 .

## Open the EDEM Input Deck

1. Click File > Open on the menu bar.
2. In the dialog, browse to your problem directory and open the sieve.dem file.

## Define the Bulk Materials and Equipment Material

In this step, you will define the material models for the bar and sphere-shaped particles.

1. In the Creator Tree, right-click on Bulk Material and select Add Bulk Material.
2. Rename the material to bar.
3. In the Creator Tree, set the Solids Density property to 200 kg/m3 and the Shear Modulus to 1e7 Pa.
4. Click below Interaction to define the interaction properties for collisions among the bar shaped particles. In the dialog, click OK.
5. Set the interaction coefficients as shown in the figure below.
6. In the Creator Tree, right click on bar and select Add Shape from Library > Straight Four Sphere Shape.
7. Rename the particle to bar.
8. Under bar, click Properties.
9. In the bar Spheres panel, set the Physical Radius and the XYZ positions as shown in the figure below.
10. In the Creator Tree, click Calculate Properties.
Note: Since the "Automatically Center Particle" option is active, EDEM will internally adjust the positions of the spheres in the particle. Although you might see minor changes in the location of the spheres, the overall dimensions of the particle stay the same.
11. Right-click on Bulk Material and select Add Bulk Material.
12. Rename the material to sphere.
13. Set the Solids Density property to 1500 kg/m3.
14. Click below Interaction to define the interaction properties for collisions with sphere particles. In the dialog, select sphere then click OK.
15. Set the interaction coefficients as shown in the figure below.
16. Click again to define the interaction properties for collisions with bar particles. In the dialog, select bar then click OK.
17. Set the interaction coefficients as shown in the figure below.
18. In the Creator Tree, right click on sphere and select Add Shape from Library > Single Sphere Shape.
19. Rename the particle to sphere.
20. Under bar, click Properties.
21. In the sphere Spheres panel, set the Physical Radius of the sphere to 0.004 m then press Enter.
22. In the Creator Tree, click Calculate Properties.
23. Right-click on Equipment Material and select Add Equipment Material.
24. Rename the material to Steel.
25. Set the Solids Density property to 7800 kg/m3.
26. Click below Interaction to define the interaction properties for collisions with bar particles. In the dialog, select bar then click OK.
27. Set the interaction coefficients as shown in the figure below.
28. Click again to define the interaction properties for collisions with sphere particles. In the dialog, select sphere then click OK.
29. Set the interaction coefficients as shown in the figure below.
30. Save the model.

## Define Geometries and Factories

1. In the Creator Tree, expand Geometries.
2. Click Sieve and verify that the type is set to Physical.
3. Right-click on Sieve and select Add Motion > Add Sinusoidal Translation Kinematic.
4. Name it oscillation and specify the parameters as shown in the figure below.
5. Click Outlet and set the type to Virtual.
6. Similarly, set the Inlet type to Virtual, the Walls type to Physical, and the Material type to Steel (if not set already).
7. Click factory and set the type to Virtual
8. Right-click on factory and select Add Factory. Name it bar factory.
9. Set the particle generation parameters as shown in the figure below.
10. Click besides Velocity, set the Z-velocity to -1 m/s, then click OK.
11. Repeat steps 8-10 to create another factory named sphere factory. Use the same parameters but set the Total Number to 200 and the Material to sphere.
12. Save the model.

## Define the Environment

In this step, you will define the extents of the domain for the EDEM simulation and the direction of gravitational acceleration.

1. In the Creator Tree, click Environment.
2. Activate the checkbox for Auto Update from Geometry (if not already selected).
When a moving particle touches the bounding faces of the domain (environment), it will be removed from the simulation.
3. Activate Gravity and set the z-value to -9.81 m/s2.
4. Save the EDEM deck.

## Define the Simulation Settings

1. Click in the top-left corner to go to the EDEM Simulator tab.
2. In the Simulator Settings tab, set the Time Integration scheme to Euler and de-activate the Auto Time Step checkbox.
3. Set the Fixed Time Step to 1e-5 s.
Note: Generally, a value of 20-40% of the Rayleigh Time Step is recommended as the time step size to ensure stability of the DEM simulation.
4. Set the Total Time to 1 s and the Target Save Interval to 0.01 s.
5. Set the Cell Size to 2.5 R min.
Generally, a value in the range of 2-6 Rmin is recommended as the optimum cell size.
6. Set the Selected Engine to CPU Solver and set the Number of CPU Cores based on availability.
7. Once the simulation settings have been defined, save the model.

## Start HyperWorks CFD and Open the HyperMesh Database

1. Start HyperWorks CFD from the Windows Start menu by clicking Start > Altair <version> > HyperWorks CFD.
2. From the Home tools, Files tool group, click the Open Model tool.
The Open File dialog opens.
3. Browse to the directory where you saved the model file. Select the HyperMesh file ACU-T6104_sieve.hm and click Open.
4. Click File > Save As.
5. Save the database as sieve_nonspherical in the same directory as the other input files.
This will be the working directory and all the files related to the simulation will be stored in this location.

## Validate the Geometry

The Validate tool scans through the entire model, performs checks on the surfaces and solids, and flags any defects in the geometry, such as free edges, closed shells, intersections, duplicates, and slivers.

To focus on the physics part of the simulation, this tutorial input file contains geometry which has already been validated. Observe that a blue check mark appears on the top-left corner of the Validate icon on the Geometry ribbon. This indicates that the geometry is valid, and you can go to the flow set up.

## Set Up Flow

### Set the General Simulation Parameters

1. From the Flow ribbon, click the Physics tool.
The Setup dialog opens.
2. Under the Physics models setting, select the Multiphase flow radio button.
3. Change the Multifluid type to Bidirectional EDEM Coupling.
4. Click the Eulerian material drop-down menu and select Material Library from the list.
You can create new material models in the Material Library.
5. In the Material Library dialog, select EDEM 2 Way Multiphase, switch to the My Material tab, then click to add a new material model.
6. In the microdialog, click EDEM Bidirectional Material in the top-left corner and change the name to Air-Particle.
7. Set the Carrier field to Air (if not set already).
8. Set the particle shape to Non-Spherical.
9. Set the drag model to Rong.
10. Set the Non spherical drag coefficient model to Holzer-Sommerfeld.
11. Click the table icon beside the drag coefficient model drop-down.
12. In the new dialog, click to add a new row, then enter the values for Aspect Ratio and Volume as shown in the figure below.
Note: The volumes entered here should be obtained from EDEM under particle properties. There might be slight variation in the volume values that you may see in your EDEM model but that is fine.

Here the aspect ratios are calculated based on the ratio of the length to diameter of the particles. The AR of 2.75 and 1 are for bar and sphere-shaped particles respectively. The volume of the particles can be obtained from EDEM under the particle properties. If the simulation has particles of a single shape, then the volume field can be set to zero.

13. Press Esc to close the dialog and then close the material model and Material Library dialogs as well.
14. In the Setup dialog, set the Eulerian Material to Air-Particle.
15. Set Time step size and Final time to 0.005 and 1, respectively. Select Spalart-Allmaras for the Turbulence model.
16. Verify that Gravity is set to 0, 0, -9.81.
17. Set the Pressure scale to Absolute.
18. Click the Solver controls setting and set the Maximum stagger iterations to 3.
19. Close the dialog and save the model.

### Assign Material Properties

1. From the Flow ribbon, click the Material tool.
2. Verify that Air-Particle has been assigned as the material.
3. On the guide bar, click to exit the tool.

### Define Flow Boundary Conditions

1. From the Flow ribbon, Profiled tool group, click the Profiled Inlet tool.
2. Click on the inlet face highlighted in the figure below. In the microdialog, enter a value of 6 m/s for the Average velocity and 1.0 for the Carrier fluid volume fraction.
3. On the guide bar, click to execute the command and exit the tool.
4. Click the Outlet tool.
5. Select the face highlighted in the figure below then click on the guide bar.
6. Save the model.

## Set Up Motion

### Select the Motion Type

1. From the Motion ribbon, click the Settings tool.
2. In the Setup dialog, set the Mesh motion to Arbitrary and close the dialog.

### Define the Mesh Boundary Conditions

1. From the Motion ribbon, click the Planar Slip tool.
2. Select the two surfaces highlighted in the figure below.
The surfaces selected have the minimum y-coordinate.
3. In the Mesh Motion legend, double-click on Planar Slip and change the name to y_neg.
4. On the guide bar, click to execute the command and remain in the tool.
5. Repeat steps 2-4 to create three more planar slip boundary conditions for the surfaces with the maximum y-coordiates, and the minimum and maximum x-coordinates. Name these groups y_pos, x_neg, and x_pos respectively.
Once the four planar slip conditions are defined, the Mesh Motion legend should look like the one shown below.
6. Save the model.

### Define Sinusoidal Translational Motion

1. From the Motion ribbon, click the Translation tool.
2. In the Mesh Motion legend, right-click on Unassigned and select Isolate.
3. On the guide bar, change the active selector to Surfaces.
4. Using box selection, select all the sieve surfaces as shown in the figure below.
Ensure that you are not selecting the inlet or outlet faces.
5. Click Vector on the guide bar.
6. Click anywhere on the sieve surfaces in the modeling window.
7. In the microdialog, click Z to align the axis to the global z axis.
8. In the microdialog, change the type to Time-varying and click the plot icon.
9. In the new plot dialog, click on the drop-down beside the table icon for function specification and select the oscillating option.
10. Enter the values for the sine function as shown in the figure below.
11. Click Convert to transform the sine function into an array for the multiplier function.
The motion profile for the translation motion should look like the one shown below.
12. Click on the guide bar.

## Generate the Mesh

1. From the Mesh ribbon, click the Volume tool.
The Meshing Operations dialog opens.
2. Set the Mesh size to Maximum size and change the Maximum element size to 0.03.
3. Click Mesh.
The Run Status dialog opens. Once the run is complete, the status is updated and you can close the dialog.
Tip: Right-click on the mesh job and select View log file to view a summary of the meshing process.
4. Save the model.

## Define Nodal Outputs

Once the meshing is complete, you are automatically taken to the Solution ribbon.

1. From the Solution ribbon, click the Field tool.
The Field Output dialog opens.
2. Check the box for Write Initial Conditions.
3. Uncheck the box for Write results at time step interval
4. Check the box for Write results at time interval.
5. Set the Time step interval to 0.05.

## Submit the Coupled Simulation

1. Start the coupling server by clicking Coupling Server in EDEM.
Once the Coupling server is activated, the icon changes.
3. From the Solution ribbon, click the Run tool.
The Launch AcuSolve dialog opens.
4. Set the Parallel processing option to Intel MPI.
5. Optional: Set the number of processors to 4 or 8 based on availability.
6. Expand Default initial conditions, uncheck Pre-compute flow and set the z-velocity value to 6. Uncheck Pre-compute Turbulence.
7. Click Run to launch AcuSolve.
Once the AcuSolve run is launched, the Run Status dialog opens.
8. In the dialog, right-click on the AcuSolve run and select View log file.
If the coupling with EDEM is successful, that information is printed in the log file.
Once the simulation is complete, the summary of the run time is printed at the end of the log file.

## Analyze the Results

### AcuSolve Post-Processing

1. In HyperWorks CFD, right-click on the AcuSolve run in the Run Status dialog and select Visualize results.
The results are loaded in the Post ribbon.
2. Click the Slice Planes tool.
3. Select the x-z plane as highlighted in the figure below.
4. In the slice plane microdialog, click to create the slice plane.
5. In the display properties microdialog, set the display to velocity and activate the Legend toggle.
6. Change the bounds of the legend to 0 and 15.
7. Click and set the Colormap name to Rainbow Uniform.
8. Click on the guide bar.
9. In the Post Browser, turn off the visibility of Flow Boundaries by clicking on its icon.
10. Select the Left face on the view cube to align the model to the x-z plane.
11. Click on the animation toolbar to view the animation of the temperature contour.
12. To plot the volume fraction edem particle variable, right-click on Slice Plane 1 in the Post Browser and select Edit.
13. In the display properties microdialog, change the display variable from temperature to volume fraction edem particle and the legend bounds to 0 and 0.025.
14. Click on the guide bar.
15. Click to start the animation.

### EDEM Post-Processing

1. Once the EDEM simulation is complete, click in the top-left corner to go to the EDEM Analyst tab.
2. In the Analyst Tree, expand Display > Geometries and then select all geometries by holding the Ctrl key.
3. Verify that the Display Mode is set to Filled and set the Opacity to 0.2.
4. In the Analyst Tree, click Particles.
5. Set the coloring to Velocity.
6. Activate the Auto Update checkboxes for both the Min and Max Value.
7. Activate the Show Legend checkbox.
8. Click Apply All.
9. On the menu bar, set the time to 0 by clicking:
10. Set the View plane to + Y.
11. In the Viewer window, set the Playback Speed to 0.1x and then click to play the particle flow animation.

Observe that the lighter bar shaped particles are blown away by the incoming fluid while the heavier particles fall through the sieve openings.

## Summary

In this tutorial, you learned how to set up and run a basic AcuSolve-EDEM bidirectional (two-way) coupling problem with non-spherical particles. You learned how to create a non-spherical particle in EDEM and set up the AcuSolve model to consider the effect of the particle shape for the fluid-particle interaction forces. Once the simulation was complete, you learned how to post-process the AcuSolve results using HyperWorks CFD and the EDEM results.