# ACU-T: 6101 Particle Separation in a Windshifter using AcuSolve - EDEM Unidirectional Coupling

This tutorial introduces you to the workflow for setting up and running a basic unidirectional coupling (one-way steady) simulation 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 ACU-T: 6100 Particle Separation in a Windshifter using Altair EDEM, 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-T6101_windshifter.hm from HyperWorksCFD_tutorial_inputs.zip.

## Problem Description

The problem to be solved is shown schematically in Figure 1. It is a windshifter model in which air enters the domain from the inlet at the bottom at a very high velocity (20 m/sec) and exits through the outlet. When particles are introduced into the domain through the particle inlet, the lighter particles get carried away with the air and the heavier particles exit through the opening at the bottom. Since the concentration of the particles is sparse, the effect of the particles on the fluid field is not considered for this simulation. Hence, one-way coupling between AcuSolve and EDEM is used to simulate the separation of particles; only the effect of the fluid forces on the particles is considered.

The model consists of a cylindrical pipe with a 45-degree bend. The radius of the pipe is 0.25 m and the particle inlet is located midway through the length of the pipe.

The workflow for an AcuSolve-EDEM unidirectional coupling simulation is shown below.

Accordingly, the tutorial consists of two parts:

1. AcuSolve setup and geometry export
2. EDEM setup and simulation

The AcuSolve model will be set up using HyperWorks CFD. Once the AcuSolve setup is complete, the EDEM deck with the geometry will be exported from HyperWorks CFD. This input deck will be opened in EDEM and will be used to complete the EDEM setup. Once the EDEM deck is set up, you will launch the coupled simulation.

Two different bulk materials used in the EDEM simulation and their properties are listed below:

Name Density (kg/m3) Size of particle (m) Average weight of individual particle (kg) Rate of generation (particles per sec)
Heavy particle 900 0.03 0.1 100
Light particle 100 0.03 0.01 100
The fluid drag forces on the particles are calculated using the Schiller-Naumann drag model. AcuSolve receives the particle position and velocity information from EDEM and calculates the drag forces on the particles. This fluid forces information is sent back to EDEM, which will be used to update the location and velocities of the particles. This loop is repeated until the end of the simulation.

## 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-T6101_windshifter.hm and click Open.
4. Click File > Save As.
5. Save the database as windshifter_unidirectional 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:
1. Select the Multiphase flow radio button.
2. Change the Multifluid type to Unidirectional EDEM Coupling.
3. Set the Eulerian material to Air-EDEM Particle -1way, if not set already.
4. Set Time step size and Final time to 0.001 and 1, respectively.
5. Select Spalart-Allmaras as the Turbulence model.
6. Verify that Gravity is set to 0, 0, -9.81.
3. Click the Solver controls setting and set the Minimum and Maximum stagger iterations to 2 and 4, respectively.
4. Close the dialog and save the model.

### Assign Material Properties

1. From the Flow ribbon, click the Material tool.
2. Verify that Air-EDEM Particle - 1way 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 20 m/s for the Average velocity and set the Carrier fluid volume fraction to 1.0.
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. Click the No Slip tool.
7. Select the face highlighted in the figure below.
8. In the Boundaries legend, double-click on Wall and rename it to Particle_inlet.
You will use this surface as a reference geometry to create a particle factory in EDEM. Hence, you are placing this surface in a different geometry group.
9. Click on the guide bar.
10. Save the model.

## Generate the Mesh

1. From the Mesh ribbon, click the Batch tool.
The Meshing Operations dialog opens.
2. Change the Average element size to 0.3.
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. Set the Time step interval to 10.

## Export the Solver Deck

1. From the menu bar, go to File > Export > Solver Deck.
2. Name the file windshifter_unidirectional and make sure that AcuSolve (*.inp) is selected as the file type.
3. Click Save.
The AcuSolve input files and the EDEM input deck with the geometry sections are created. You will use this EDEM deck to set up the DEM simulation deck.

## Part 2 - EDEM Simulation

Start Altair EDEM from the Windows start menu by clicking Start > Altair 2021 > EDEM 2021 .

## Open the EDEM Input Deck

As mentioned earlier, when the AcuSolve simulation was launched, HyperWorks CFD created a set of EDEM files in the problem directory. You will open that EDEM input deck and setup the DEM simulation

1. In the Creator tab in EDEM, go to File > Open.
2. In the dialog, browse to the AcuSolve problem directory and open the windshifter_unidirectional.dem file located in the EDEM folder.
3. Click the Environment tab under the Creator Tree, uncheck Auto Update from Geometry, then check the box again to fit the geometry within the boundary.

## Define the Bulk Materials and Equipment Material

In this step, you will define the material models for the heavy and light bulk material and the equipment material.

1. In the Creator Tree, right-click on Bulk Material and select Add Bulk Material.
2. Rename the material to Heavy.
3. In the Creator Tree, set the Solids Density property to 900 kg/m3.
You will use the default values for other properties for this tutorial.
4. Click below Interaction to define the interaction properties for collisions among the heavy particles. In the dialog, click OK.
5. In the Creator Tree, right click on Heavy and select Add Shape from Library > Dual Sphere Shape.
6. Rename the particle to Heavy particle.
7. Under Heavy particle, click Properties.
8. In the Heavy particle Spheres panel, set the Physical Radius of both the spheres to 0.03 m and press Enter.
9. In the Creator Tree, click Calculate Properties.
10. In the Creator Tree, right-click on Bulk Material and select Add Bulk Material.
11. Rename the material to Light.
12. In the Creator Tree, set the Solids Density property to 100 kg/m3.
You will use the default values for other properties for this tutorial.
13. Click below Interaction to define the interaction properties for collisions among the heavy particles. In the dialog, select Heavy then click OK.
14. Click again to define the interaction properties for collisions among the light particles. In the dialog, select Light then click OK.
15. In the Creator Tree, right click on Light and select Add Shape from Library > Dual Sphere Shape.
16. Rename the particle to Light particle.
17. Under Light particle, click Properties.
18. In the Light particle Spheres panel, set the Physical Radius of both the spheres to 0.03 m and press Enter.
19. In the Creator Tree, click Calculate Properties.
20. In the Creator tree, right-click on Equipment Material and select Add Equipment Material. Rename it to Steel.
21. Set the Density to 7800 kg/m3.
22. Click below Interaction to define the interaction properties for collisions among the heavy particles. In the dialog, select Heavy then click OK.
23. Click again to define the interaction properties for collisions among the light particles. In the dialog, select Light then click OK.
24. Save the model.

## Create the Particle Factory

1. Expand Geometries under the Creator Tree tab. Next, right-click on the Particle inlet surface group and select Copy Geometry > Single Copy.
2. Rename the new geometry section to Particle_factory.
3. Right-click on the Default Wall geometry section in the Creator Tree and select Merge Geometry(s).
4. In the Merge Geometry dialog, select the Particle_inlet then click OK.
5. Click on the Default Wall geometry section, set the Type to Physical, and the Material to Steel (if not set already).
6. In the Creator Tree, click the Inlet section and change the Type to Virtual.
7. Similarly, change the Type to Virtual for the Outlet and Particle_factory sections.
8. Under Particle_factory, click Transform. Set the X-Position to 0.035 m
Note: Set the Opacity value to 0.2 to see the transformed surface location inside the pipe geometry.

This is done to make sure that the particles are generated inside the fluid domain.

## Define the Particle Factory

Now that the bulk material, geometry sections, and equipment materials are defined, you need to create a particle factory to generate the particles. You will create one factory for each bulk material.

1. In the Creator Tree, right-click on Particle_factory and select Add Factory.
2. Rename the new factory to Heavy factory.
3. Set the particle generation parameters as shown in the figure below.
4. Click besides Velocity, set the X-velocity to 1 m/s, then click OK.
5. Repeat steps 1-4 to create another factory named Light factory using the same parameters but with Light as the Material.

## 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 activate the Auto Time Step checkbox (if not set already).
3. Set the Total Time to 1 s and the Target Save Interval to 0.01 s.
4. Set the Cell Size to 4 R min.
Generally, a value in the range of 3-6 Rmin is recommended as the optimum cell size. The cell size in EDEM doesn’t have any impact on the accuracy of the simulation and affects only the run time.
5. Set the Selected Engine to CPU Solver and set the Number of CPU Cores based on availability.
6. Once the simulation settings have been defined, save the model.

## 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. Enter the following text in the additional arguments field: -tlog -lprobe.
This will instruct AcuSolve to launch the AcuTail and AcuProbe windows, which can be used to monitor the solution as the simulation progresses.
5. Set the Parallel processing option to Intel MPI.
6. Optional: Set the number of processors to 4 or 8 based on availability.
7. Expand Default initial conditions, uncheck Pre-compute flow and set the velocity values to 0. Uncheck Pre-compute Turbulence.
8. Click Run to launch AcuSolve.
If the coupling between AcuSolve and EDEM is successful, a message will be printed in the AcuSolve Log file before the first time step.
As the solution progresses, the AcuTail and AcuProbe windows are launched automatically. In the AcuTail window, the residual ratio and solution ratio information is printed as the simulation progresses. A summary of the simulation is printed in the end, indicating that the simulation is complete.
9. Once the solution is complete, close both the AcuTail and AcuProbe windows.

## Analyze the Results

### AcuSolve Post-Processing

1. Once the solution is completed, navigate to the Post ribbon.
2. From the menu bar, click File > Open > Results.
3. Select the AcuSolve log file in your problem directory to load the results for post-processing.
The solid and all the surfaces are loaded in the Post Browser.
4. Select the Left face on the view cube to align the model to the x-z plane.
5. In the Post Browser, turn off the display of the boundary surfaces by clicking on the icon next to Flow Boundaries.
6. Click the Slice Planes tool.
7. In the modeling window, click on the plane that is parallel to the screen (the x-z plane).
8. In the slice plane microdialog, click to create the slice plane.
9. In the display properties microdialog, set the display to velocity and activate the Legend toggle.
10. Change the upper bound of the legend to 36.
11. Click and set the Colormap name to Rainbow Uniform.
12. Click on the guide bar.
The velocity contour should look like the one shown below at the beginning of the simulation.
13. Plot the contours at 0.25s, 0.5s, 0.75s, and 1.0s by dragging the slider on the bottom to the 26th, 51th, 76th, and 101st frames.
Since the effect of particles on the pressure and velocity fields is not considered for unidirectional coupling, the velocity contours should look similar for all the time frames mentioned above.
14. Right-click on Slice Plane 1 in the Post Browser and select Edit.
15. In the microdialog, change the Display variable from velocity to volume fraction edem particle and set the upper bound of the legend to 0.186.
16. Click on the guide bar.
17. Plot the contours at 0.5s (step=51/101), 0.75s (step=76/101), and 1.0s (step = 101/101) to see the volume fraction edem particle distribution inside the fluid domain.

### 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 click Default Wall.
3. Verify that the Display Mode is set to Filled and set the Opacity to 0.2.
4. In the Analyst Tree, expand Particles and click on Heavy particle.
5. Change the display color to Magenta.
6. Click on Light particle and set the display color to Green.
7. On the menu bar, set the time to 0 by clicking:
8. Set the View plane to + Y.
9. In the Viewer window, set the Playback Speed to 0.1x then click on the play icon to play the particle flow animation.
10. You can also plot the results at different timesteps by clicking the drop-down menu.
For the current case, the results are plotted at 0.25s, 0.5s, 0.75s, and 0.98s to see the particle distribution inside the fluid domain at both inlet and outlet.

Observe that the lighter particles (green) get carried by the fluid and escape the domain through the outlet at the top and the heavier particles (magenta) stay inside the domain for a longer time while some of them fall through the bottom of the pipe.

11. On the menu bar, click the Create Graph icon .
12. In the Analyst Tree, change the plot type to Line by clicking .
13. Click on the X-axis tab and verify that the values are set as shown in the figure below.
14. Click on the Y-axis tab. Create a plot of average residence time of the heavy particle over the simulation time by setting the values as shown in the figure below.
15. Click to add another Y-axis and set the Type to Light particle.
16. Leave all the other options unchanged then click Create Graph to create a plot of average residence time of both the particles.

The plot in green is for the heavier particles and it can be observed that the average residence time is higher for the heavier particles compared to the lighter particles (blue).

## Summary

In this tutorial, you learned how to setup and run a basic AcuSolve-EDEM unidirectional (one-way transient) coupling problem. In the first part, you set up the AcuSolve model in HyperWorks CFD and exported the geometry. Next, you imported the EDEM input files created by HyperWorks CFD, set up the EDEM model, and ran the coupled simulation. Once the coupled simulation was completed, you learned how to create animations and plots in both HyperWorks CFD Post and EDEM Analyst.