# ACU-T: 6103 AcuSolve - EDEM Bidirectional Coupling with Heat Transfer

This tutorial introduces you to the workflow for setting up and running a basic bidirectional coupling (two-way) simulation with heat transfer 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-T6103_windshifter_heat.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 velocity of 20 m/sec and exits through the outlet. The temperature of the incoming fluid is 293 K. Particles at a temperature of 363 K are introduced into the fluid domain. As the particles move through the fluid domain, they exchange energy with the surrounding fluid and as a result their temperature drops down before they exit the fluid domain. The walls of the pipe are maintained at a constant temperature of 293 K.

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 bidirectional 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 mass 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 thermal material properties used for the particles are listed in the table below:

Name Thermal conductivity (W/m-k) Specific heat capacity (J/kg-K) Temperature (K)
Particles 1.4 840 363 (initial)
Walls 30 - 293

## 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-T6103_windshifter_heat.hm and click Open.
4. Click File > Save As.
5. Save the database as windshifter_heat 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 drag model and the drag coefficients as shown in the figure below.
9. Close the material model microdialog and then close the Material Library dialog.
10. In the Setup dialog, set the Eulerian Material to Air-Particle.
11. Set Time step size and Final time to 0.001 and 1, respectively. Select Spalart-Allmaras for the Turbulence model.
12. Verify that Gravity is set to 0, 0, -9.81.
13. Activate the Heat transfer checkbox.
14. Click the Solver controls setting and set the Minimum and Maximum stagger iterations to 2 and 4, respectively.
15. 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 20 m/s for the Average velocity, 293 K for Temperature, 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. Click the No Slip tool.
7. Select all the faces except the inlet and outlet faces.
8. In the microdialog, click the Temperature tab and set the parameters as shown in the figure below.
9. On the guide bar, click to execute the command and remain in the tool.
10. Select the face highlighted in the figure below. In the microdialog, click the Temperature tab and set the parameters as shown.
11. Click on the guide bar.
12. In the Boundaries legend, right-click on Wall 1 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.
13. Click on the guide bar.
14. Save the model.

## Generate the Mesh

1. From the Mesh ribbon, click the Volume 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_heat 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 2021.1 > EDEM 2021.1 .

## 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_heat.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 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 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 Heat Transfer Paramaters

1. In the Creator Tree, click on Physics.
2. Set the Interaction drop down to Particle to Particle and click Edit Contact Chain.
3. In the dialog, activate Heat Conduction and click OK.
4. In the Physics tab, click Heat Conduction then click .
5. In the dialog, set the Thermal conductivity of both Heavy and Light particles to 1.4 W/mK then click OK.
6. In the Physics tab, change the Interaction to Particle to Geometry and click Edit Contact Chain.
7. In the dialog, activate Heat Conduction and click OK.
8. In the Physics tab, click Heat Conduction then click .
9. In the dialog, set the thermal conductivity of the particles to 1.4 W/mK and the conductivity and temperature of the wall to 30 W/mK and 293 K, respectively. Click OK.
10. In the Physics tab, change the interaction to Particle Body Force.
11. Click Edit Contact Chain.
12. In the dialog, activate Temperature Update then click OK.
13. In the Physics tab, click Temperature Update then click .
14. In the dialog, set the specific heat capacity for both the particle types to 840 J/kgK then click OK.
15. Save the model.

## 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. Click besides Temperature, set the value to 363 K, then click OK.
Note: The fields for Temperature and Heat Flux will not be visible unless heat transfer properties are defined.
6. Repeat steps 1-5 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 de-activate the Auto Time Step checkbox.
3. Set the Fixed Time Step to 2.5e-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 4 R min.
Generally, a value in the range of 3-6 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.

## 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 velocity values to 0. Uncheck Pre-compute Turbulence.
7. Set the Temperature to 293 K.
8. Click Run to launch AcuSolve.
Once the AcuSolve run is launched, the Run Status dialog opens.
9. 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 temperature and activate the Legend toggle.
6. Change the bounds of the legend to 293 and 363.
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 0.2190.
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 click Wall.
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 Temperature.
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 particles which are at a higher temperature at the time generation become colder as they exchange energy with the fluid phase.

## Summary

In this tutorial, you learned how to set up and run a basic AcuSolve-EDEM bidirectional (two-way) coupling problem with heat transfer. In the first part, set up the AcuSolve model in HyperWorks CFD and exported the geometry. Next, you imported the EDEM input files created by HyperWorks CFD and set up the EDEM model. You learned how to set up the thermal properties for the particles as well as their interaction with other particles and equipment. Once the coupled simulation was completed, you learned how to create animations in both HyperWorks CFD Post and EDEM Analyst.