ACU-T: 6100 Particle Separation in a Windshifter using Altair EDEM

This tutorial introduces you to the workflow for setting up and running a basic one-way coupled 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 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-T6100_windshifter.hm, Windshifter.x_t, windshifter.dll, and field_prefs_query.txt from HyperWorksCFD_tutorial_inputs.zip.

Note: This tutorial does not cover the steps related to geometry cleanup and meshing.

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.


Figure 1.
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. To simplify things, the particle inlet is considered as a wall for the CFD simulation. The workflow for an AcuSolve-EDEM one-way coupling simulation is shown below.


Figure 2.

The tutorial consists of two parts:

  1. AcuSolve simulation
  2. EDEM simulation

The setup for the AcuSolve simulation is done using HyperWorks CFD. Currently, only steady state flow analysis is supported for one-way coupling. Once the AcuSolve simulation is complete, the velocity nodal data is exported into CGNS format using the AcuTrans utility available in AcuSolve. This field data will be imported into EDEM and will be used to calculate the drag forces on the particles due to the fluid using an external library linked to EDEM.

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 0.01 0.004 100
Light particle 100 0.01 0.0004 100
The fluid drag forces on the particles are calculated using a Plug-in model provided along with the input files for this tutorial. The files windshifter.dll and field_query_prefs.txt should be placed in the same directory in which the EDEM database will be saved. The plug-model calculates the drag force on the particle using the relative velocity of the particle with respect to the local fluid velocity. This particle body force will used to update the location of the particles and then the new drag forces are calculated. This loop is repeated, and the process flow is explained in the figure below. To keep the tutorial simple, the steps for creating the plug-in model are not discussed in this tutorial.


Figure 3.

Part 1 - AcuSolve 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.


    Figure 4.
    The Open File dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file ACU-T6100_windshifter.hm and click Open.
  4. Click File > Save As.
    The Save File As dialog opens.
  5. Save the database as windshifter.hm 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.


Figure 5.

Set Up Flow

Set the General Simulation Parameters

  1. From the Flow ribbon, click the Physics tool.


    Figure 6.
    The Setup dialog opens.
  2. Click the Time setting and ensure that Steady is selected.


    Figure 7.
  3. Click the Flow setting.
  4. Check that the flow type is set to Turbulent.
  5. Select Spalart-Allmaras as the Turbulence model.


    Figure 8.
  6. Close the dialog and save the model.

Assign Material Properties

  1. From the Flow ribbon, click the Material tool.


    Figure 9.
  2. Verify that Air 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.


    Figure 10.
  2. Click on the inlet face, highlighted in the figure below.
  3. In the microdialog, enter 20 m/s as the Average velocity.


    Figure 11.
  4. On the guide bar, click to execute the command and exit the tool.
  5. Click the Outlet tool.


    Figure 12.
  6. Select the face highlighted in the figure below then click on the guide bar.


    Figure 13.
  7. Save the model.

Generate the Mesh

To focus on the solver setup, the mesh settings are predefined in the input file given to you.
  1. From the Mesh ribbon, click the Batch tool.


    Figure 14.
    The Meshing Operations dialog opens.


    Figure 15.
  2. 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.
  3. Save the model.

Run AcuSolve

  1. From the Solution ribbon, click the Run tool.


    Figure 16.
    The Launch AcuSolve dialog opens.
  2. 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.
  3. Set the Parallel processing option to Intel MPI.
  4. Optional: Set the number of processors to 4 or 8 based on availability.
  5. Expand Default initial conditions and enter the values as shown below to define the initial conditions.
  6. Click Run to launch AcuSolve.


    Figure 17.

Export Velocity Field Data

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 at the end, indicating that the simulation is complete.


Figure 18.
  1. Once the solution has converged, close the AcuTail and AcuProbe windows.
  2. Start AcuSolve Command Prompt from the Windows Start menu by clicking Start > Altair <version> > AcuSolve Cmd Prompt .
  3. In the terminal, cd to the problem directory and enter the following command:

    acuTrans -out -to cgns -outv velocity

    This will translate the velocity field data from the CFD simulation into CGNS format, which will be imported into EDEM.


    Figure 19.
    The velocity field on a cut plane at the middle of the pipe is shown below.


    Figure 20.

Part 2 - EDEM Simulation

Start Altair EDEM from the Windows start menu by clicking Start > DEM Solutions > EDEM <version>. The user interface in EDEM is divided into three tabs: Creator, Simulator and Analyst. The Creator is used to setup and initialize your model. It is where you import particles and geometries and define the other model parameters. The Simulator is where you configure and control the EDEM simulation engine, and where you can observe the progress of your simulation. The Analyst is the post-processor used to analyze and visualize the results of your simulation.

The materials, geometry sections, and particle factories are already defined in the input EDEM database. To learn more about how to set up the materials, particles, geometries, and factories, please refer to the EDEM help documentation.

Before you start the EDEM simulation, make sure that the windshifter.dem, windshifter_run1.cgns, windshifter.dll, and field_prefs_query.txt files are all in the same directory.

Open the EDEM Input Database

When you start EDEM, the Creator tab is open by default.

  1. From the menu bar, go to File > Open.
  2. In the dialog, browse to the directory where you saved the EDEM input database and open the windshifter.dem file.
  3. Verify that the bulk material, equipment material, and geometries sections have been defined properly.

Define the Physics and Import CFD Field Data

In this step, you will define the physics models for particle collisions and the particle body force.

  1. In the Creator Tree, click Physics.
  2. Click the Interaction drop-down menu and select Particle Body Force.


    Figure 21.
  3. Click Edit Contact Chain.
  4. In the dialog, select the windshifter Plug-in model then click OK.
  5. In the Creator Tree, click then browse to the problem directory where you saved the CGNS file exported using the CFD field data. Open windshifter_run1.cgns.


    Figure 22.
  6. Once the data import is complete, close the Field Data Manager dialog.
  7. Save the EDEM database.

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 database.

Define the Simulation Settings and Run the Simulation

  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 5 s and the Target Save Interval to 0.01 s.
  4. Set the Cell Size to 6 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.


    Figure 23.
  6. Once the simulation settings have been defined, click to start the EDEM simulation.

Analyze the Results

  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 on Walls.
  3. Verify that the Display Mode is set to Filled and set the Opacity to 0.2.


    Figure 24.
  4. In the Analyst Tree, expand Particles and click on Heavy particle.
  5. Change the display color to Magenta.


    Figure 25.
  6. Click on Light particle and set the display color to Green.


    Figure 26.
  7. On the menu bar, set the time to 0 by clicking:


    Figure 27.
  8. Set the View plane to + Y.


    Figure 28.
  9. In the Viewer window, set the Playback Speed to 0.5x then click on the play icon to play the particle flow animation.


    Figure 29.


    Figure 30.

    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.

  10. On the menu bar, click the Create Graph icon .
  11. In the Analyst Tree, change the plot type to Line by clicking .
  12. Click on the X-axis tab and verify that the values are set as shown in the figure below.


    Figure 31.
  13. 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.


    Figure 32.
  14. Click to add another Y-axis and set the Type to Light particle.


    Figure 33.
  15. Leave all the other options unchanged then click Create Graph to create a plot of average residence time of both the particles.


    Figure 34.

Summary

In tutorial you learned how to setup a basic AcuSolve-EDEM one-way coupling problem. In the first part, you set up and solved a steady state flow simulation using AcuSolve and then exported the CFD field data using AcuTrans. Next, you imported the CFD field data into EDEM using the Field Data Manager and defined the simulation settings. Once the EDEM simulation was completed, you learned how to create animations and plots in EDEM Analyst.