ACU-T: 4102 Fluidized Bed using the Granular Multiphase Model

Prerequisites

This tutorial provides the instructions for setting up and running a gas-solid fluidized bed simulation using the granular multiphase model. 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 and AcuSolve. To run this simulation, you will need access to a licensed version of HyperWorks CFD and AcuSolve.

Prior to running through this tutorial, click here to download the tutorial models. Extract ACU-T4102_FluidizedBed.hm from HyperWorksCFD_tutorial_inputs.zip.

Problem Description

The problem to be addressed in this tutorial is shown schematically in . Some of the most common applications of the granular multiphase model are fluidized beds, mixing tanks, sedimentation of particles in liquid columns, and so on. In this tutorial, you will set up and run a gas-particle fluidized bed. The inlet velocity used for the simulation is 0.3 m/s and the initial bed height is 0.2 m. The initial solid packing fraction is set to 0.63.


Figure 1.
For simplicity, the gas and solid phase material models have already been defined in the input file that is provided. The steps for creating the granular multiphase material model are included in the tutorial. For information about creating fluid and solid material models, please refer to the introductory tutorials. The summary of the material models have been listed below.
Phase Density (kg/m3) Viscosity (Pa s)
Gas 21.56 1.781e-05
Particle 910 -

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 2.
    The Open File dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file ACU-T4102_FluidizedBed.hm and click Open.
  4. Click File > Save As.
  5. Create a new directory named Fluidized_Bed and navigate into this directory.
    This will be the working directory and all the files related to the simulation will be stored in this location.
  6. Enter Fluidized_Bed as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

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 3.

Set Up Flow

Set the General Simulation Parameters

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


    Figure 4.
    The Setup dialog opens.
  2. Under the Physics models setting, select the Multiphase flow radio button.
  3. Change the Multifluid type to Granular.
  4. Click the Granular 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 Granular Multiphase, switch to the My Material tab, then click to add a new material.
  6. In the microdialog, click on the top-left corner and change the name to gas-particle.
  7. Set the Carrier field to gas and the Disperse field to particle.
    Note: The input file provided with the tutorial has a predefined gas and particle material models in it.
  8. Set the diameter, drag model, and other granular parameters as shown in the image below.


    Figure 5.
  9. Close the material model microdialog and then close the Material Library dialog.
  10. In the Setup dialog, set the Granular Material to gas-particle.
  11. Set Time step size and Final time to 0.005 and 7, respectively. Select Spalart-Allmaras for the Turbulence model.
  12. Set the gravity to 0, -9.81, 0 and the pressure scale to Absolute.


    Figure 6.
  13. Click the Solver controls setting and set the Minimum and Maximum stagger iterations to 2 and 4, respectively.


    Figure 7.
  14. Close the dialog and save the model.

Assign Material Properties

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


    Figure 8.
  2. Verify that gas-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, click the Constant tool.


    Figure 9.
  2. Click the inlet face highlighted in the figure below.


    Figure 10.
  3. In the microdialog, enter the values shown in the figure below.


    Figure 11.
  4. In the turbulence tab, set the turbulence input type to Direct and set the eddy viscosity value to 0.0001.


    Figure 12.
  5. On the guide bar, click to execute the command and exit the tool.
  6. Click the Outlet tool.


    Figure 13.
  7. Select the face highlighted below and verify the settings in the microdialog.


    Figure 14.
  8. Click on the guide bar.
  9. Click the Slip tool.


    Figure 15.
  10. Select the top and bottom faces highlighted below then click on the guide bar.


    Figure 16.
  11. Save the model.

Generate the Mesh

The meshing parameters for this tutorial are already set in the input file.
  1. From the Mesh ribbon, click the Volume tool.


    Figure 17.
    Note: If the model has not been validated, you are prompted to create the simulation model before running the batch mesh.
  2. In the Meshing Operations dialog, check that the Average Element size is set to 0.01.


    Figure 18.
  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.

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.


    Figure 19.
    The Field Output dialog opens.
  2. Check the box for Write Initial Conditions.
  3. Set the time interval to 10.


    Figure 20.

Define the Nodal Initial Conditions

In this step, you’ll define the nodal initial condition for the volume fraction of the gas and solid phases.
  1. From the Solution ribbon, click the Plane tool.


    Figure 21.
  2. Select the solid in the modeling window.
  3. On the guide bar, change the active selection to Plane.
  4. Click anywhere on the solid body to define the plane location. By default, the plane normal is aligned with the y-axis.
  5. In the variable dialog, click in the top-left corner and select Carrier Volume Fraction.


    Figure 22.
  6. Click on the white space in the dialog and set the value of the carrier volume fraction to 0.37.
  7. Click in the top-right corner of the dialog.
    The Vector tool appears, which can be used change the location and orientation of the plane defining the initial condition.
  8. In the Vector tool, verify that the orientation of the tool is along the negative y-axis then click XYZ.


    Figure 23.
  9. Enter the coordinates of the center of plane as shown in the figure below.


    Figure 24.
  10. Click on the guide bar then save the model.

Run AcuSolve

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


    Figure 25.
    The Launch AcuSolve dialog opens.
  2. Set the Parallel processing option to Intel MPI.
  3. Optional: Set the number of processors to 4 or 8 based on availability.
  4. Expand Default initial conditions, uncheck Pre-compute flow, and set the velocity values to 0. Uncheck Pre-compute Turbulence.


    Figure 26.
  5. Click Run to launch AcuSolve.
    The Run Status dialog opens. Once the run is complete, the status is updated and you can close the dialog.
    Tip: While AcuSolve is running, right-click on the AcuSolve job in the Run Status dialog and select View Log File to monitor the solution process.

Post-Process the Results with HW-CFD Post

In this step, you will create a contour plot for the particle volume fraction.
  1. Once the solution is complete, right-click the AcuSolve run in the Run Status dialog and select Visualize results.
  2. Once the results are loaded in the Post ribbon, click the Top face of the view cube to orient to the xy-plane.
  3. Click the Boundary Groups tool.


    Figure 27.
  4. In the modeling window, select the top slip surface.
  5. In the microdialog, set the display variable to volume fraction:particle.
  6. Activate the Legend toggle and set the legend limits to 0 and 0.63, respectively (if not already set).
  7. Click and set the colormap properties as shown below.


    Figure 28.
  8. Click on the guide bar to create the volume fraction contour plot.
  9. Click the play icon at the bottom of the modeling window to play the animation.


    Figure 29.

Summary

In this tutorial, you learned how to set up and solve a fluidized bed simulation using the Granular multiphase model available in AcuSolve using HyperWorks CFD. You started by importing the HyperWorks CFD input database and then defined the flow setup. Once the solution was computed, you created a contour plot of particle volume fraction using HyperWorks CFD Post.