ACU-T: 4101 T-Junction Flow using the Eulerian Multiphase Model

Prerequisites

This tutorial provides the instructions for setting up and running a basic transient multiphase simulation using the Eulerian multiphase model. Prior to starting this tutorial, you should have already run through the introductory tutorial, ACU-T: 1000 UI Introduction, and have a basic understanding of HyperMesh CFD and AcuSolve. To run this simulation, you will need access to a licensed version of HyperMesh CFD and AcuSolve.

Before you begin, copy the file(s) used in this tutorial to your working directory.

Problem Description

The problem to be addressed in this tutorial is shown schematically in Figure 1. An Air-Water mixture is entering a t-junction pipe through the inlet with a carrier (Water) volume fraction of 0.98. The diameter of the disperse field is 0.001 m. The velocity of the incoming carrier field (Water) is 1.5 m/s, while the velocity of the disperse field (Air) is set to 1.6 m/s. The simulation will be solved as a 2D-problem, therefore a slip condition is applied on the top and bottom surfaces.
Figure 1.


Start HyperMesh CFD and Open the HyperMesh Database

  1. Start HyperMesh CFD from the Windows Start menu by clicking Start > Altair <version> > HyperMesh 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-T4101_TJunction.hm and click Open.
  4. Click File > Save As.
  5. Create a new directory named T_Junction 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 T_Junction 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 Eulerian.
  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 Eulerian 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 WaterAirEul.
  7. Set the Carrier field to Water and the Disperse field to Air.
  8. Set the diameter, drag model, and other 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 Eulerian Material to WaterAirEul.
  11. Set Time step size and Final time to 0.01 and 1, 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 WaterAirEul 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, activate Phasic inflow and then change the inflow velocity type to Normal.
  4. Enter a value of 1.5 and 1.6 m/s for the Normal velocity of the Carrier Field and Disperse Field, respectively.
  5. Set the Volume fraction specification type to Value and set the Carrier fluid volume fraction to 0.98.
    Figure 11.


  6. Click the Turbulence tab in the microdialog. Set the Turbulence input type to Direct and the Eddy viscosity to 0.001.
    Figure 12.


    Note: When phasic inflow is active, Turbulence input type = Direct should be used.
  7. On the guide bar, click to execute the command and exit the tool.
  8. Click the Outlet tool.
    Figure 13.


  9. Select the face highlighted below and verify the settings in the microdialog.
    Figure 14.


  10. On the guide bar, click to execute the command and remain in the tool.
  11. With the Outlet tool still active, select the face highlighted below after rotating the model. Then click on the guide bar.
    Figure 15.


  12. Click the Slip tool.
    Figure 16.


  13. Select the top and bottom faces highlighted below then click on the guide bar.
    Figure 17.


  14. 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 18.


    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 0.0025.
    Figure 19.
  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 20.


    The Field Output dialog opens.
  2. Check the box for Write Initial Conditions.
  3. Set the time interval to 1.
    Figure 21.


Run AcuSolve

  1. From the Solution ribbon, click the Run tool.
    Figure 22.


    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 23.


  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 HM-CFD Post

In this step, you will create contour plots for velocity and field 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 24.


  4. In the modeling window, select the top slip surface.
  5. In the microdialog, set the display variable to velocity.
  6. Activate the Legend toggle and set the legend limits to 0 and 2.5, respectively.
  7. Click and set the colormap properties as shown below.
    Figure 25.


  8. Click on the guide bar to create the velocity contour plot.
    Figure 26.


  9. In the Post Browser, right-click Boundary Group 7 and select Edit.
  10. In the microdialog, change the display variable to volume fraction: air and set the legend limits to 0 and 0.1.
  11. Click on the guide bar to create the volume fraction contour plot.
    Figure 27.


Summary

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