ACU-T: 4100 Multiphase Flow using Algebraic Eulerian Model

This tutorial provides instructions for running a transient simulation of a two-phase flow in a pipe using the Algebraic Eulerian model. Prior to starting this tutorial, you should have already run through the introductory tutorial, ACU-T: 1000 Basic Flow Set Up, 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, copy HyperWorksCFD_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract ACU-T4100_LPipe.hm 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 addressed in this tutorial is shown schematically in Figure 1. The Algebraic Eulerian (AE) model is used to simulate the momentum exchange between a carrier field and a dispersed field. When simulating multiphase flows using the AE model, the carrier field has to be a fluid and the dispersed field can be of any medium.

In this problem, Water is considered a Carrier field material and Air is considered as Dispersed field material. Fluid enters the Inlet at an Average Velocity of 1 m/sec and the Water and Air volume fractions at the inlet are 96% and 4% respectively.



Figure 1.

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-T4100_LPipe.hm and click Open.
  4. Click File > Save As.
    The Save File As dialog opens.
  5. Create a new directory named Algebraic_Eulerian 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 LPipe_Disperse 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

Create Materials

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


    Figure 4.
    The Material Library dialog opens.
  2. Under Settings, click Disperse Multiphase, then click the My Materials tab.
  3. Click to create a new material.
  4. Name the material Air in Water and assign the properties shown below.


    Figure 5.

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, change the option to Transient, and ensure that the Time step size is 0.01.


    Figure 7.
  3. Click the Flow setting, then:
    1. Change the option to Turbulent.
    2. Set the Turbulence model to Spalart-Allmaras.
    3. Check the Include Gravitational Acceleration option and set the Gravity value to -9.81 in the y direction.


    Figure 8.
  4. Click the Multifluid setting, set the Multifluid type to Disperse, and the Boiling material to Air in Water.


    Figure 9.
  5. Click the Solver controls setting and verify that:
    1. Minimum stagger iteration is set to 2.
    2. Maximum stagger iteration is set to 4.
    3. Transient maximum step is set to 150.
    4. The Flow, Multifluid, and Turbulence checkboxes are activated.


    Figure 10.
  6. Close the dialog and save the model.

Assign Material Properties

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


    Figure 11.
  2. Select the model solid.
  3. Select Air in Water from the Material drop-down menu.


    Figure 12.
  4. On the guide bar, click to execute the command and exit the tool.

Define Flow Boundary Conditions

  1. From the Flow ribbon, Profiled tool group, click the Profiled Inlet tool.


    Figure 13.
  2. Click on the inlet face, highlighted in the figure below.


    Figure 14.
  3. In the microdialog, enter 1.0 for the Average velocity and 0.96 for the Carrier fluid volume fraction.


    Figure 15.
  4. On the guide bar, click to execute the command and exit the tool.
  5. Click the Outlet tool.


    Figure 16.
  6. Select the face highlighted in the figure below then click on the guide bar.


    Figure 17.
  7. Click the Slip tool.


    Figure 18.
  8. Select the top and bottom faces highlighted below then click on the guide bar.


    Figure 19.
  9. 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 20.
  2. In the Meshing Operations dialog, set the Average Element size to 0.00104 (if not set already).


    Figure 21.
  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.

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. Check the box for Use hybrid message passing and set the number of threads to the same as the number of processors.
  5. Expand Default initial conditions and verify that the Carrier field volume fraction is 1.0.


    Figure 23.
  6. 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 AcuSolve solution process.

Post-Process the Results with HW-CFD Post

  1. Once the solution is completed, navigate to the Post ribbon.
    Important: In order to access the Post ribbon in HyperWorks CFD, you have to set the following environment variable: HWCFD_Post=1.
  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.


    Figure 24.
  4. In the Post Browser, right-click on the Slip surface and select Isolate.
  5. Right-click on Slip again and select Edit.
  6. In the microdialog, set the Display option to Volume fraction air.
  7. Activate the Legend radio button then click and set the Colormap name to Rainbow Uniform.


    Figure 25.
    The volume fraction of air contours are displayed on the model.


    Figure 26.

Summary

In this tutorial, you worked through a basic workflow to set up and solve a transient multiphase flow problem using the Algebraic Eulerian multiphase model in HyperWorks CFD. You started by opening the HyperMesh input file with the geometry and then defined the simulation parameters and flow boundary conditions. Upon completion of the solution by AcuSolve, you used HyperWorks CFD Post to post-process the results and create a contour plot of volume fraction.