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 HyperWorks tutorial, ACU-T: 1000 HyperWorks UI Introduction, and have a basic understanding of HyperWorks, AcuSolve, and HyperView. To run this simulation, you will need access to a licensed version of HyperMesh and AcuSolve.

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

Since the HyperMesh database (.hm file) contains meshed geometry, this tutorial does not include steps related to geometry import and mesh generation.

Problem Description

The problem to be addressed in this tutorial is shown schematically in Figure 1. As an example, an LPipe problem is attached here to show the capability of the Disperse modeling in AcuSolve. 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 heavier fluid (or higher density fluid).

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.

Open the HyperMesh Model Database

  1. Start HyperMesh and load the AcuSolve user profile.
    Refer to the HM introductory tutorial, ACU-T: 1000 HyperWorks UI Introduction, to learn how to select AcuSolve from User Profiles.
  2. Click the Open Model icon located on the standard toolbar.
    The Open Model dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file and click Open.
  4. Click File > Save As.
    The Save Model As dialog opens.
  5. Create a new directory named Lpipe_Disperse 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 as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Set the General Simulation Parameters

Set the Analysis Parameters

  1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
  2. In the Entity Editor, set the Analysis type to Transient.
  3. Set the Turbulence Model to Spalart Allmaras.
  4. Set Multiphase equation to Algebraic Equation.

    Figure 2.

Specify the Solver Settings

  1. In the Solver Browser, click 02.SOLVER_SETTINGS under 01.Global.
  2. In the Entity Editor, set the Max time steps to 150.
  3. Set the Initial time increment to 0.01 sec.
  4. Set the Min stagger iterations to 2.
  5. Set the Max stagger iterations to 4.
  6. Change the Relaxation factor to 0.
  7. Verify that Flow, Turbulence, and Field are turned On.

    Figure 3.

Define the Nodal Outputs

  1. In the Solver Browser, expand 17.Output and click on NODAL_OUTPUT.
  2. In the Entity Editor, set Time step frequency to 10.
  3. Toggle On the Output initial condition field.

    Figure 4.

Set Up Material Model Parameters and Body Force

In this step, you will start by setting up the Multiphase material model and body force parameters. Then, you will assign the surface boundary conditions and material properties to the fluid volume.

Set Up Material Model Parameters

  1. In the Solver Browser, expand 02.Materials > MULTIPHASE and click on AirWater Eulerian HM.
  2. In the Entity Editor, verify that the Field Interaction Type is set to Algebraic Eulerian.
  3. By default, Water_HM is set as the Carrier Material. Since water is the carrier field for this analysis, leave this option as is.
  4. Verify that the Number of Dispersed Field is set to 1.

    Figure 5.
  5. Activate the check box beside Edit Field Interaction Models.
    The Field Interaction Model dialog opens.
  6. In the dialog, set the Dispersed Field 1 Material to Air_HM, if not set already.

    Figure 6.
  7. Click Save and Close.

Set Up the Body Force

  1. In the Solver Browser, expand 03.Body_Force then expand BODY_FORCE and click on Gravity_HM.
  2. In the Entity Editor, set the Z gravity to 0.0 and change the Y gravity to -9.81 m/sec2.

    Figure 7.

Set Up Boundary Conditions and Nodal Initial Conditions

Assign Boundary Conditions and Material Properties

By default, all components are assigned to the wall boundary condition. In this step, you will change them to the appropriate boundary conditions and assign material properties to the fluid volumes.
  1. In the Solver Browser, expand 12.Surfaces > WALL.
  2. Click Fluid. In the Entity Editor,
    1. Change the Type to MULTIPHASE.
    2. Select AirWater_Eulerian_HM as the Material.
    3. Set Body force to Gravity_HM.

    Figure 8.
  3. Click Inflow. In the Entity Editor,
    1. Change the Type to INFLOW.
    2. Set the Inflow type to Average velocity.
    3. Set the Average velocity to 1.0 m/s.
    4. Set No. of multiphase incoming fields to 2.0 and press Enter on the keyboard.

      Figure 9.
      The Incoming Fields dialog opens.
    5. Select Air_HM_DF1.AirWater_Eulerian_Hm as the first Incoming Field and set Volume Fractions to 0.04.
    6. Select Water_HM_CF.AirWater_Eulerian_Hm as the second Incoming Field and set Volume Fraction to 0.96.

      Figure 10.
    7. Click Save & Close.
  4. Click Outflow. In the Entity Editor, change the Type to OUTFLOW.

    Figure 11.
  5. Click Wall. In the Entity Editor, verify that the Type is set to WALL.

    Figure 12.
  6. Click Slip_1. In the Entity Editor, change the Type to SLIP.

    Figure 13.
  7. Similarly, change the Type to SLIP for the Slip_2 component.
  8. Save the model.

Set the Nodal Initial Conditions

  1. In the Solver Browser, expand the 01.Global tree then expand 03.NODAL_INITIAL_CONDITION and click on NODAL_INITIAL_CONDITION.
  2. In the Entity Editor, verify that the default value for Eddy viscosity is set to 0.0001 m2/sec.
  3. Under the Field tab, set the No. of Fields to 2 and press Enter.

    Figure 14.
    The Fields dialog opens.
  4. Set the fields as shown in the figure below.

    Figure 15.
  5. Click Save & Close.
  6. Save the model.

Compute the Solution

In this step, you will launch AcuSolve directly from HyperMesh and compute the solution.

Run AcuSolve

  1. Turn on the visibility of all mesh components.
    For the analysis to run, the mesh for all active components must be visible.
  2. Click on the ACU toolbar.
    The Solver job Launcher dialog opens.
  3. Optional: For a faster solution time, set the number of processors to a higher number (4 or 8) based on availability.
  4. The Output time steps can be set to All or Final. Since this is a Transient analysis, set it to All.
  5. Leave the remaining options as default and click Launch to start the solution process.

    Figure 16.

Post-Process the Results with HyperView

Once the solution has converged, close the AcuProbe and AcuTail windows. Go to the HyperMesh window and close the AcuSolve Control tab.

Open HyperView and Load the Model and Results

  1. In the HyperMesh main menu area, click Applications > HyperView.
    Once the HyperView window is loaded, the Load model and results panel should be open by default. If you do not see the panel, click File > Open > Model.
  2. In the Load model and results panel, click next to Load model.
  3. In the Load Model File dialog, navigate to your working directory and select the AcuSolve .Log file for the solution run that you want to post-process. In this example, the file to be selected is LPipe.1.Log.
  4. Click Open.
  5. Click Apply in the panel area to load the model and results.
    The model is colored by geometry after loading.

Create Contours for Volume Fraction of Water

In this step, you will create a contour plot of the volume fraction of water at the end of the simulation.
  1. In the Results Browser, set the Time to 1.5 sec.

    Figure 17.
  2. In the Results Browser, expand the list of Components.
  3. Click the Isolate shown icon and then click on the Fluid component to turn off the display of all components except the Fluid component.

    Figure 18.
  4. Orient the display to the xy-plane by clicking on the Standard Views toolbar.
  5. Click on the Results toolbar to open the Contour panel.
  6. From the top drop-down menu under the Result type, select Volume_fraction-2-Water_HM_CF.AirWater_Eulerian(s).
  7. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
  8. In the panel area, click Apply.
  9. In the panel area, under the Display tab, turn off the Discrete color option.

    Figure 19.
  10. Click the Legend tab then click Edit Legend.
  11. In the Edit Legend dialog, change the Numeric format to Fixed. In the Values section, click on the Minimum value in the legend and set it to 0.80. Similarly, set the Maximum value to 1.0.

    Figure 20.
  12. Click OK to close the dialog.
  13. Verify that the contour plot looks like the figure below at frame 16.

    Figure 21.


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 using HyperWorks products, namely HyperMesh and AcuSolve. You started by importing the model in HyperMesh. Then, you defined the simulation parameters and launched AcuSolve directly from within HyperMesh. Upon completion of the solution by AcuSolve, you used HyperView to post-process the results and created a contour plot of the volume fraction.