ACU-T: 3311 Multiphase Nucleate Boiling Using the Algebraic Eulerian Model


This tutorial provides instructions for running a transient simulation of a two-phase Nucleate Boiling 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 HyperWorks UI Introduction, and have a basic understanding of HyperMesh, 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, the Steiner problem is attached here to show the capability of the Multiphase Nucleate Boiling modeling in AcuSolve. The Algebraic Eulerian (AE) model with phase change is used to simulate the heat transfer and momentum exchange between a carrier field and a dispersed field.

In this problem, water is considered a carrier field material and vapor is considered a dispersed field material. Water at 2 bar pressure and 95℃ temperature enters the inlet at an average velocity of 0.39 m/sec and passes through the heated wall which is maintained at 130 ℃.

Figure 1. Schematic of Channel

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 Multiphase_NB 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 Steiner 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 Abs. pressure offset to 200000.
  4. Set the Turbulence model to Spalart Allmaras.
  5. Set the Temperature equation to Advective Diffusive.
  6. Set Multiphase equation to Algebraic Eulerian.
  7. Set the Global Gravity in the Z direction to -9.8.

    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 40.
  3. Set the Initial time increment to 0.01.
  4. Set the Min stagger iterations to 2.
  5. Set the Max stagger iterations to 4.
  6. Set the Relaxation factor to 0.
  7. Verify that the Flow, Turbulence, and Field settings are turned On.

    Figure 3.

Define the Nodal Outputs

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

    Figure 4.

Set Up Material Model Parameters

In this step, you will start by creating a new material named Vapor. Then, you will set up the Multiphase material model.

  1. In the Solver Browser, expand 02.Materials.
  2. Right-click on FLUID and select Create to create a new fluid material. Name it Vapor.
  3. In the Entity Editor, set the Density value to 1.128.
  4. Set the Specific heat value to 2174.59.
  5. Change the Latent heat type to Constant.
  6. Set the Latent heat value to 2256000.
  7. Set the Latent heat temperature value to 393.45.
  8. Set the Viscosity value to 1.29e-05.
  9. Set the Conductivity value to 0.02749.

    Figure 5.
  10. In the Solver Browser, under FLUID, click Water_HM and change the material properties.
    1. Change the Density to 956.36.
    2. Change the Specific heat to 4204.8.
    3. Change the Viscosity to 0.000314.
    4. Change the Conductivity to 0.675.
  11. In the Solver Browser, under 02.Materials, right-click on MULTIPHASE and select Create to create a new multiphase material. Name it VapourWater-Eulerian_HM.
  12. In the Entity Editor, verify that the Field Interaction Type is set to Algebraic Eulerian.
  13. Set Water_HM as the Carrier Material if it's not already set.
    Since Water is the carrier field for this analysis, leave this option as is.
  14. Verify that the Number of Dispersed Field is set to 1.

    Figure 6.
  15. Activate the check box beside Edit Field Interaction Models.
    The Field Interaction Model dialog opens.
  16. In the dialog, set the Dispersed Field 1 Material to Vapor.
  17. Activate the Enable Phase change check box.
  18. Set Phase change type to Wall boiling if not set.
  19. Set Dispersed field diameter type to Boiling Kurul exponential.

    Figure 7.
  20. Click Save & Close.

Set Up Boundary Conditions and Nodal Initial Conditions

Set Up Boundary Conditions and Nodal Initial Conditions

In this step, you will assign the material properties to the multiphase fluid volume and then assign surface boundary conditions.

  1. In the Solver Browser, expand 11.Volumes > MULTIPHASE.
  2. Click FluidVolume. In the Entity Editor,
    1. Change the Type to MULITPHASE if not set.
    2. Set VaperWater_Eulerian_HM as the Material.

    Figure 8.
  3. In the Solver Browser, expand 12.Surfaces > INFLOW.
  4. Click Inflow. In the Entity Editor,
    1. Change the Type to INFLOW if not set.
    2. Set the Inflow type to Average velocity.
    3. Set the Average velocity to 0.39 m/sec.
    4. Set the Temperature to 368.15.

      Figure 9.
    5. Set the No. of multiphase incoming fields to 2 and press Enter.
    6. In the dialog, select Water_CF.VaporWater_Eulerian_HM as the first Incoming Field and set its Volume Fraction to 1.
    7. Similarly, select Vapor_DF1. VaporWater_Eulerian_HM as the second Incoming Field and set its Volume Fraction to 0.

      Figure 10.
    8. Click Save and Close.
  5. Similarly, expand OUTFLOW then click the Outflow component. In the Entity Editor, change the Type to OUTFLOW if not set.

    Figure 11.
  6. Similarly, expand WALL then click the Side_MaxY component. In the Entity Editor, verify that the Type is set to WALL.

    Figure 12.
  7. Similarly, click the Side_MaxY, Top, and Bottom components and verify that the Type is set to WALL.
  8. Click HeatedWall. In the Entity Editor,
    1. Verify that the Type is set to WALL.
    2. Set Temperature BC type to Value.
    3. Set the Temperature value to 403.15.

    Figure 13.
  9. Save the model.

Set the Nodal Initial Conditions

  1. In the Solver Browser, expand 01.Global then click 03.NODAL_INTIAL_CONDITION.
  2. In the Entity Editor, set the x-Velocity value to 0.39.
  3. Set the default value of Temperature to 368.15.
  4. In the Field tab, set the No. of Fields to 2 then press Enter.
  5. In the Fields dialog, set the values shown in the figure below.

    Figure 14.
  6. Click Save & Close.
  7. Save the model.

Compute the Solution

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

  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. Verify that the Output time steps is set to All.
  5. Leave the remaining options as default and click Launch to start the solution process.

    Figure 15.

Post-Process the Results with HyperView

Once the AcuSolve run is complete, close the HyperWorks Solver View dialog. In the HyperMesh Desktop window, close the AcuSolve Control and Solver job Launcher dialogs. In the next few steps, you will plot a contour of the vapor volume fraction.

Switch to the HyperView Interface and Load the AcuSolve Model and Results

  1. In the HyperMesh Desktop window, click the ClientSelector drop-down in the bottom-left corner of the graphics window.

    Figure 16.
  2. Select HyperView from the list.
  3. In the pop-up dialog that appears, click Yes.
    The interface is changed to HyperView.

    Once HyperView is loaded, the Load model and results panel should be open by default. If you do not see the panel, click File > Open > Model.

  4. In the Load model and results panel, click next to Load model.
  5. 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 Steiner.1.Log.
  6. Click Open.
  7. Click Apply in the panel area to load the model and results.
    The model is colored by geometry after loading.

Create Contours for the Volume Fraction of Vapor

In this step, you will display volume fraction contours of vapor.
  1. Since this is a transient case, you need to plot the results at the last timestep. To do this, click the Time drop-down menu in the Results Browser and select the last option in the list.

    Figure 17.
  2. In the Results Browser, expand the list of Components.
  3. Click the Isolate Shown icon , hold Ctrl, then select the HeatedWall and Bottom components to turn off the display of all components except those that are required.

    Figure 18.
  4. Click on the Results toolbar to open the Contour panel.
  5. In the panel area, change the Result type to Volume_fraction-1-Vapor_DF1.VaporWater_Eulerian_HM(s).
  6. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
  7. Click Apply to plot the vapor volume fraction contours.
  8. In the panel area, under the Display tab, turn off the Discrete color option.

    Figure 19.
  9. Click the Legend tab then click Edit Legend. In the dialog, change the Numeric format to Fixed then click OK.
    The contour plot should look similar to the figure below.

    Figure 20.


In this tutorial, you worked through a basic workflow to set-up and solve a transient two-phase Nucleate Boiling flow problem using the Algebraic Eulerian multiphase model. You started by importing the model in HyperMesh. Then, you defined the simulation parameters and launched AcuSolve directly from within HyperMesh. Upon completion of solution by AcuSolve, you used HyperView to post-process the results and create a contour plot of the volume fraction.