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

This tutorial provides instructions for modeling 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 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.

Before you begin, copy the file(s) used in this tutorial to your working directory.
Note: This tutorial does not cover the steps related to geometry cleanup and mesh settings.

Problem Description

The problem to be addressed in this tutorial is shown schematically in Figure 1. It consists of a channel with a heated wall at the bottom. The temperature of the wall is selected to onset the nucleate boiling at the heated wall.

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 ℃.

The pre-heated air enters the inlets and heat is transferred to the fluid from the walls. The heat causes sub-cooled boiling to occur in the region close to the wall and leads to formation of bubbles at nucleation sites.

The heat transfer in this regime is basically dominated by two effects, the macro convection due to the motion of the bulk liquid and the latent heat transport associated with the evaporation of the liquid micro-layer between the bubble and the heated wall.

The Algebraic Eulerian (AE) model is used to simulate the heat transfer and momentum exchange between a carrier field and a dispersed field.

Figure 1. Schematic of Channel

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 and click Open.
  4. Click File > Save As.
  5. Create a new directory named NB2 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 NB2_Steiner 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

Verify and Create Materials

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

    Figure 4.
    The Material Library dialog opens.
  2. Under Settings, click Fluid, then click the My Materials tab.
  3. Verify that the material Water_NB has the properties shown below.

    Figure 5.
  4. Under Settings, click Boiling Multiphase, then click the My Materials tab.
  5. Click to create a new material.
  6. Name the material Boiling_NB and verify the following properties in the microdialog.

    Figure 6.

Set the General Simulation Parameters

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

    Figure 7.
    The Setup dialog opens.
  2. Under the Physics models setting:
    1. Activate the Multiphase flow radio button.
    2. Set the Multifluid type to Boiling and the Boiling material to Boiling_NB.
    3. Ensure that the Time step size is 0.01.
    4. Select Spalart-Allmaras as the Turbulence model.
    5. Set the Gravity value to -9.81 in the z direction.
    6. Set the Pressure scale to Gauge then click besides the drop-down and set the Absolute pressure offset to 200000.

    Figure 8.
  3. 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 40.
    4. The Flow, Temperature, Multifluid, and Turbulence checkboxes are activated.

    Figure 9.
  4. Close the dialog and save the model.

Assign Material Properties

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

    Figure 10.
  2. Select the model solid.
  3. Select Boiling_NB from the Material drop-down menu.

    Figure 11.
  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 12.
  2. Click on the inlet face, highlighted in the figure below.
  3. In the microdialog, enter 0.39 for the Average velocity and 368.15 for the Temperature.

    Figure 13.
  4. On the guide bar, click to execute the command and exit the tool.
  5. Click the Outlet tool.

    Figure 14.
  6. Select the face highlighted in the figure below then click on the guide bar.

    Figure 15.
  7. Click the No Slip tool.

    Figure 16.
  8. Select the face highlighted in the figure below to create the Heated_wall face.

    Figure 17.
  9. Click the Temperature tab in the microdialog, set the Thermal Boundary condition to Temperature, and set the Temperature value to 403.15.

    Figure 18.
  10. On the guide bar, click to execute the command and remain in the tool.
  11. In the Boundaries legend, right-click on Wall, select Rename, and enter Heated_wall.

    Figure 19.
  12. Select the 8 highlighted surfaces shown in the figure below to create the Bottom_wall faces then click on the guide bar.

    Figure 20.
  13. In the Boundaries legend, rename Wall to Bottom_wall.
  14. From the Solution ribbon, click the Field tool.

    Figure 21.
    The Field Output dialog opens.
  15. Set the Time step interval to 10.

    Figure 22.
  16. 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 Volume tool.

    Figure 23.
  2. In the Meshing Operations dialog, set the Average Element size to 0.004 (if not set already).

    Figure 24.
  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 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. 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 enter the values as shown below to define the initial conditions.

    Figure 26.
  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 solution process.

Post-Process the Results with HW-CFD Post

  1. Once the solution is completed, navigate to the Post ribbon.
  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 27.
  4. To check the contours of volume fraction of vapor on the Heated_Wall and Bottom_wall surfaces, right-click on those surfaces in the Post Browser and select Isolate.
  5. From the Post ribbon, click the Boundary Groups tool.

    Figure 28.
  6. Select all the surfaces on the model.
  7. In the microdialog, set the Display option to volume fraction vapor.
  8. Activate the Legend radio button then click and set the legend properties as shown below.

    Figure 29.
  9. Click on the guide bar.
  10. Move the slider at the bottom of the modeling window to 4/4.
    The volume fraction of vapor contours are displayed on the model.

    Figure 30.


In this tutorial, you successfully learned how to set up and solve a simulation involving a two-phase nucleate boiling using HyperWorks CFD. You started by opening the HyperMesh input file with the geometry and then defined the simulation parameters and flow boundary conditions. Once the solution was computed, you used HyperWorks CFD Post to create the contours of volume fraction of vapor.