ACU-T: 3310 Single Phase Nucleate Boiling

This tutorial provides instructions for modeling a single-phase nucleate boiling using HyperMesh CFD. 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.
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 is based on the popular wall heat transfer model for sub-cooled boiling (Steiner Model). 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.
Figure 1. Schematic of Channel


The dimensions of the inlet are 0.03 x 0.04 m; the inlet velocity (v) is 0.39 m/s and the temperature (T) of the fluid entering the inlets is 368.15 K (95 C).

The preheated 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 fluid in this problem is water, which has temperature dependent material properties: density, viscosity, enthalpy and conductivity. There are also surface tension and vapor phase models specified for this material.

Water vapor which also has temperature dependent material properties is specified as the vapor phase model.

The AcuSolve simulation will be set up to model steady state heat transfer to determine the temperature and heat flux on the heated walls of the manifold.

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-T3310_NB1_Steiner.hm and click Open.
  4. Click File > Save As.
  5. Create a new directory named NB1 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 NB1_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

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:
    1. Verify that Time marching is set to Steady.
    2. Select Spalart-Allmaras as the Turbulence model.
    3. Activate the Heat transfer checkbox.
    4. Click the Solve for boiling checkbox to activate Nucleate Boiling.
    5. Select Vapor_Therm for the Vapor phase model.
    6. Check that the Surface tension type is set to Constant and set the Surface tension value to 0.01.
    Figure 5.


  3. Close the dialog and save the model.

Assign Material Properties

  1. From the Flow ribbon, click the Material tool.
    Figure 6.


  2. Select the model solid.
  3. Select Water_Therm from the Material drop-down menu.
    Figure 7.


  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 8.


  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 9.


  4. On the guide bar, click to execute the command and exit the tool.
  5. Click the Outlet tool.
    Figure 10.


  6. Select the face highlighted in the figure below, set the Static pressure to 200000, and activate the Back flow conditions.
    Figure 11.


  7. In the Turbulence and Temperature tabs, set the back flow type to Exiting Mass Flux Average
    Figure 12.


  8. On the guide bar, click to execute the command and exit the tool.
  9. Click the No Slip tool.
    Figure 13.


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


  11. Select the next face highlighted in the figure below.
  12. In the microdialog, click the Temperature tab, set the Thermal boundary condition to Temperature and set the temperature value to 403.15.
    Figure 15.


  13. Click on the guide bar.
  14. In the Boundaries legend, double-click on Wall 1 and rename it to Heated_Wall.
  15. Double-click on Wall and rename it to Bottom.
    Figure 16.


  16. Click on the guide bar.
  17. 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 17.


  2. In the Meshing Operations dialog, check that the Mesh growth rate is set to 1.3.
    Figure 18.


  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 19.


    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 and enter the values as shown below to define the initial conditions.
    Figure 20.


  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

  1. Once the solution is completed, navigate to the Post ribbon.
  2. From the Home tools, Files tool group, click the Open Model tool.
    Figure 21.


  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 22.


  4. To check the temperature contours on the Heated_Wall and Bottom surfaces, right-click on those surfaces in the Post Browser and select Isolate.
  5. In the Post Browser, right-click on Heated_Wall and Bottom again and select Edit.
    A surface coloring microdialog opens.
  6. Set the Display option to Temperature.
    Figure 23.


  7. Activate the Legend radio button then click and set the legend properties as shown below.
    Figure 24.


    The temperature contours are displayed on the model.
    Figure 25.


Summary

In this tutorial, you successfully learned how to set up and solve a simulation involving a single-phase nucleate boiling using HyperMesh 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 HyperMesh CFD Post to create the contours of temperature.