ACU-T: 3310 Single Phase Nucleate Boiling

This tutorial provides instructions for modeling a single-phase nucleate boiling using HyperWorks CFD. 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.

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-T3310_NB1_Steiner.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. 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 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-T3310_NB1_Steiner.hm and click Open.
  4. Click File > Save As.
    The Save File As dialog opens.
  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. Click the Time setting and ensure that Steady is selected.


    Figure 5.
  3. Click the Flow setting, change the radio button to Turbulent, and set the Turbulence model to Spalart-Allmaras.


    Figure 6.
  4. Click the Heat Transfer setting and activate the Heat transfer option.
  5. Click Solve for boiling to activate Nucleate Boiling.
  6. Select Vapor_Therm for the Vapor phase model.
  7. Check that the Surface tension type is set to Constant and set the Surface tension value to 0.01.


    Figure 7.
  8. Close the dialog and save the model.

Assign Material Properties

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


    Figure 8.
  2. Select the model solid.
  3. Select Water_Therm from the Material drop-down menu.


    Figure 9.
  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 10.
  2. Click on the inlet face, highlighted in the figure below.
  3. In the microdialog, enter 0.39 as the Average velocity.


    Figure 11.
  4. Click the Temperature tab in the microdialog and enter 368.15.


    Figure 12.
  5. On the guide bar, click to execute the command and exit the tool.
  6. Click the Outlet tool.


    Figure 13.
  7. Select the face highlighted in the figure below, set the Static pressure to 200000, and activate the Back flow conditions.


    Figure 14.
  8. In the Turbulence and Temperature tabs, set the back flow type to Exiting Mass Flux Average


    Figure 15.
  9. On the guide bar, click to execute the command and exit the tool.
  10. Click the No Slip tool.


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


    Figure 17.
  12. Select the next face highlighted in the figure below.
  13. In the microdialog, click the Temperature tab, set the Thermal boundary condition to Temperature and set the temperature value to 403.15.


    Figure 18.
  14. Click on the guide bar.
  15. In the Boundaries legend, double-click on Wall 1 and rename it to Heated_Wall.
  16. Double-click on Wall and rename it to Bottom.


    Figure 19.
  17. Click on the guide bar.
  18. 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, check that the Mesh growth rate is set to 1.3.


    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. Expand Default initial conditions and enter the values as shown below to define the initial conditions.


    Figure 23.
  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 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 Home tools, Files tool group, click the Open Model tool.


    Figure 24.
  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 25.
  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 26.
  7. Activate the Legend radio button then click and set the legend properties as shown below.


    Figure 27.
    The temperature contours are displayed on the model.


    Figure 28.

Summary

In this tutorial, you successfully learned how to set up and solve a simulation involving a single-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 HW-CFD post to create the contours of temperature.