ACU-T: 3310 Single Phase Nucleate Boiling

Prerequisites

This tutorial introduces you to setting up and solving a single phase nucleate boiling problem using HyperMesh. 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 HyperMesh, AcuSolve, and HyperView. To run this simulation, you will need access to a licensed version of HyperMesh and AcuSolve.

Prior to running through this tutorial, copy HyperMesh_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract ACU-T3310_NB1.hm from HyperMesh_tutorial_inputs.zip.

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. 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.

Open the HyperMesh Model Database

  1. Start HyperMesh Desktop 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 ACU-T3310_NB1.hm and click Open.
  4. Click File > Save As.
    The Save Model 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.

Set the Simulation Parameters

Set the General Simulation Parameters

  1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
  2. In the Entity Editor, verify that the Analysis type is set to Steady State.
  3. Set the Abs. pressure offset to 200000 N/m2.
  4. Set the Temperature equation to Advective Diffusive.
  5. Change the Turbulence model to Spalart Allmaras.
  6. Set Nucleate boiling single phase to On.
  7. Set the Global Gravity to -9.81 in the Z direction.


    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 Relaxation factor to 0.4.
  3. Verify that Flow, Temperature, and Turbulence are set to On.

Set the Nodal Initial Conditions

  1. In the Solver Browser, click 03.NODAL_INITIAL_CONDITION under 01.Global.
  2. Set a constant X-Velocity value of 0.39.
  3. Set a constant Temperature value of 368.15.
  4. Set a constant Eddy viscosity value of 0.0001.


    Figure 3.

Assign Material Properties and Boundary Conditions

Create Curves/Plots for Material Properties

  1. In the Model Browser, right-click and select Create > Curve.
  2. In the Curve Editor, click New.
  3. In the panel area, enter Density_Water for the name then click proceed.
  4. Enter the X and Y values shown below.


    Figure 4.
  5. Create another curve, name it Viscosity_Water, and enter the values shown below.


    Figure 5.
  6. Create a curve named Enthalpy_Water and enter the following values


    Figure 6.
  7. Create a curve named Conductivity_Water and enter the following values.


    Figure 7.
  8. Create a curve named Density_Vapor and enter the following values.


    Figure 8.
  9. Create a curve named Viscosity_Vapor and enter the following values.


    Figure 9.
  10. Create a curve named Enthalpy_Vapor and enter the following values.


    Figure 10.
  11. Create a curve named Conductivity_Vapor and enter the following values.


    Figure 11.
  12. Close the Curve Editor.
  13. In the Model Browser, right-click and select Create > Plot.
  14. In the Entity Editor, set the name to Water-srfTns and set the type to Surface_Tension_Model.
  15. Set the value of the surface tension to 0.01.


    Figure 12.

Define Material Properties

  1. In the Solver Browser, right-click on the 02.Materials folder and select Material(Fluid) to create a new fluid material. Name it Vapor.
  2. In the Entity Editor, change the Density type to Cubic Spline, set the Curve fit variable to Temperature, and select the Density_Vapor curve from the list for Curve fit values.
  3. Change the Specific Heat type to Cubic Spline Enthalpy, set the Curve fit variable to Temperature, and select the Enthalpy_Vapor curve from the list for Curve fit values.
  4. Set the Latent heat type to Constant, the Latent heat to 2256000 J/kg, and the Latent heat temperature to 393.45 K.
  5. Similarly for Viscosity and Conductivity, set the cubic spline values to Viscosity_Vapor and Conductivity_Vapor, respectively.


    Figure 13.
  6. In the Solver Browser, right-click on FLUID and select Create to create a new fluid material. Name it Water.
  7. In the Entity Editor, change the Density type to Cubic Spline, set the Curve fit variable to Temperature, and select the Density_Water curve from the list for Curve fit values.
  8. Similarly for Specific Heat, Viscosity, and Conductivity, set the cubic spline values to Enthalpy_Water Viscosity_Water and Conductivity_Water, respectively.


    Figure 14.
  9. Under the vapor Phase heading, set the vapor phase model to Vapor by selecting it from the Material list.
  10. Under the Surface Tension heading, set the Surface tension model to Water-srfTns by selecting it from the Plot list.


    Figure 15.

Assign Material Properties and Boundary Conditions

  1. In the Solver Browser, expand 11.Volumes > FLUID.
  2. Click FluidVolume. In the Entity Editor,
    1. Verify that the Type is set to FLUID.
    2. Select Water as the Material.


    Figure 16.
  3. In the Solver Browser, expand 12.Surfaces > WALL.
  4. 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 0.39 m/sec.
    4. Set the Temperature to 368.15 K.


    Figure 17.
  5. Click Outflow. In the Entity Editor,
    1. Change the Type to OUTFLOW.
    2. Verify that the Pressure value is set to 0 N/m2.
    3. Turn on the Hydrostatic Pressure and set the coordinate to (0.12, 0.015, 0).
    4. Turn on the Backflow conditions and set the Temperature backflow type and Eddy viscosity backflow type to Mass Flux Average.


    Figure 18.
  6. Click HeatedWall. In the Entity Editor,
    1. Verify that the Type is set to WALL.
    2. Set the Temperature BC Type to Value.
    3. Set the Temperature to 403.15 K.


    Figure 19.
  7. Click Side_MaxY. In the Entity Editor, verify that the Type is set to WALL.
  8. Repeat the above step for the Side_Miny, Top, and Bottom components.

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. Leave the remaining options as default and click Launch to start the solution process.


    Figure 20.
    Once you hit the Launch button, the AcuTail and AcuProbe windows are launched automatically. A summary of the run in the AcuTail window indicates that the solver run is complete.


    Figure 21.

    Once the run is complete, you can close the AcuTail and AcuProbe windows.

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 temperature on the Heated Wall and Bottom surfaces.

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 22.
  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 NB1_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 Temperature Distribution

In this step, you will display temperature contours on the HeatedWall and the Bottom surfaces.
  1. In the Results Browser, expand the list of Components.
  2. 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 23.
  3. Click on the Results toolbar to open the Contour panel.
  4. In the panel area, change the Result type to Temperature (s).
  5. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
  6. Click Apply to plot the temperature contours.
  7. In the panel area, under the Display tab, turn off the Discrete color option.


    Figure 24.


    Figure 25.

Summary

In this tutorial, you learned how to set up a single phase nucleate boiling problem using HyperMesh and solve it using AcuSolve. Once you computed the solution, you post-processed the results using HyperView and created temperature contour plots.