# ACU-T: 3204 Radiation Heat Transfer in a Simple Headlamp using the Discrete Ordinate Model

## Prerequisites

This tutorial introduces you to setting up a radiation heat transfer problem using the Discrete Ordinate radiation model in HyperWorks CFD. Prior to starting this tutorial, you should have already run through the introductory tutorial, ACU-T: 1000 Basic Flow Set Up, 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.

## Problem Description

The problem to be solved is shown schematically in Figure 1 and Figure 2. It consists of a simple headlamp with a housing, lens, and a bulb. The inner cavity of the bulb is filled with air and the wattage of the bulb is 1W, which is modeled as a volumetric heat source. The Boussinesq density model is used for the air to consider the natural convection effects in the fluid volume. The heat generated in the bulb is transferred by three means: conduction from the bulb to the housing, natural convection in the air volume, and radiation from the bulb to the air and lens volume. The outer surfaces of the headlamp are assumed to be at a constant temperature of 300 K.
The air and the lens are modeled as participating media for radiation heat transfer. For the purpose of this tutorial, the absorption coefficient of air is considered to be zero. The following radiation material properties are used for the air and the lens volumes.
Table 1.
Absorption Coefficient Refractive Index
Air 0 1.0
Lens 900 1.57
For simulations involving participating media, the following radiation surface types must be defined at the boundaries of each participating medium.
Table 2.
Participating medium - Participating medium Interface Radiation Interface - Internal
Participating medium - (Non- Participating) medium Interface Wall
External boundaries of Participating medium Radiation Interface - External or Wall
The discrete ordinate radiation model implementation in AcuSolve allows for modeling specular, diffuse, and partially specular interfaces. This can be done by specifying the appropriate value of diffused fraction while defining the radiation surfaces. For the diffused fraction, a value of 1 means the surface is purely diffuse, a value of 0 means it is purely specular. Any value between 0 and 1 means the surface is partially specular. In this tutorial, since both the air and lens are modeled as participating media, the lens-air interface and the lens-outer surfaces will be modeled as internal and external radiation interface respectively. The internal interface will be defined as a specular interface whereas the external interface will be defined as a diffuse interface.

## Start HyperWorks CFD and Create the HyperMesh Model Database

1. Start HyperWorks CFD from the Windows Start menu by clicking Start > Altair <version> > HyperWorks CFD.
When HyperWorks CFD is loaded, the Geometry ribbon is open by default.
2. Create a new .hm database in one of the following ways:
• From the menu bar, click File > Save.
• From the Home tools, Files tool group, click the Save As tool.
3. In the Save File As dialog, navigate to the directory where you would like to save the database.
4. Enter Headlamp_DO as the name for the database then click Save.
This will be your problem directory and all the files related to the simulation will be stored in this location.

## Import and Validate the Geometry

### Import the Geometry

1. From the menu bar, click File > Import > Geometry Model.
2. In the Import File dialog, browse to your working directory then select ACU-T3204_headlamp.x_t and click Open.
3. In the Geometry Import Options dialog, leave all the default options unchanged then click Import.

### Validate the Geometry

1. From the Geometry ribbon, click the Validate tool.
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.
The surface and solid errors display in the list below the tool.
2. Click SolidChecks.
The Solid Repair tool opens, which you can use to fix the geometric errors in the model.
From the SolidChecks legend, you can see the model's solids have five intersections.
3. Click Intersections.
A guide bar used to fix intersecting solids displays.
4. Optional: Click and to review each error.
5. Activate the Keep common interface option then click Combine All.
The SolidChecks legend should now display zero for all errors.
6. Click the Validate tool once again.
Observe that a blue check mark now appears on the top-left corner of the tool icon. This indicates that no issues are detected and you are ready to continue.

## Set Up Flow

### Set the General Simulation Parameters

1. From the Flow ribbon, click the Physics tool.
The Setup dialog opens.
2. Under the Physics models setting:
1. Verify that Time marching is set to Steady.
2. Select Laminar as the Turbulence model.
3. Activate the Include gravitational acceleration checkbox and set the gravity in the y direction to -9.81.
4. Activate the Heat transfer checkbox.
3. Click the Solver controls setting and activate the Thermal flow equation.
4. Close the dialog and save the model.

### Define the Material Models

1. From the Flow ribbon, click the Material Library tool.
The Material Library dialog opens.
2. Click the My Materials tab.
3. Click to add a new fluid material model.
4. In the material creation dialog, click the name in the top-left corner and rename the material to Air_Boussinesq.
5. In the Density tab,
1. Set the Type to Boussinesq.
2. Set the Density value to 1.225.
3. Set the Expansivity value to 0.00347222.
4. Reference temperature value to 288.
6. Click the Specific Heat tab and set the Specific heat value to 1005.
7. Click the Viscosity tab and set the Viscosity value to 1.781e-05.
8. Click the Conductivity tab and set the Conductivity value to 0.02521.
9. Close the material creation dialog to return to the Material Library dialog.
10. Select Solid in the Settings menu, click the My Materials tab, then click to create a new solid material model.
11. Name the material Plastic and set the following values.
The Type should be Constant for each property.
• Density: 1270
• Specific Heat: 1900
• Conductivity: 0.2
12. Close the material creation dialog to return to the Material Library dialog.
13. Similarly, create new solid material models named Arnite and LED with the following properties.
The Type should be Constant for each property.
Arnite:
• Density: 1670
• Specific Heat: 2050
• Conductivity: 1.6
LED:
• Density: 5500
• Specific Heat: 0.3
• Conductivity: 5.0
14. Close all dialogs and save the model.

### Assign Material Properties

1. From the Flow ribbon, click the Material tool.
2. Click the lens volume highlighted in the figure below and select Arnite from the Material drop-down menu.
3. On the guide bar, click to execute the command and remain in the tool.
4. Click the housing volume and assign the Plastic material model.
5. On the guide bar, click to execute the command and remain in the tool.
6. In the Materials legend, right-click on Air and select Isolate.
7. Click the air volume and assign the Air_Boussinesq material model.
8. On the guide bar, click to execute the command and remain in the tool.
9. In the Materials legend, right-click on Air and select Isolate.
10. Click the bulb volume and assign the LED material model.
11. On the guide bar, click to execute the command and exit the tool.
12. Save the model.

### Define the Heat Source

1. From the Flow ribbon, click the Sources > Heat tool.
2. In the modeling window, select the bulb volume.
3. In the Heat Source dialog, set the heat source value to 2049180 W/m3.
4. On the guide bar, click to execute the command and exit the tool.
5. Press Esc to exit the Sources tool then press the A key to turn on the display of all solids.
6. Save the model.

### Define Flow Boundary Conditions

In this problem, all the surfaces are walls and will therefore be assigned the default wall boundary condition. The outer walls of the headlamp will be given a no-slip wall boundary condition with a constant temperature.

1. From the Flow ribbon, click the No Slip tool.
2. In the modeling window, select the surfaces highlighted in the figure below.
3. In the microdialog, enter the values shown in the figure below.
4. In the Boundaries legend, double-click Wall, rename it to Outerwalls, then press Enter.
5. On the guide bar, click to execute the command and exit the tool.
6. Save the model.

In this step, you will specify the parameters related to the thermal radiation setup.

1. From the Radiation ribbon, Thermal Radiation tools, click the Physics tool.
2. Activate Thermal radiation and set the Radiation model to Discrete Ordinate.
4. Close the dialog.

### Define the Emissivity Models

1. From the Radiation ribbon, click the Surface Finish Library tool.
The Surface finish library opens.
Click to add a new emissivity model.
2. Set the Name of the model to Inner and the Emissivity value to 0.05 by double-clicking on the entity fields.
3. Close the dialog.

### Define the Participating Media Radiation Models

1. From the Radiation ribbon, Participating Media tools, click the Model tool.
The Participating media model library opens.
2. Click to add a new model.
3. Name the new model Air and assign the following property values:
• Absorption coefficient - 0
• Scattering coefficient - 0
• Phase coefficient - 0
• Refractive index - 1
4. Similarly, create another model named Lens and assign the following property values:
• Absorption coefficient - 900
• Scattering coefficient - 0
• Phase coefficient - 0
• Refractive index - 1.57
5. Close the dialog.

### Assign Participating Media Models

1. From the Radiation ribbon, click the Assign tool.
2. Click the lens volume and assign the Lens model from the microdialog drop-down.
3. On the guide bar, click to execute the command and remain in the tool.
4. In the Participating Media legend, right-click on Lens and select Hide.
5. Select the air volume and assign the Air model.
6. On the guide bar, click to execute the command and remain in the tool.
7. In the Participating Media legend, right-click on Air and select Hide.
8. Save the model.

### Assign Surface Finish Models

1. From the Radiation ribbon, click the Surface Finish tool.
2. Select only the inner surfaces of the housing - i.e. the housing-air interface.

A total of nine surfaces should be selected.

3. Assign the Inner model from the microdialog drop-down
4. On the guide bar, click to execute the command and exit the tool.
5. Turn on the display of all surfaces in the model by pressing the A key.

Since the lens and air are defined as semi-transparent media, the interface between the two will be modeled as a specular interface of type: internal. Accordingly, the outer surfaces of the lens will be modeled as external interface radiation surface.

1. From the Radiation ribbon, click the Interface tool.
Notice that all the surfaces except the Lens-Air interface surface are made transparent. Since the Air and Lens volumes are defined as participating media, HyperWorks CFD automatically detects the surfaces that can be defined as an internal radiation interface and only those surfaces will be available for selection when this tool is active.
2. Using the box selection method, draw a window around the model.
Observe that the lens-air interface is the only surface that is selected.
3. In the microdialog, set the Radiation diffused fraction to 0.
4. On the guide bar, click to execute the command and exit the tool.
5. Click the External Boundary tool.
6. Select the three outer surfaces of the lens volume.
7. In the microdialog, set the Radiation diffused fraction to 1, the External refractive index to 1, and the External temperature to 300 K.
8. On the guide bar, click to execute the command and exit the tool.
9. Save the model.

## Generate the Mesh

In this step, you will define the mesh controls and then generate the mesh.

### Define the Surface Mesh Controls

1. From the Mesh ribbon, click the Surface tool.
2. Using the box selection method, select all the surfaces in the model.
3. In the microdialog, set the Average element size to 0.002.
4. On the guide bar, click to execute the command and remain in the tool.
5. Select the surface highlighted in the figure below and hide it by pressing the H key or by right-clicking and select Hide from the context menu.
6. Select the three surfaces highlighted in the figure below.
7. In the microdialog, set the Average element size to 0.001 and the Mesh growth rate to 1.
8. On the guide bar, click to execute the command and exit the tool.

### Define the Boundary Layer Controls

1. From the Mesh ribbon, click the Boundary Layer tool.
2. Right-click in the modeling window and go to Select > Advanced Select > By Material > Air_Boussinesq.
All the fluid wall surfaces should be selected and a microdialog for BL specification appears.
3. Enter the following values in the microdialog:
• First layer thickness definition: Constant
• First layer thickness: 0.0005
• Total number of layers: 4
• Growth method: Constant
• Initial growth rate: 1.3
• Termination policy: Truncate
• Activate the Enable surface mesh modification option
4. On the guide bar, click to execute the command and exit the tool.
5. Turn on the display of all the surfaces.

### Define the Volume Mesh Controls

Since the thickness of the housing and the lens solids are small, you will use the thin layer meshing tool so that when the volume mesh is generated, there will be two layers across the thickness of those solids.

1. From the Mesh ribbon, click the Volume Mesh tool.
2. Select the housing and the lens solids.
3. In the microdialog,
1. Set the Average size to 0.001.
2. Set the Growth rate to 1.0.
3. Activate the Thin layer meshing option and set the Number of layers to 2.
4. On the guide bar, click to execute the command and exit the tool.

### Generate the Mesh

1. From the Mesh ribbon, click the Volume tool.
The Meshing Operations dialog opens.
2. Set the Mesh growth rate to 1.
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.
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 the Default initial conditions menu and deactivate the Pre-compute flow option.
5. Set the x-velocity to 0 and the Temperature to 300.
6. Leave the remaining options as default and 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.
4. Click the Slice Planes tool.
5. Select the plane perpendicular to the x-axis, as shown in the figure below.
6. Click the Front face on the View Cube to align the model.
7. Click in the slice plane microdialog.
8. In the display properties microdialog, set the display to temperature.
9. Activate the Legend toggle and click to reset the range.
10. Click , set the Legend location to Upper Right Corner, and the Colormap Name to Rainbow Uniform.
11. Click on the guide bar.
12. In the Post Browser, hide the Boundary Collections.
13. Right-click on Slice Plane 1 in the browser and select Edit.
14. Change the display to incident radiation.
15. Click to refresh the legend's range.
16. Click on the guide bar.

## Summary

In this tutorial, you learned how to set up and solve a radiation heat transfer problem in a headlamp using the discrete ordinate radiation model in HyperWorks CFD. You started by importing and cleaning up the geometry and then set up the flow, thermal, and radiation boundary conditions. Once the solution was computed, you processed the results using the Post ribbon where you created contour plots of temperature and incident radiation.