## Prerequisites

This tutorial introduces you to the workflow for setting up a thermal radiation problem in a headlamp using the enclosure radiation model in 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, AcuSolve, and HyperView. 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-T3200_headlamp.x_t from HyperWorksCFD_tutorial_inputs.zip.

## 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 surface to other surfaces. The external reference temperature is 300 K for the outer surfaces of the headlamp. You will use the Enclosure radiation model to simulate the surface to surface radiation.
The enclosure radiation methodology in AcuSolve involves a two-step process: view factor computation and heat flux addition. View factor is the proportion of radiation incident one surface due to another surface. The view factors are computed, and the radiative heat fluxes are added to the energy equation during the solver run. These radiative heat fluxes are computed based on the view factors using the Stefan-Boltzmann law. The enclosure radiation model is supported only on fluid mediums.

## 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_Enclosure 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-T3200_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 convective heat flux boundary condition.

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.
3. Close the dialog.

### Define the Emissivity Models

1. From the Radiation ribbon, click the Surface Finish Library tool.
The Surface finish library opens.
2. Click to add a new emissivity model.
3. Set the Name of the model to Walls and the Emissivity value to 0.7 by double-clicking on the entity fields.
4. Close the dialog.

### Assign Surface Finish Models

1. From the Radiation ribbon, click the Surface Finish tool.
2. Using the window selection method, select all the surfaces in the model.
3. In the microdialog, assign the Walls emissivity model.
4. On the guide bar, click to execute the command and exit the tool.
5. 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 window 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 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.

### 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 Batch 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 HyperView

Once the solver run is complete, you will use HyperView to process the results.

### Open HyperView and Load the Model and Results

1. Start HyperView from the Windows Start menu by clicking Start > All Programs > Altair <version> > HyperView.
Once the HyperView window is loaded, the Load model and results panel should be open by default. If you do not see the panel, click File > Open > Model.
2. In the Load model and results panel, click next to Load model.
3. 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 Headlamp_Enclosure.1.Log.
4. Click Open.
5. Click Apply in the panel area to load the model and results.

### Create a Contour Plot of Temperature

1. In the Results Browser, expand the list of Components.
2. Click the Isolate Shown icon then select the AUTO Lamp5-2 SolidBody_3_3 wall component to turn of the display of all the components except the walls of the air volume.
3. Orient the display to the xy-plane by clicking on the Standard Views toolbar.
4. Click on the Results toolbar to open the Contour panel.
5. In the panel area, set the Result type to Temperature (s).
6. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
7. Click Apply.
8. In the panel area, under the Display tab, turn off the Discrete color option.
9. Click the Legend tab then click Edit Legend. In the dialog, change the Numeric format to Fixed then click OK.
10. Click the Mask icon on the HV-Display toolbar.
11. Select an element on the lens outer surface.
12. In the panel area, click the Elements entity selector. In the Extended Entity Selection dialog, select By Face then close the dialog.
13. In the panel area, click Mask Selected to turn off the display of the lens-outer surface.
The contour plot should look like the one shown in the figure below.

### Display Temperature Contours and Velocity Vectors on a Section Cut

In this step, you will create a section cut on the mid-z plane and then display the temperature and velocity vectors on that cross section.

1. In the Results Browser, turn on the display of all the components.
2. Click the Section cut icon icon on the HV-Display toolbar.
3. In the panel area, click Add to create a new section cut named Section 1.
4. In the Define plane section, set the axis to Z Axis then click Apply.
5. Set the Z base coordinate to 0.0005 then press Enter.
6. Change the Display options from Clipping plane to Cross section.
7. Click Gridline. In the Gridline Options dialog, deactivate the Show check box under Grid line then click OK.
8. Click the Vector icon on the Results toolbar to open the Vector panel.
9. In the panel area, set the Result type to Velocity (v).
10. Click the Selection drop-down and select Sections from the list of options.
11. Click the Sections entity selector then select All.
12. In the panel area, activate the Overlay result display check box (if not set already).
13. Click Apply.
14. Under the Plot tab, verify that only the X+Y+Z Resultant option is selected.
15. Go to the Display tab, set the Size scaling option to Uniform, and enter a value of 0.0015 in the size field.
16. Set the Color by option to Direction and set the X+Y+Z color to White.
17. Go to the Section tab, activate the Projected check box, then click Apply.
18. Click on the Results toolbar to open the Contour panel.
19. In the panel area, set the Result type to Temperature (s).
20. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
21. In the panel area, under the Result tab, activate the Overlay result display check box (if not set already).
22. Click Apply to create the contour plot of temperature on the section cut along with velocity vectors.
Zoom in to the contour plot to observe the natural convection phenomenon inside the headlamp.

## Summary

In this tutorial, you learned how to set up and solve a radiation heat transfer problem in a headlamp using the enclosure radiation model in AcuSolve using HyperWorks CFD. You started by importing the headlamp geometry file, then you set up the simulation parameters and boundary conditions. Once the solution was computed, you processed the results using HyperView, where you created contour plots of temperature and velocity vectors in the fluid domain.