# ACU-T: 3201 Solar Radiation and Thermal Shell Tutorial

This tutorial introduces you to setting up a CFD simulation involving solar radiation and thermal shells using AcuSolve and 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, 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-T3201_Atrium.x_t and SolarLoad.dat from HyperWorksCFD_tutorial_inputs.zip.

## Problem Description

The problem to be addressed is shown schematically in Figure 1. The model consists of an atrium with a couch and chairs in the center. Air flows into the atrium through the inlet vent and exits through the outlet. The front portion of the atrium consists of glass walls supported by an aluminum frame. This aluminum frame will be modeled as a thermal shell; hence, this tutorial introduces you to the process of setting up a transient solar radiation simulation and thermal shells in HyperWorks CFD.

AcuSolve uses an ideal gray surface solar radiation model to calculate the solar heat flux. The fluxes are computed using a ray trace algorithm and five optical properties of the surface, specular transmissivity (${\tau }_{s}$), diffuse transmissivity (${\tau }_{d}$), specular reflectivity (${\rho }_{s}$), diffuse reflectivity (${\rho }_{d}$) and absorptivity ($\alpha$).
A specular transmission occurs when a photon passes straight through a surface with no change of direction. In a diffuse transmission the photon penetrates the surface, but its outgoing energy is uniformly distributed in solid angle over the hemisphere, weighted by projected surface area. For a specular reflection, the angle of reflection is equal to the angle of incidence. Diffuse reflections are similar to diffuse transmissions, except the hemisphere over which the outgoing energy is distributed is on the same side of the surface as the incident photon. Finally, the photon may be absorbed by the surface. These five interactions are associated with five surface properties that together must obey the following constraint:(1) ${\tau }_{s}\left(\theta \right)+{\tau }_{d}\left(\theta \right)+{\rho }_{s}\left(\theta \right)+{\rho }_{d}\left(\theta \right)+\alpha \left(\theta \right)=1$
Where,
${\tau }_{s}$
Specular transmissivity
${\tau }_{d}$
Diffuse transmissivity
${\rho }_{s}$
Specular reflectivity
${\rho }_{d}$
Diffuse reflectivity
$\alpha$
Absorptivity
$\theta$
Angle of incidence

For the solar radiative heat fluxes to be computed, a solar radiation surface needs to be defined on that given surface.

In this tutorial, the solar flux loading is given in the form of a data file which was generated using the acuSflux script available in AcuSolve. The script can be used to generate a data file with a four-column array of solar flux vector data values. The piecewise linear type is used in this tutorial to emulate the pattern of sunrise to sunset over the atrium.

For example, to generate the solar load data file for a location with known geological coordinates, enter the following command in the AcuSolve Command Prompt: acuSflux -time "dec-3-2019 11:00:00" -tinc 1800 -nts 25 -lat 42.6064 -lon -83.1498 -ndir "1,0,0" -udir "0,0,1"

Here,
time
The start time in GMT (ex: “dec-3-2019 21:00:00”)
tinc
The time increment in seconds
nts
Number of discrete time steps
lat
Latitude coordinates of the location in degrees North (ex: 45.112 or -37.56 (equal to 37.56 S))
lon
Longitude coordinates of the location in degrees East (ex: 86.26 or -54.84 (equal to 54.84 W))
ndir
The north direction unit vector in model coordinates (should be enclosed in double quotes) (ex: “0,1,0”)
udir
The upward direction unit vector in model coordinates (should be enclosed in double quotes) (ex: “0,1,0”)

## Thermal Shell Modeling

The thermal shell in AcuSolve is a feature that creates zero physical thickness volumetric shell elements from surface elements. This is useful when the thickness of the component is too small to be modeled as a solid medium. The thermal shell can have multiple layers, each with different thicknesses and material models. A schematic of the thermal shell is shown below.

When defining a thermal shell on a surface, two sets of boundary conditions are needed. One for the Primary Wall surface i.e. Shell Inner and one for the Shell Outer Wall surface. In this tutorial, a solar radiation surface will be defined on the outer shell surface so that it receives solar heat flux, whereas the inner shell surface will be modeled as a default wall.

## 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 Atrium_Solar 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-T3201_Atrium.x_t and click Open.
3. In the Geometry Import Options dialog, leave all the default options unchanged then click Import.

The model contains an atrium with glass panes supported by an aluminum frame in the front. Air enters from the opening on the roof in the front and exits through the outlet in the rear.

### 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 current model doesn’t have any of the issues mentioned above. Alternatively, if any issues are found, they are indicated by the number in the brackets adjacent to the tool name.

Observe that a blue check mark appears on the top-left corner of the Validate icon. This indicates that the tool found no issues with the geometry model.
2. Press Esc or right-click in the modeling window and swipe the cursor over the green check mark from right to left.
3. Save the database.

## Set Up Flow

### Set Up the Simulation Parameters and Solver Settings

1. From the Flow ribbon, click the Physics tool.
The Setup dialog opens.
2. Under the Physics models setting:
1. Set Time marching to Transient.
2. Set the Time step size to 1 and the Final time to 30.
3. Set the Turbulence model to Laminar.
4. Activate the Heat transfer checkbox.
3. Click the Solver controls setting and set the Maximum stagger iterations to 3.
4. Close the dialog and save the model.

### Assign Material Properties

1. From the Flow ribbon, click the Material tool.
2. Verify that Air is assigned as the material for the fluid domain.
The legend in the top-left corner of the modeling window lists all the material models assigned to the current model.
Since this model has a single volume, by default air is assigned as the material for the fluid domain.
3. On the guide bar, click to execute the command and exit the tool.

### Define Thin Solids

In this simulation, you will model the aluminum frames as a thin solid.

1. From the Flow ribbon, click the Thin tool.
2. In the modeling window, select the four surfaces highlighted in the image below.
3. In the microdialog, set the Layer thickness to 0.025 and the Material to Aluminum.
4. On the guide bar, verify that the number of Parent Surfaces selected is 4 then click to execute the command.
Once the command is executed, the legend should be updated accordingly to reflect the changes.
5. Save the model.

### Define Flow Boundary Conditions

1. From the Flow ribbon, click the Constant tool.
2. In the modeling window, click the inlet surface highlighted in the figure below.
3. In the microdialog, enter the values shown below.
4. Click the Temperature icon and enter a value of 295.35 K.
5. Click on the guide bar to execute the changes.
6. Click the Outlet tool.
7. Select the surface highlighted in the figure below then click on the guide bar.
8. Click the No Slip tool.
9. Select all three wall surfaces of the atrium, the roof, and the front glass walls.

In total, 21 surfaces should be selected.

10. In the microdialog, enter the values shown in the figure below.
11. Click . In the new microdialog that appears, set the Nodal Output frequency to 1.
12. On the guide bar, click to execute the command and remain in the tool.
13. On the guide bar, click the drop-down menu next to Surfaces and change the selection entity to Thin Solids.
The visibility of all the surfaces except the thin solids is made transparent.
14. Select all the thin solid surfaces using the window selection method.
15. In the microdialog, enter the values shown in the figure below.
16. Click . In the new microdialog that appears, set the Nodal Output frequency to 1.
17. On the guide bar, verify that the number of Thin Solids selected is 4 and the Direction is set to Away from Parent Surface, then click .
18. Change the selection entity on the guide bar back to Surfaces.
19. From the Boundaries legend, right-click on Default Wall and select Isolate.
20. Select all the surfaces except the aluminum frame, as highlighted in the figure below.
21. In the microdialog, enter the values shown in the figure below.
22. Click . In the new microdialog that appears, set the Nodal Output frequency to 1.
23. From the Boundaries legend, rename Wall 1 to Floor by double-clicking on it.
24. Click on the guide bar.
The updated Boundaries legend should look similar to the one shown below.
25. Turn on the visibility of all the surfaces by right-clicking in the modeling window and selecting Show All or by simply pressing the A key.
26. Save the model.

### Set Up the Solar Radiation Parameters

1. From the Radiation ribbon, Solar Radiation tools, click the Physics tool.
2. In the Solar Radiation Settings dialog, activate the Solar radiation equation.
3. Click to load the solar flux input from a file.
4. In the Open file dialog, set the filter to Dat file (.dat) and select the SolarLoad.dat file provided with the input file for this tutorial.
5. Click Open.
The plot in the dialog should look like the one shown in the figure below.
6. Close the dialog and save the model.

### Define the Solar Radiation Models

1. From the Radiation ribbon, Solar Radiation tools, click the Model tool.
3. In the Name column, enter BB out and set the Side to Outward.
4. Similarly, create the other models and enter the values as shown in the figure below.
5. Close the dialog and save the model.

### Assign the Solar Radiation Models

1. From the Radiation ribbon, click the Surface tool.
2. Select the three wall surfaces, the inlet, and the roof surface, as highlighted in the figures below.
3. In the microdialog, set the Solar radiation model to BB out then click on the guide bar.
4. Select all the glass surfaces shown in the figure below, assign the Glass model to them, then click on the guide bar.
5. Rotate the model and select the floor surface. In the microdialog, assign the BB in model then click on the guide bar.
6. From the Solar Radiation Model legend, right-click on Unassigned and select Isolate.
7. Select the surfaces of the couch, table, and chairs, assign the BB def model to them, then click on the guide bar.
8. On the guide bar, change the selection entity to Thin Solids.
9. Using the window selection method, select the four thin solid surfaces and assign the BB out model to them.
10. On the guide bar, verify that the Direction is set to Away from Parent Surface then click to execute the changes.
11. Turn on the display of all the surfaces and 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 0.15 and the Mesh growth rate to 1.0.
4. On the guide bar, click to execute the command and exit the tool.
5. Save the model.

### Generate the Mesh

1. From the Mesh ribbon, click the Batch tool.
2. In the Meshing Operations dialog, set the Mesh growth rate to 1.1 then click Mesh to start the meshing process.
The Run Status dialog opens and the status of the meshing process is shown.
3. Once the mesh is generated, close the Run Status dialog and save the model.
Note: Considering the run time of the simulation, a very coarse mesh with no boundary layers is used for this tutorial. Otherwise, a relatively fine mesh with boundary layers to adequately resolve the gradients in the flow and temperature fields should be used.

## Compute the Solution

### Define the Nodal Output Frequency

1. From the Solution ribbon, click the Field tool.
2. In the Field Output dialog, activate the check box for Write initial conditions.
3. Set the Time step interval to 1.

### Define the Nodal Initial Conditions and Compute the Solution

1. From the Solution ribbon, click the Run tool.
2. In the Launch AcuSolve dialog, set the Parallel processing option to Intel MPI.
3. Optional: Set the number of processors to 4 or 8 based on availability.
4. Deactivate the Automatically define pressure reference option.
5. Expand the Default initial conditions menu.
6. Deactivate the Pre-compute flow option.
7. Set the Temperature to 288.15.
8. Verify that all the values are set as shown in the figure below.
9. Click Run.
Once the solution process is started, the Run Status dialog appears.
10. In the dialog, right-click on the AcuSolve run and select View log file.
Once the run is complete, a summary of the solution process is shown in the log file.

## Post-Process the Results with HyperView

In this step, you will create an animation of solar heat flux and temperature over run time.

### 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 Atrium_Solar.1.Log.
4. Click Open.
5. In the panel area, click Reader Options.
6. In the Reader Options dialog, set the Reader to AcuSolve Result Reader and the Extended nodal output option to Yes then click OK.
7. Click Apply in the panel area to load the model and results.

### Create an Animation of Temperature Contour

In this step, you will start by creating an expression for plotting the temperature values in Fahrenheit units. Then, you will create an animation of the magnitude of temperature on the floor and the thin solid wall surfaces.

1. From the menu bar, go to Results > Create > Derived Results.
2. In the Expression Builder dialog, enter Temperature_fahrenheit as the Label (name) of the expression.
3. In the Expression text box, enter the following expression: 1.8*(
4. Set the Table option to Temperature and the Resource to model. Then, click Insert to add the temperature variable in the expression.
5. Complete the expression by entering the remaining portion of the formula as shown in the figure below.
Here the term ‘R1.S10’ corresponds to the Temperature (scalar) variable in Kelvin. Variables can be inserted in the expression by selecting the required variable under Table option and then clicking Insert. The actual ID for the scalar variable might be different for your simulation.
6. Click OK to apply the changes and close the dialog.
7. In the Results Browser, expand the list of Components. Turn off the display of all the components except Floor - Output and Thin Solid Wall - Dynamic.
8. In the graphics window, rotate the model so that you have a better view of the glass walls and the chair.
9. Click on the Results toolbar to open the Contour panel.
10. In the panel area, set the Result type to Temperature_fahrenheit (s).
11. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
12. Click Apply.
13. In the panel area, under the Display tab, turn off the Discrete color option.
14. Go to the Legend tab then click Edit Legend.
15. In the Edit Legend dialog, change the Type to Dynamic scale and the Numeric format to Fixed then click OK.
16. Click on the Animation toolbar to play the temperature animation.
17. Click the Animation Controls icon . In the panel area, set the Max Frame Rate to 5 Frames/Sec by dragging the slider.

### Create an Animation of Solar Heat Flux

1. Click on the Results toolbar to open the Contour panel.
2. In the panel area, set the Result type to Solar_heat_flux (s).
3. Click Apply.
4. On the ImageCapture toolbar, click on the Capture Graphics Area Video icon .
5. In the Save Graphics Area Video As dialog, browse to the directory where you want to save the animation and give a name to the video, ex: solar heat flux animation, then click Save.

## Summary

In this tutorial, you learned how to set up and solve a CFD analysis involving solar radiation. You started by importing a geometry model into HyperWorks CFD and setting up the simulation parameters and boundary conditions. Once you computed the solution, you post-processed the results using HyperView. Also, you learned how to create expressions in HyperView so that you can build plots of derived results.