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

## Prerequisites

This tutorial introduces you to setting up a CFD simulation involving solar radiation and thermal shells using AcuSolve and 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.

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 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 HyperMesh.

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.

## 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-T3201_SolarRadiation.hm and click Open.
4. Click File > Save As.
The Save Model As dialog opens.
5. Create a new directory named Atrium_Solar 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 Atrium_Solar as the file name for the database, or choose any name of your preference.
7. Click Save to create the database.

## Set Up 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, change the Analysis type to Transient.
3. Set the Temperature equation to Advective Diffusive.
4. Set the Turbulence model to Laminar (if not set already).

### Specify the Solver Settings

1. In the Solver Browser, click 02.SOLVER_SETTINGS under 01.Global.
2. In the Entity Editor, set the Max time steps to 0.
3. Set the Final time to 30 sec.
4. Set the Initial time increment to 1 sec.
5. Set the Max stagger iterations to 3.
6. Change the Relaxation factor to 0.
7. Verify that the Flow and Temperature fields are turned On.

### Set the Solar Radiation Parameters

1. In the Solver Browser, click 05.SOLAR_RADIATION_PARAMETERS under 01.Global.
2. In the Entity Editor, change the Curve fit options to Dat file.
3. Click on the open file icon beside the Dat file field, browse to the location where you saved SolarLoad.dat, and open it.
4. Leave the remaining options as default.
5. Save the model.

## Assign Material Properties and Boundary Conditions

### Create the Solar Radiation Model

1. In the Solver Browser, right click on 08.Solar_Radiation_Model and select Create.
2. In the Entity Editor, name it Glass.
3. Set the Specular Transmissivity to 0.8.
4. Set the Diffusive Transmissivity to 0.08.
5. Set the Specular reflectivity to 0.01.
6. Set the Diffusive reflectivity to 0.01.

### Assign Material Properties and Boundary Conditions

By default, all components are assigned to the wall boundary condition. In this step, you will change them to the appropriate boundary conditions and assign material properties to the fluid volumes.
1. In the Solver Browser, expand 12.Surfaces > WALL.
2. Click Fluid. In the Entity Editor,
1. Change the Type to FLUID.
2. Set the Material to Air_HM.
3. Click Walls. In the Entity Editor,
1. Verify that the Type is set to WALL and the Temperature BC type is set to Flux.
2. Set the Convective heat flux coefficient to 20.0 J/m2-sec-K.
3. Set the Convective heat flux reference temperature to 283.15 K.
4. Under the Solar Radiation Surface tab, turn on the Display field. Turn On the Activate solar radiation surface option. Set the Type to Outward. Set the Solar radiation model to Solar Radiation Black Body.
5. Under the Surface Output tab, turn On Surface Output and set the Nodal time step frequency to 1.
4. Click Inlet. In the Entity Editor,
1. Change the Type to INFLOW.
2. Set the Inflow velocity type to Cartesian.
3. Set the X, Y and Z-velocity to 0, 22.78 and -39.45 m/sec respectively.
4. Set the Temperature of the incoming fluid to 295.35 K.
5. Under the Solar Radiation Surface tab, turn on the Display field. Turn On the Activate solar radiation surface option. Set the Type to Outward. Set the Solar radiation model to Solar Radiation Black Body.
5. Click Outlet. In the Entity Editor, change the Type to OUTFLOW.
6. Click Glass. In the Entity Editor,
1. Verify that the Type is set to WALL and the Temperature BC type is set to Flux.
2. Set the Convective heat flux coefficient to 20.0 J/m2-sec-K.
3. Set the Convective heat flux reference temperature to 283.15 K.
4. Under the Solar Radiation Surface tab, turn on the Display field. Turn On the Activate solar radiation surface option. Set the Type to Both. Set the Solar radiation model to Glass.
5. Under the Surface Output tab, turn On Surface Output and set the Nodal time step frequency to 1.
7. Click Floor. In the Entity Editor,
1. Verify that the Type is set to WALL and the Temperature BC type is set to Flux.
2. Under the Solar Radiation Surface tab, turn on the Display field. Turn On the Activate solar radiation surface option. Set the Type to Inward. Set the Solar radiation model to Solar Radiation Black Body.
3. Under the Surface Output tab, turn On Surface Output and set the Nodal time step frequency to 1.
8. Click Glass_walls. In the Entity Editor,
1. Change the Type to THERMAL_SHELL.
2. Set the Number of shell layers to 1.
3. Set the Shell thickness to 0.025 m.
4. Set the Shell Material to Aluminum_HM.
5. For the Primary Wall boundary condition, leave the default values unchanged.
6. Change the Select Wall Boundary Condition value from Primary Wall to Shell Outer Wall.
7. Set the Convective heat flux coefficient to 20 J/m2-sec-K and the Convective heat flux reference temperature to 283.15 K.
8. Under the Solar Radiation Surface tab, turn on the Display field. Turn On the Activate solar radiation surface option. Set the Type to Outward. Set the Solar radiation model to Solar Radiation Black Body.
9. Expand the Surface Output tab, turn On Surface Output, and set the Nodal time step frequency to 1.
9. Click Chair. In the Entity Editor,
1. Verify that the Type is set to WALL.
2. Under the Solar Radiation Surface tab, turn on the Display field. Turn On the Activate solar radiation surface option. Set the Type to Default. Set the Solar radiation model to Solar Radiation Black Body.
3. Under the Surface Output tab, turn On Surface Output and set the Nodal time step frequency to 1.
10. Save the model.

### Set Nodal Initial Conditions

1. In the Solver Browser, click 03.NODAL_INITIAL_CONDITION under 01.Global.
2. In the Entity Editor, change the Default value of Temperature to 288.15 K.

### Define Nodal Output Frequency

1. In the Solver Browser, expand 17.Output then click NODAL_OUTPUT.
2. In the Entity Editor, set the Time step frequency to 1.
3. Activate the Output initial condition checkbox.
4. Save the model.

## 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.

## Post-Process the Results using HyperView

In this step, you will create an animation of solar heat flux and temperature over run time. Once the solver run is complete, close the AcuProbe and AcuTail windows. In the HyperMesh Desktop window, close the AcuSolve Control tab and save the model.

### 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.
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 Atrium_Solar.1.Log.
6. Click Open.
7. In the panel area, click Reader Options.
8. In the Reader Options dialog, set the Reader to AcuSolve Result Reader and the Extended nodal output option to Yes then click OK.
9. 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, glass_walls and the man surface.

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.S16’ 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, Glass_walls Shell Outer, and Chair surfaces.
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 and thermal shells. You started by importing a HyperMesh model database and set 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 and build plots using derived results.