# ACU-T: 3203 Heat Transfer Between Concentric Spheres – Discrete Ordinate Radiation Model

## Prerequisites

This tutorial provides instructions for setting, solving and viewing results for a steady state simulation of radiation heat transfer between concentric spheres using the Discrete Ordinates Radiation model. 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 knowledge 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-T3203_DiscreteOrdinate.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. In this problem, a DO radiation model is used to simulate the heat transfer due to radiation between concentric spheres. The inside surface of the inner and the outside surface of the outer sphere are both held at constant temperature while the gap between them radiates the heat from one sphere to the other.

The problem consists of a fluid region with arbitrary material properties between two concentric spheres with surfaces held at fixed temperature, as shown in the following figure, which is not drawn to scale. The radius of the outer sphere is 0.04 m and the radius of the inner sphere is 0.01 m. The inner surface of the inner sphere is defined to have a constant wall temperature at 300.0 K (26.85 ºC). The outer surface of the outer sphere is defined to have a constant wall temperature at 1300.0 K (1026.85 ºC). The fluid within the spheres is defined as a non-conducting material, allowing heat to transfer via radiation only.

The problem is solved as a steady state case to allow the heat transfer in the solid and fluid regions to reach an equilibrium.

## Open the HyperMesh Model Database

1. Start HyperMesh 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-T3203_DiscreteOrdinate.hm and click Open.
4. Click File > Save As.
The Save Model As dialog opens.
5. Create a new directory named DO-Radiation_Sphere 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 DO-Radiation_Sphere as the file name for the database, or choose any name of your preference.
7. Click Save to create the database.

## Set the General Simulation Parameters

1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
2. In the Entity Editor, set the Temperature equation to Advective Diffusive.
3. Set the Radiation equation to Discrete Ordinate.
5. In the Solver Browser, click 02.SOLVER_SETTINGS under 01.Global.
6. In the Entity Editor, set the Convergence tolerance to 0.001.
7. Verify that the Relaxation Factor is set to 0.3.
8. Turn off Flow and verify that the Temperature and Radiation fields are turned On.

## Set Up Radiation Parameters and Boundary Conditions

In this step, you will define the radiation parameters i.e. emissivity models, surface boundary conditions for the problem, and assign material properties to the fluid and solid regions.

### Set Up Material Model Parameters

1. In the Solver Browser, right-click on 02.Materials and select Material(Fluid).
3. In the Entity Editor, set the Density to 1000 kg/m3.
4. Set the Specific heat to 10000 J/kg-K.
5. Set the Conductivity to 1e-6 W/m-K.
This is done to prioritize heat transfer only through radiation.
7. Set the Absorption coefficient to 0.001.
8. In the Solver Browser, right-click on 02.Materials and select Material(Solid).
9. Name the material Inner.
10. In the Entity Editor, set the Density to 1000 kg/m3.
11. Set the Specific heat to 10000 J/kg-K.
12. Set the Conductivity to 2 W/m-K.
13. In the Solver Browser, right-click on Inner and select Duplicate. Rename it Outer.
14. In the Entity Editor, change the Conductivity to 0.35 W/m-K.
15. Verify that the Allow Participating Media Radiation is turned off for both Inner and Outer.
This is done because only the fluid medium participates in heat transfer through radiation.

### Set Up Emissivity Model Parameters

1. In the Solver Browser, right-click on 07.Emissivity_Model collector and select Create.
2. Name the emissivity model Inner.
3. In the Entity Editor, set the Emissivity to 0.5.
4. Repeat the above steps and create another emissivity model named Outer with an Emissivity of 0.8.

### Set Up 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 Radiating. In the Entity Editor, change the Type to FLUID and set Radiating as the Material.
3. Click Inner. In the Entity Editor, change the Type to SOLID and set Inner as the Material.
4. Click Outer. In the Entity Editor, change the Type to SOLID and set Outer as the Material.
5. Click Inner_Inner_ri. In the Entity Editor,
1. Verify that the Type is set to WALL.
2. Change the Temperature BC type to Value.
3. Set the Temperature to 300 K.
6. Click Outer_Outer_ro. In the Entity Editor,
1. Verify that the Type is set to WALL.
2. Change the Temperature BC type to Value.
3. Set the Temperature to 1300 K.
7. Click Inner_Radiating_r1. In the Entity Editor,
1. Verify that the Type is set to WALL.
2. Change the Temperature BC type to Flux.
3. Under the Radiation Surface tab, activate the Display check box and turn On the Activate radiation surface field.
4. Verify that the Type is set to WALL and select Inner as the Emissivity model.
8. Click Outer_Radiating_r2. In the Entity Editor,
1. Verify that the Type is set to WALL.
2. Change the Temperature BC type to Flux.
3. Under the Radiation Surface tab, activate the Display check box and turn On the Activate radiation surface field.
4. Verify that the Type is set to WALL and select Outer as the Emissivity model.
9. Save the model.

## Compute the Solution

In this step, you will launch AcuSolve directly from HyperMesh and compute the solution.

### Run AcuSolve

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. The Output time steps can be set to All or Final. Since this is a steady state analysis, the Final time step output is sufficient.
5. Leave the remaining options as default and click Launch to start the solution process.

## Post-Process the Results with HyperView

Once the solution has converged, close the AcuProbe and AcuTail windows. Go to the HyperMesh window and close the AcuSolve Control tab.

### Open HyperView and Load the Model and Results

1. In the HyperMesh main menu area, click Applications > 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 DO-Radiation_Sphere.1.Log.
4. Click Open.
5. Click Apply in the panel area to load the model and results.

### Create Temperature Contours

In this step, you will create a contour plot of temperature distribution across the domain.

1. Click on the Results toolbar to open the Contour panel.
2. Under Result type, select Temperature(s).
The drop-down below should be automatically set to Scalar value.
3. Click Apply.
4. In the panel area, under the Display tab, turn off the Discrete color option.
5. Click the Legend tab then click Edit Legend. In the dialog, change the Numeric format to Fixed then click OK.
6. Right-click on empty space in the Results Browser and select Create > Section Cut > Planar to create a planar section cut.
A new entity named Section 1 is created under the Section Cuts tree.
7. Click beside Section 1 to turn off the grid display in the graphics window.
8. Orient the display to the xz-plane by clicking on the Standard Views toolbar.
9. Verify that the contour plot looks like the figure below.

## Summary

In this tutorial, you worked through a workflow to set-up a DO-Radiation model, carry out a radiation heat transfer simulation, and post-process the results using HyperWorks products, namely AcuSolve, HyperMesh, and HyperView. You started by importing the model in Altair HyperMesh. Then you defined the simulation parameters and launched AcuSolve directly from within HyperMesh. Upon completion of the solution by AcuSolve, you used HyperView to post-process the results and create contour plots.