ACU-T: 3202 Heat Transfer Between Concentric Spheres – P1 Radiation Model

Prerequisites

This tutorial provides the instructions for setting up, solving, and viewing results for a steady state simulation of radiation heat transfer between concentric spheres using the P-1 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 understanding of HyperWorks CFD and AcuSolve. To run this simulation, you will need access to a licensed version of HyperWorks CFD and AcuSolve.

Prior to running through this tutorial, click here to download the tutorial models. Extract ACU-T3202_P1Rad.hm from HyperWorksCFD_tutorial_inputs.zip.

Problem Description

The problem to be addressed in this tutorial is shown schematically in Figure 1. In this problem, a P1 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.



Figure 1.

Start HyperWorks CFD and Open the HyperMesh Database

  1. Start HyperWorks CFD from the Windows Start menu by clicking Start > Altair <version> > HyperWorks CFD.
  2. From the Home tools, Files tool group, click the Open Model tool.


    Figure 2.
    The Open File dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file ACU-T3202_P1Rad.hm and click Open.
  4. Click File > Save As.
  5. Create a new directory named P1_radiation 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 P1_radiation as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Validate the Geometry

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.

To focus on the physics part of the simulation, this tutorial input file contains geometry which has already been validated. Observe that a blue check mark appears on the top-left corner of the Validate icon on the Geometry ribbon. This indicates that the geometry is valid, and you can go to the flow set up.


Figure 3.

Set Up Flow

Set Up the Simulation Parameters and Solver Settings

  1. From the Flow ribbon, click the Physics tool.


    Figure 4.
    The Setup dialog opens.
  2. Under the Physics models setting:
    1. Set Time marching to Steady.
    2. Set the Turbulence model to Laminar.
    3. Activate the Heat transfer checkbox.


    Figure 5.
  3. Click the Solver controls setting.
  4. Deactivate the Flow checkbox.
    In this tutorial, you will only be solving for the temperature field.


    Figure 6.
  5. Close the dialog and save the model.

Create Material Models

  1. From the Flow ribbon, click the Material Library tool.


    Figure 7.
    The Material Library dialog opens.
  2. Under Settings, click Fluid then click the My Materials tab.
  3. Click to create a new material.
  4. In the new dialog, rename the material to Radiating by clicking the name in the top-left corner.
  5. Enter the following values for each of the material property tabs then close the dialog.
    • Density – 1000 kg/m3
    • Specific Heat – 10000 J/kg-K
    • Viscosity – 1e-5 kg/m-sec
    • Conductivity – 1e-6 W/m-K





    Figure 8.
  6. Click the Solid setting.
  7. Repeat the above steps to create two material models (Inner and Outer) using the following parameters:
    Inner
    • Density – 1000 kg/m3
    • Specific Heat – 10000 J/kg-K
    • Conductivity – 2 W/m-K
    Outer
    • Density – 1000 kg/m3
    • Specific Heat – 10000 J/kg-K
    • Conductivity – 0.35 W/m-K

Assign Material Properties

  1. From the Flow ribbon, click the Material tool.


    Figure 9.
  2. Select the outer solid and assign the Outer material model from the microdialog.


    Figure 10.
  3. On the guide bar, click to execute the command and remain in the tool.
  4. In the Materials legend, right-click on Air and select Isolate.
  5. Select the outer solid and assign the Radiating material model to it.
  6. On the guide bar, click .
  7. In the Materials legend, right-click on Air again and select Isolate.
  8. Select the remaining solid and assign the Inner material model to it.
  9. On the guide bar, click to execute the command and exit the tool.
  10. Save the model.

Assign the Flow Boundary Conditions

  1. From the Flow ribbon, click the No Slip tool.


    Figure 11.
  2. Select the two faces of the sphere then right-click and select Hide.
  3. Select the two faces remaining in the modeling window. In the microdialog, assign a Temperature boundary condition at 300 K.


    Figure 12.
  4. In the Boundaries legend, double-click on Wall and rename it to Inner.
  5. On the guide bar, click to execute the command and remain in the tool.
  6. Press the A key to turn on the display of all surfaces.
  7. Select the two outer faces. In the microdialog, assign a Temperature boundary condition at 1300 K.
  8. In the Boundaries legend, double-click on Wall and rename it to Outer.
  9. On the guide bar, click to execute the command and exit the tool.
  10. Save the model.

Set Up Radiation

Select the Radiation Model

  1. From the Radiation ribbon, Thermal Radiation tools, click the Physics tool.


    Figure 13.
    The Radiation Settings dialog opens.
  2. Activate the Thermal radiation checkbox and set the Radiation model to P1 Model.


    Figure 14.

Define the Radiation Material Properties

  1. Click the Surface Finish Library tool.


    Figure 15.
    The Surface finish library opens.
  2. Click .
  3. In the table, double-click on Surface Finish, rename it to Inner, and the Emissivity to 0.5.
  4. Similarly, create another Emissivity model named Outer with an Emissivity of 0.8.


    Figure 16.
  5. From the Participating Media tools, click the Model tool.


    Figure 17.
    The Participating media model library opens.
  6. Click and create a model with the following properties.


    Figure 18.

Assign the Participating Media Model

  1. From the Participating Media tools, click the Assign tool.


    Figure 19.
  2. In the modeling window, right-click and select Select > Advanced > By Material > Radiating
  3. In the microdialog, verify that the Air model is selected.
  4. Click on the guide bar.
  5. In the Participating Media legend, right-click on Air and select Isolate.

Assign the Emissivity Model

  1. From the Thermal Radiation tools, click the Surface Finish tool.


    Figure 20.
  2. Select the two outer surfaces.
  3. In the microdialog, select the Outer surface finish model.
  4. Click on the guide bar.
  5. In the Participating Media legend, right-click on Black Body and select Isolate.
  6. Select the two visible surfaces and assign the Inner surface finish model.
  7. Click on the guide bar.
  8. Save the model.

Generate the Mesh

The meshing parameters for this tutorial are already set in the input file.
  1. From the Mesh ribbon, click the Volume tool.


    Figure 21.
    The Meshing Operations dialog opens.
    Note: If the model has not been validated, you are prompted to create the simulation model before running the batch mesh.
  2. Check that the Average element size is 0.0025 and the Mesh growth rate is 1.0.
  3. Accept all other default parameters.


    Figure 22.
  4. 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.

Run AcuSolve

  1. From the Solution ribbon, click the Run tool.


    Figure 23.
  2. Set the Parallel processing option to Intel MPI.
  3. Optional: Set the number of processors to 4 or 8 based on availability.
  4. Leave the remaining options as default and click Run to launch AcuSolve.


    Figure 24.
  5. In the Run Status dialog, right-click on the AcuSolve run and select Plot time history.
  6. In the Plot Utility dialog, double-click on Residual Ratio to plot the residuals.


    Figure 25.

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. In the browser, click the icon beside Flow Boundaries to turn off the display of all the surfaces.


    Figure 26.
  5. Click the Slice Planes tool.


    Figure 27.
  6. Select the x-y plane in the modeling window.
  7. In the slice plane microdialog, click to create the slice plane.
  8. In the display properties microdialog, set the display to Temperature and activate the Legend toggle.
  9. Click and set the Colormap Name to Rainbow Uniform.


    Figure 28.
  10. Click on the guide bar then press F to fit the section cut to the screen.


    Figure 29.

Summary

In this tutorial, you learned how to set up and solve a radiation heat transfer simulation using the P1 radiation model. You started by importing the HyperWorks CFD input database and defining the flow and radiation setup. Then, you generated the mesh and submitted the AcuSolve simulation. Once the solution was computed, you created a plot of residual ratios using the plot utility in HyperWorks CFD. Finally, you created a contour plot of temperature distribution on a section cut using HyperWorks CFD Post.