Defining cavity radiation properties and view factors

You can model heat transfer due to radiation in enclosures by creating a cavity radiation interaction. Select InteractionCreate from the main menu bar, and select the surface. For a brief overview of cavity radiation, see Understanding interactions. For a more detailed discussion, see Cavity Radiation in Abaqus/Standard.

See Also
Interaction editors
Defining a cavity radiation interaction property
In Other Guides
Cavity Radiation in Abaqus/Standard
  1. From the main menu bar, select InteractionCreate.

    Tip: You can also create a cavity radiation interaction using the tool in the Interaction module toolbox.

  2. In the Create Interaction dialog box that appears, do the following:

    • Name the interaction. For more information about naming objects, see Using basic dialog box components.

    • Select the step. You can define cavity radiation only during a heat transfer or coupled thermal-electrical step.

    • Select the Cavity radiation type of interaction.

  3. Click Continue to close the Create Interaction dialog box.
  4. Use one of the methods below to select the cavity surface. Select only the portion of the surface to which one cavity radiation interaction property applies.

    • Use an existing surface to define the region. On the right side of the prompt area, click Surfaces. Select an existing surface from the Region Selection dialog box that appears, and click Continue.

      Note:

      The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Surfaces on the right side of the prompt area.

    • Use the mouse to select a region in the viewport. (For more information, see Selecting objects within the current viewport.)

      If the model contains a combination of mesh and geometry, click one of the following from the prompt area:

      • Click Geometry if you want to select the surface or vertex from a geometry region.

      • Click Mesh if you want to select the surface or node from a native or orphan mesh selection.

      You can use the angle method to select a group of faces or edges from geometry or a group of element faces from a mesh. For more information, see Using the angle and feature edge method to select multiple objects.

    Abaqus/CAE displays the Edit Interaction dialog box, and the surface name or (Picked) appears in the Surface column on the Properties tabbed page.

  5. To define additional cavity surfaces, click mouse button 3 in the table, select Add Row, and do one of the following:

    • Double-click an empty cell in the Surfaces column.

    • Click mouse button 3 in an empty table row, and select Edit Surface.

    Note:

    You can also use these techniques to replace an existing cavity surface; Abaqus/CAE does not indicate or retain your original selection when you edit an existing surface.

  6. Choose the cavity type in the Definition field.

    • Select Closed to specify a set of closed surfaces for radiation.

    • Select Open to include some radiation to the surroundings, and specify an Ambient temperature for the open cavity definition.

  7. Specify the Properties options.
    1. Select the Blocking surface checks. By default, Abaqus checks for blocking surfaces within the cavity when performing radiation view factor calculations.

      • Choose All to indicate that all blocking checks are active.

      • Choose None to skip blocking checks.

      • Choose Partial to specify potential blocking surfaces that Abaqus should check.

      For more information, see Controlling Checks for Surface Blocking.

    2. If you chose the Partial option, double-click an empty cell in the Blocking Surface table to select surfaces that you want Abaqus to check.

      Tip: You can also click mouse button 3 in the Blocking Surface table and choose Edit Surface, Add Row, or Delete Row to edit the table.

      The surface selection methods are the same as those described in Step 4.

    3. Select the heat reflection behavior.

      • Choose Yes for gray body radiation. Gray bodies have an emissivity between zero and one, as defined by a cavity radiation interaction property.

      • Choose No for black body radiation. Black bodies have a fixed emissivity of one—no heat is reflected.

    4. If you chose gray body radiation in the previous step, you must specify a cavity radiation interaction property for each row in the table. You can use any of the following methods:

      • Click a cell in the Property column to choose a predefined cavity radiation interaction property.

      • Click mouse button 3 in the table, and select Create Property to create a new interaction property or Edit Property to edit the existing cavity radiation interaction property in the selected row. (For more information, see Defining a cavity radiation interaction property.)

      • Enter a value in the Emissivity column. Abaqus/CAE automatically creates a cavity radiation interaction property with a default name and the specified emissivity.

    When you are finished, each row in the table contains a surface and an emissivity value or (table), indicating that there is a tabular emissivity defined in the interaction property. Property cells may be empty if you entered an emissivity value—Abaqus/CAE will add a default interaction property name when you close the Edit Interaction dialog box.

  8. Specify the View factors options.
    1. If desired, toggle on Specify blocking range and enter a value for the distance beyond which Abaqus should not calculate view factors due to blocking effects.
    2. Specify the Accuracy tolerance. The default value is 0.05.

      The view factor tolerance indicates the allowable deviation from the ideal sum of view factors. Abaqus ends the analysis if the tolerance is exceeded for a closed cavity. If the tolerance is exceeded for an open cavity, radiation to the ambient environment occurs.

    3. Specify the Infinitesimal facet area ratio. The default value is 64.

      This value represents the ratio of the largest facet area to the smallest facet area. Abaqus calculates this ratio for each facet pair.

    4. Specify the Gauss integration points per edge. The default value is 3.

      This value is used for the numerical integration method. Possible values range from 1 to 5.

    5. Specify the Lumped area distance-square value. The default value is 5.

      This value represents the ratio of the distance between the centroids of each facet pair, squared, to the area of the larger facet. If the calculated value is greater than this setting, Abaqus uses a lumped area approximation for the integration.

    6. If desired, click the Defaults button to reset all view factor entries to the Abaqus default values.

    If the calculated value for a pair of facets is less than or equal to the Lumped area distance-square value setting and the Infinitesimal facet area ratio is exceeded, Abaqus uses an infinitesimal-to-finite area approximation. If the Lumped area distance-square value is exceeded but the facet area ratio is not exceeded, Abaqus completes a numerical integration of the contour integral to get an accurate value.

    For more information, see Controlling the Accuracy of View Factor Calculations.

  9. Specify the Symmetry options. For detailed information on the available cavity radiation symmetry types, see Defining cavity radiation symmetry.”
  10. Specify the absolute zero temperature, θZ, on the temperature scale being used and the Stefan-Boltzmann constant, σ, in the Edit Model Attributes dialog box, as described in Specifying model attributes.
  11. Click OK to create the interaction and to close the editor.