Defining a concentrated radiative interaction

You can model heat transfer between one or more points in an assembly and a nonreflecting environment due to radiation by creating a concentrated radiation to ambient interaction. Select InteractionCreate from the main menu bar, and select one or more nodes or vertices or a saved set of nodes or vertices. For a brief overview of radiative interactions, see Understanding interactions. For a more detailed discussion, see Thermal Loads.

See Also
Interaction editors
Using analytical expression fields
Creating expression fields
In Other Guides
Thermal Loads
  1. From the main menu bar, select InteractionCreate.

    Tip: You can also create a concentrated radiative 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 radiation from a nodal area only during a heat transfer, coupled temperature-displacement, or coupled thermal-electrical step.

    • Select the Concentrated radiation to ambient type of interaction.

  3. Click Continue to close the Create Interaction dialog box.
  4. Use one of the following methods to select the points:

    • Use an existing set of nodes or vertices to define the region. On the right side of the prompt area, click Sets. Select an existing set 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 Sets on the right side of the prompt area.

    • Use the mouse to select nodes or vertices 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 vertices from a geometry region.

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

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

  5. In the Edit Interaction dialog box that appears, perform the following steps:
    1. If desired, specify how the concentrated radiation condition is applied to the boundary of an adaptive mesh domain. This option is valid only for Abaqus/Explicit analyses. Click the arrow to the right of the Adaptive mesh boundary type field, and select an option from the list that appears. For more information, see Defining ALE Adaptive Mesh Domains in Abaqus/Explicit.

      • Select Lagrangian to apply a concentrated radiation condition to a node that follows the material (nonadaptive).

      • Select Sliding to apply a concentrated radiation condition to a node that can slide over the material. Mesh constraints are typically applied to the node to fix it spatially.

      • Select Eulerian to apply a concentrated radiation condition to a node that can move independently of the material. This option is used only for boundary regions where the material can flow into or out of the adaptive mesh domain. Mesh constraints must be used normal to an Eulerian boundary region to allow material to flow through the region. If no mesh constraints are applied, an Eulerian boundary region will behave in the same way as a sliding boundary region.

    2. In the Associated nodal area field, enter the area associated with the node where the concentrated radiation condition is applied.
    3. Click the arrow to the right of the Emissivity distribution field, and select the option of your choice from the list that appears:

      • Select Uniform to define an emissivity that is uniform over the region.

      • Select an analytical field to define a spatially varying emissivity. Only analytical fields that are valid for this interaction type are displayed in the selection list. Alternatively, you can click to create a new analytical field. (See The Analytical Field toolset for more information.)

    4. In the Emissivity field, enter the emissivity of the surface, ϵ.
    5. In the Ambient temperature field, enter the ambient temperature, θ0.
    6. If you want to vary the ambient temperature with time, click the arrow to the right of the Ambient temperature amplitude field and select an amplitude from the list that appears. If desired, click to create a new amplitude; see Selecting an amplitude type to define, for more information.
  6. 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.
  7. Click OK to create the interaction and to close the editor.