Defining a concentrated film condition interaction

You can model heat transfer from one or more points in an assembly due to convection by creating a concentrated film condition 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 film conditions, see Understanding interactions. For a more detailed discussion, see Thermal loads.

Related Topics
Interaction editors
Using analytical expression fields
Creating expression fields
In Other Guides
Defining ALE adaptive mesh domains in Abaqus/Explicit
Thermal loads

  1. From the main menu bar, select InteractionCreate.

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

    • Select the Concentrated film condition 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, click the arrow to the right of the Definition field and select an option from the list that appears:

    • Select Embedded Coefficient to specify the film coefficient in this dialog box.

    • Select Property Reference to define the film coefficient as a function of temperature and field variables using a film condition interaction property.

    • Select User-defined to define nonuniform film coefficients in user subroutine FILM. (This option is valid only in Abaqus/Standard analyses). See the following sections for more information:

    • Select an analytical field to define a spatially varying film coefficient. The analytical field does not affect the sink temperature. 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.)

  6. If desired, specify how the concentrated film 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 film to a node that follows the material (nonadaptive).

    • Select Sliding to apply a concentrated film 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 film 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.

  7. In the Associated nodal area field, enter the area associated with the node where the concentrated film condition is applied.

  8. If you selected the Embedded Coefficient or analytical field definition option, perform the following steps:

    1. In the Film coefficient field, enter the film coefficient, h.
    2. If you want to vary the film coefficient with time, click the arrow to the right of the Film coefficient 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.
    3. In the Sink temperature field, enter the sink temperature, θ0.
    4. If you want to define a spatially varying sink temperature, click the arrow to the right of the Sink definition field and select an analytical field, labeled with an (A), or a discrete field, labeled with a (D). Only analytical fields and discrete fields that are valid for temperature are available in the selection list. See The Analytical Field toolset,” and The Discrete Field toolset,” for more information.

      Alternatively, you can click to create a new discrete field.

    5. If you want to vary the sink temperature with time, click the arrow to the right of the Sink 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.

  9. If you selected the Property Reference definition option, perform the following steps:

    1. Select a film interaction property. If desired, click to create the interaction property; see Defining a film condition interaction property, for more information.
    2. In the Sink temperature field, enter the sink temperature, θ0.
    3. If you want to define a spatially varying sink temperature, click the arrow to the right of the Sink definition field and select an analytical field, labeled with an (A), or a discrete field, labeled with a (D). Only analytical fields and discrete fields that are valid for temperature are available in the selection list. See The Analytical Field toolset,” and The Discrete Field toolset,” for more information.

      Alternatively, you can click to create a new discrete field.

    4. If you want to vary the sink temperature with time, click the arrow to the right of the Sink 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.

  10. If you selected the User-defined definition option, perform the following steps:

    1. In the Film coefficient field, enter the film coefficient, h.
    2. In the Sink temperature field, enter the sink temperature, θ0.
    3. Enter the Job module, and display the job editor for the analysis job of interest. (For more information, see Creating, editing, and manipulating jobs.)
    4. In the job editor, click the General tab, and specify the file containing the user subroutine FILM. For more information, see Specifying general job settings.

      Note:

      You can specify only one user subroutine file in the job editor; if your analysis involves more than one user subroutine, you must combine the user subroutines into one file and then specify that file.

  11. Click OK to create the interaction and to close the editor.