You can model heat transfer from surfaces due to convection by creating a surface film condition interaction. Select Interaction
Create from the main menu bar and select the surface. For a brief overview of film conditions, see “Understanding interactions,” Section 15.3. For a more detailed discussion, see “Thermal loads,” Section 34.4.4 of the Abaqus Analysis User's Guide.
To define a surface film condition interaction:
From the main menu bar, select InteractionCreate.
Tip:
You can also create a surface film condition interaction using the 
tool in the Interaction module toolbox.
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,” Section 3.2.1.
Select the step. You can define convection from a surface only during a heat transfer, coupled temperature-displacement, or coupled thermal-electrical step.
Select the Surface film condition type of interaction.
Click Continue to close the Create Interaction dialog box.
Use one of the following methods to select the surface:
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,” Section 6.2.)
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.
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 Chapter 58, “The Analytical Field toolset,” for more information.)
If you selected the Embedded Coefficient or analytical field definition option, perform the following steps:
In the Film coefficient field, enter the film coefficient, h.
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,” Section 57.3, for more information.
In the Sink temperature field, enter the sink temperature, 
.
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 Chapter 58, “The Analytical Field toolset,” and Chapter 63, “The Discrete Field toolset,” for more information.
Alternatively, you can click 
to create a new discrete field.
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,” Section 57.3, for more information.
If you selected the Property Reference definition option, perform the following steps:
Select a film interaction property. If desired, click 
to create the interaction property; see “Defining a film condition interaction property,” Section 15.14.2, for more information.
In the Sink temperature field, enter the sink temperature, .
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 Chapter 58, “The Analytical Field toolset,” and Chapter 63, “The Discrete Field toolset,” for more information.
Alternatively, you can click to create a new discrete field.
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,” Section 57.3, for more information.
If you selected the User-defined definition option, perform the following steps:
In the Film coefficient field, enter the film coefficient, h.
In the Sink temperature field, enter the sink temperature, .
Enter the Job module, and display the job editor for the analysis job of interest. (For more information, see “Creating, editing, and manipulating jobs,” Section 19.7.)
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,” Section 19.8.6.
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.
Click OK to create the interaction and to close the editor.
