To create or edit a body force:

Display the body force load editor using one of the following methods:

To create a new body force load, follow the procedure outlined in “Creating loads,” Section 16.8.1 (Category: Mechanical; Types for Selected Step: Body force).

To edit an existing body force load using menus or managers, see “Editing step-dependent objects,” Section 3.4.12. To edit the region to which the load is applied, see “Editing the region to which a prescribed condition is applied,” Section 16.8.4.

Click the arrow to the right of the Distribution field, and select the option of your choice from the list that appears:

Select Uniform to define a load that is uniform over the body.

Select User-defined to define the magnitude of the load in user subroutine DLOAD (for ABAQUS/Standard) or VDLOAD (for ABAQUS/Explicit). See the following sections for more information:

• “Specifying general job settings,” Section 18.6.6

• “DLOAD,” Section 1.1.5 of the ABAQUS User Subroutines Reference Manual

• “VDLOAD,” Section 1.2.1 of the ABAQUS User Subroutines Reference Manual

If you selected the Uniform distribution option, perform the following steps:

In the Component 1, Component 2, and (if you are working in three-dimensional space) Component 3 fields, enter the body force per unit volume in each direction (units FL^–3):

If you are working in three-dimensional or two-dimensional space, the Component 1, Component 2, and Component 3 fields correspond to the 1-, 2-, and (if applicable) 3-directions.

If you are working in axisymmetric space, Component 1 corresponds to the radial direction and Component 2 corresponds to the axial direction.

If desired, click the arrow to the right of the Amplitude field, and select the amplitude of your choice from the list that appears. Alternatively, you can click Create to create a new amplitude. (See Chapter 38, “The Amplitude toolset,” for more information.)

Click OK to save your data and to exit the editor.

If you selected the User-defined distribution option, perform the following steps:

If desired, in the Component 1, Component 2, and (if applicable) Component 3 fields enter the body force per unit volume in each direction (units FL^–3).

Load magnitude data that you enter in the editor are passed into the user subroutine in an ABAQUS/Standard analysis but are ignored in an ABAQUS/Explicit analysis.

Click OK to save your data and to exit the editor.

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 18.5.)

In the job editor, click the General tab, and specify the file containing the user subroutine that defines the load magnitude. For more information, see “Specifying general job settings,” Section 18.6.6.

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.