Defining a line load

Display the line load editor using one of the following methods:

• To create a new line load, follow the procedure outlined in Creating loads (Category: Mechanical; Types for Selected Step: Line load).

• To edit an existing line load using menus or managers, see Editing step-dependent objects. To edit the region to which the load is applied, see Editing the region to which a prescribed condition is applied.

Click the arrow to the right of the System field, and from the list that appears select the coordinate system in which you want to define the load:

• Select Global if you want to specify the load components in the global 1-, 2-, and (if you are working in three-dimensional space) 3-directions.

• Select Local if you want to specify the load components in the beam local 1-direction (if you are working in three-dimensional space) and the beam local 2-direction. (For more information, see Assigning a beam orientation.)

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 region.

• 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

  • DLOAD

  • VDLOAD

• Select an analytical field to define a spatially varying load. Only analytical fields that are valid for this load 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.)

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

1. In the Component fields, enter the body force per unit length in each direction (units FL⁻¹):

   • If you selected the Global system, the Component 1, Component 2, and Component 3 fields correspond to the 1-, 2-, and 3-directions.

   • If you selected the Local system, the Component 1 field corresponds to the beam local 1-direction, and the Component 2 field corresponds to the beam local 2-direction.

2. 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 to create a new amplitude. (See The Amplitude toolset for more information.)
3. Click OK to save your data and to exit the editor.

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

1. If desired, in the Component fields enter the force per unit length in each direction (units FL⁻¹).

   Entering load magnitude data in the editor is optional for user-defined loads. Any data you enter are passed to the user subroutine in an Abaqus/Standard analysis but are ignored in an Abaqus/Explicit analysis.

2. Click OK to save your data and to exit the editor.
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 that defines the load magnitude. 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.