A distributed load is a load that is applied over the length of a beam element. A distributed load can be applied in any direction specified by a vector.
In the case of a Linear analysis, for the distributed load to be applied to your model, you must assign a Pressure multiplier in the Multipliers tab of the Analysis Parameters dialog box. The product of the Magnitude and the Pressure multiplier updates the magnitude of the distributed load.
In the case of a Nonlinear analysis, a load curve controls the magnitude of the distributed load during the event duration. You specify the load curve number within the Creating Beam Distributed Load Object dialog box.
Apply Distributed Loads
If you select one or more beam elements using the Selection 
Select Lines command and right-click in the display area, you can select the Add pull-out menu and select the Beam Distributed Loads command to add a distributed load to each beam element.
If the magnitude and direction of the load is constant across the length of each selected beam, specify the magnitude of the load per unit of length in the Magnitude field and the direction of the load in the Direction section. If the magnitude or direction of the load varies across the length of each selected beam, deactivate the Uniform check box and specify the magnitude of the force per unit of length at each end in the I-Node Magnitude and J-Node Magnitude fields and the direction in the I-Node Direction and J-Node Direction sections. The magnitude of the load varies linearly between the nodes. This is done on a per-beam basis.
If you are applying a non-uniform load to the beam, you can have the load start and end at any point along the beam. This is done by specifying a ratio of the length of the beam in two ratio from I-Node fields. The first field determines how far from the I-Node the load starts. The second field determines how far from the I-Node the load ends. For example, if you want a load to be applied only along the third-quarter of a beam, you specify 0.5 in the first field and 0.75 in the second field.
Visibility Object Visibility Element Axis 1 command. This axis lies along the direction of the beam element line and the positive direction is from the I‑Node to the J‑Node. If axis 1 needs to be reversed for some elements, this can be done by selecting the elements (Selection Select Lines), right-clicking, and choosing Beam Orientations Invert I and J Nodes. For Nonlinear Analyses Only
Specify the load curve that will be used to multiply the distributed load in the Load Case / Load Curve field. Press the Curve button to define a load curve in the Load Curve Editor, or use the Analysis: Parameters dialog. Specify an additional multiplier applied to this load in the Multiplier field.
For the load to maintain the same orientation with respect to the element as it deforms, activate the Follows Displacement check box (and the Large Displacement analysis type in the Element Definition). When using Follows Displacement, the following additional calculations are performed:
- The user's load is converted from global X, Y, Z directions into the beam element's local 1, 2, 3 directions at the start of the analysis.
- Throughout the analysis, the loads remain in the local 1, 2, 3 directions. So, as the beam moves and rotates, the local axes also change orientation in space. Consequently, the direction of the loads in global X, Y, Z are changing.
- The magnitude of the load remains constant. But if the length of the element changes, the total load changes. If the element gets twice as long, the load will be twice as much (constant magnitude x updated length).