A load case is a set of loads and boundary conditions used to define a particular loading condition. You can use one or more load cases in a static perturbation or steady-state dynamic, direct step to study the linear responses of a structure subjected to different loading conditions. A load case analysis is generally much more efficient than the equivalent multiple step analysis since it takes advantage of the principal of linear superposition.

You can define load cases directly in terms of loads and boundary conditions or in terms of combinations of previously defined load cases. You use the Load module to define load cases directly in terms of loads and boundary conditions. You use the Visualization module to define load case combinations of previously defined load cases during postprocessing. Load case output is stored in separate frames in the output database (.odb), and you can create results for load case combinations by combining the results from multiple frames.

You use the Load Case menu in the Load module to create load cases that include previously defined loads and boundary conditions. You can use a nonzero scale factor to scale the magnitude of individual loads and boundary conditions within a load case. You may include a load or boundary condition only once within each load case. If a step contains load cases, you must include each load and boundary condition in the step in one or more load cases. By default, ABAQUS/CAE includes all boundary conditions propagated or modified from the base state in each load case you create but allows you to modify this behavior for individual load cases. You can use the boundary condition manager to deactivate unused propagated boundary conditions in a step containing load cases.

In steps containing load cases ABAQUS supports only field output requests. The field output requests created in the Step module apply to all load cases in the step. You can use the Visualization module to view and manipulate load case results (see “Viewing load case output,” Section 21.7.4).

For more information on load cases, see “Multiple load case analysis,” Section 6.1.3 of the ABAQUS Analysis User's Manual. For more information on creating loads and boundary conditions in the Load module, see “Creating and modifying prescribed conditions,” Section 16.4.