The general goal of an ABAQUS simulation is to determine the response of the model to the applied loads. Recall that in a general sense the term load in ABAQUS refers to anything that induces a change in the response of a structure from its initial state; for example, nonzero boundary conditions or applied displacements, point forces, pressures, fields, etc. In some cases loads are relatively simple, such as a single set of point loads on a structure. In other problems the loads applied to a structure can be very complex. For example, different loads may be applied to different portions of the model in a particular sequence over some period of time, or the magnitude of the loads may vary as a function of time. The term load history is used to refer to such complex loading of a model.

In ABAQUS the user divides the complete load history of the simulation into a number of steps. Each step is a period of “time,” specified by the user, for which ABAQUS calculates the response of the model to a particular set of loads and boundary conditions. The user must specify the type of response, known as the analysis procedure, during each step and may change analysis procedures from step to step. For example, static dead loads, perhaps gravitational loads, could be applied to a structure in one step; and the dynamic response of the loaded structure to earthquake accelerations could be calculated in the next step. Both implicit and explicit analyses can contain multiple steps; however, implicit and explicit steps cannot be combined in the same analysis job. To combine a series of implicit and explicit steps, the results transfer (or import) capability can be used. This feature is discussed in “Transferring results between ABAQUS/Explicit and ABAQUS/Standard,” Section 7.7.2 of the ABAQUS Analysis User's Manual, and is not discussed further here.

ABAQUS divides all of its analysis procedures into two main groups: linear perturbation and general. General analysis steps can be included in an ABAQUS/Standard or an ABAQUS/Explicit analysis; linear perturbation steps are available only in ABAQUS/Standard. Loading conditions and “time” are defined differently for the two cases. Furthermore, the results from each type of procedure should be interpreted differently.

The response of the model during a general analysis procedure, known as a general step, may be either nonlinear or linear. In a step that uses a perturbation procedure, which is called a perturbation step, the response can only be linear. ABAQUS/Standard treats such steps as a linear perturbation about the preloaded, predeformed state (known as the base state) created by any previous general steps; therefore, its capability for doing linear simulations is rather more general than that of a purely linear analysis program.