The general goal of an
Abaqus
simulation is to predict the response of a structure to 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
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.