Abaqus is designed as a flexible tool for finite element modeling. An important aspect of this flexibility is the manner in which Abaqus allows the user to step through the history to be analyzed. This is accomplished by defining analysis procedures. A basic concept in Abaqus is the division of the problem history into steps. A step is any convenient phase of the history—a thermal transient, a creep hold, a dynamic transient, etc. In its simplest form in Abaqus/Standard, a “step” is just a static analysis of a load change from one magnitude to another. In each “step” the user chooses a procedure, thus defining the type of analysis to be performed during the step: dynamic stress analysis, eigenvalue buckling, transient heat transfer analysis, etc. The procedure choice can be changed from step to step in any meaningful way. Since the state of the model (stresses, strains, temperatures, etc.) is updated throughout all analysis steps, the effects of previous history are always included in the response in each new step. Thus, for example, if natural frequency extraction is performed after a geometrically nonlinear static analysis step, the preload stiffness will be included. Abaqus/Standard provides both linear and nonlinear response options. The program is truly integrated, so linear analysis is always considered as linear perturbation analysis about the state at the time when the linear analysis procedure is introduced. This linear perturbation approach allows general application of linear analysis techniques in cases where the linear response depends on preloading or the nonlinear response history of the model. In nonlinear problems the objective is to obtain a convergent solution at a minimum cost. The nonlinear procedures in Abaqus/Standard offer two approaches to this. Direct user control of increment size is one choice, whereby the user specifies the incrementation scheme. Automatic control is the alternate approach: the user defines the step and specifies certain tolerances or error measures. Abaqus/Standard then automatically selects the increments as it develops the response in the step. This approach is usually more efficient, because the user cannot predict the response ahead of time. Automatic control is particularly valuable in cases where the time or load increment varies widely through the step, as is often the case in diffusion type problems (such as creep, heat transfer, and consolidation). In Abaqus/Explicit the time incrementation is controlled by the stability limit of the central difference operator. The time incrementation scheme is, hence, fully automatic and requires no user intervention. User-specified time incrementation is not available because it would always be nonoptimal. Abaqus/Standard and Abaqus/Explicit are separate program modules with different data structures; hence, the explicit dynamics procedure cannot be used in the same analysis as any of the procedures in Abaqus/Standard. However, Abaqus provides a capability to import a deformed mesh and associated material state from Abaqus/Explicit into Abaqus/Standard and vice versa. This procedure is described in Transferring results between Abaqus/Explicit and Abaqus/Standard. |