We now discuss how to account for nonlinearity in an ABAQUS analysis. The main focus is on geometric nonlinearity.
Incorporating the effects of geometric nonlinearity in an analysis requires only minor changes to an ABAQUS/Standard model. You need to make sure the step definition considers geometrically nonlinear effects. This is the default setting in ABAQUS/Explicit. In ABAQUS/Standard you can also specify the maximum number of increments allowed during the step. ABAQUS/Standard terminates the analysis with an error message if it needs more increments than this limit to complete the step. The default number of increments for a step is 100; if significant nonlinearity is present in the simulation, the analysis may require many more increments. You specify an upper limit on the number of increments that ABAQUS/Standard can use, rather than the number of increments it must use.
In a nonlinear analysis a step takes place over a finite period of “time,” although this “time” has no physical meaning unless inertial effects or rate-dependent behavior are important. In ABAQUS/Standard you specify the initial time increment, 
, and the total step time, 
. The ratio of the initial time increment to the step time specifies the proportion of load applied in the first increment. The initial load increment is given by:
Although you must specify the initial increment size in ABAQUS/Standard, ABAQUS/Standard automatically controls the size of the subsequent increments. This automatic control of the increment size is suitable for the majority of nonlinear simulations performed with ABAQUS/Standard, although further controls on the increment size are available. ABAQUS/Standard will terminate an analysis if excessive cutbacks caused by convergence problems reduce the increment size below the minimum value. The default minimum allowable time increment, 
, is 10–5 times the total step time. By default, ABAQUS/Standard has no upper limit on the increment size, 
, other than the total step time. Depending on your ABAQUS/Standard simulation, you may want to specify different minimum and/or maximum allowable increment sizes. For example, if you know that your simulation may have trouble obtaining a solution if too large a load increment is applied, perhaps because the model may undergo plastic deformation, you may want to decrease .
Local directions
In a geometrically nonlinear analysis the local material directions may rotate with the deformation in each element. For shell, beam, and truss elements the local material directions always rotate with the deformation. For solid elements the local material directions rotate with the deformation only if the elements refer to nondefault local material directions; otherwise, the default local material directions remain constant throughout the analysis.
Local directions defined at nodes remain fixed throughout the analysis; they do not rotate with the deformation. See “Transformed coordinate systems,” Section 2.1.5 of the ABAQUS Analysis User's Manual, for further details.
Effect on subsequent steps
Once you include geometric nonlinearity in a step, it is considered in all subsequent steps. If nonlinear geometric effects are not requested in a subsequent step, ABAQUS will issue a warning stating that they are being included in the step anyway.
Other geometrically nonlinear effects
The large deformations in a model are not the only important nonlinear geometric effects that are considered when geometric nonlinearity is considered. ABAQUS/Standard also includes terms in the element stiffness calculations that are caused by the applied loads, the so-called load stiffness. These terms improve convergence behavior. In addition, the membrane loads in shells and the axial loads in cables and beams contribute much of the stiffness of these structures in response to transverse loads. By including geometric nonlinearity, the membrane stiffness in response to transverse loads is considered as well.
The addition of material nonlinearity to an ABAQUS model is discussed in Chapter 10, “Materials.”
The introduction of boundary nonlinearity is discussed in Chapter 12, “Contact.”