Automatic incrementation control in Abaqus/Standard

Abaqus/Standard automatically adjusts the size of the load increments so that it solves nonlinear problems easily and efficiently. You only need to suggest the size of the first increment in each step of your simulation. Thereafter, Abaqus/Standard automatically adjusts the size of the increments. If you do not provide a suggested initial increment size, Abaqus/Standard will try to apply all of the loads defined in the step in the first increment. In highly nonlinear problems Abaqus/Standard will have to reduce the increment size repeatedly, resulting in wasted CPU time. Generally it is to your advantage to provide a reasonable initial increment size (see Modifications to the model for an example); only in very mildly nonlinear problems can all of the loads in a step be applied in a single increment.

The number of iterations needed to find a converged solution for a load increment will vary depending on the degree of nonlinearity in the system. By default, if the solution appears to diverge, Abaqus/Standard abandons the increment and starts again with the increment size set to 25% of its previous value. An attempt is then made at finding a converged solution with this smaller load increment. If the increment still fails to converge, Abaqus/Standard reduces the increment size again. By default, Abaqus/Standard allows a maximum of five cutbacks of increment size in an increment before stopping the analysis.

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 present. In Abaqus/Standard you specify the initial time increment, Δ⁢Ti⁢n⁢i⁢t⁢i⁢a⁢l, and the total step time, Tt⁢o⁢t⁢a⁢l. 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

Δ⁢Ti⁢n⁢i⁢t⁢i⁢a⁢lTt⁢o⁢t⁢a⁢l×Load Magnitude.

The choice of initial time increment can be critical in certain nonlinear simulations in Abaqus/Standard, but for most analyses an initial increment size that is 5% to 10% of the total step time is usually sufficient. In static simulations the total step time is usually set to 1.0 for convenience, unless, for example, rate-dependent material effects or dashpots are included in the model. With a total step time of 1.0 the proportion of load applied is always equal to the current step time; i.e., 50% of the total load is applied when the step time is 0.5.

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, Δ⁢Tm⁢i⁢n, is 10−5 times the total step time. By default, Abaqus/Standard has no upper limit on the increment size, Δ⁢Tm⁢a⁢x, 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 Δ⁢Tm⁢a⁢x.

If the increment converges in fewer than five iterations, this indicates that the solution is being found fairly easily. Therefore, Abaqus/Standard automatically increases the increment size by 50% if two consecutive increments require fewer than five iterations to obtain a converged solution.

Details of the automatic load incrementation scheme are given in the Job Diagnostics dialog box, as shown in more detail in Job diagnostics.