Fully automatic time incrementation versus fixed time incrementation in Abaqus/Explicit

Abaqus/Explicit uses equations such as those discussed in the previous section to adjust the time increment size throughout the analysis so that the stability limit, based on the current state of the model, is never exceeded. Time incrementation is automatic and requires no user intervention, not even a suggested initial time increment. The stability limit is a mathematical concept resulting from the numerical model. Since the finite element program has all of the relevant details, it can determine an efficient and conservative stability limit. However, Abaqus/Explicit does allow the user to override the automatic time incrementation, if desired.

The time increment used in an explicit analysis must be smaller than the stability limit of the central-difference operator. Failure to use a small enough time increment will result in an unstable solution. When the solution becomes unstable, the time history response of solution variables such as displacements will usually oscillate with increasing amplitudes. The total energy balance will also change significantly. If the model contains only one material type, the initial time increment is directly proportional to the size of the smallest element in the mesh. If the mesh contains uniform size elements but contains multiple material descriptions, the element with the highest wave speed will determine the initial time increment.

In nonlinear problems—those with large deformations and/or nonlinear material response—the highest frequency of the model will continually change, which consequently changes the stability limit. Abaqus/Explicit has two strategies for time incrementation control: fully automatic time incrementation (where the code accounts for changes in the stability limit) and fixed time incrementation.

Two types of estimates are used to determine the stability limit: element by element and global. An analysis always starts by using the element-by-element estimation method and may switch to the global estimation method under certain circumstances.

The element-by-element estimate is conservative; it will give a smaller stable time increment than the true stability limit that is based upon the maximum frequency of the entire model. In general, constraints such as boundary conditions and kinematic contact have the effect of compressing the eigenvalue spectrum, and the element-by-element estimates do not take this into account.

The adaptive, global estimation algorithm determines the maximum frequency of the entire model using the current dilatational wave speed. This algorithm continuously updates the estimate for the maximum frequency. The global estimator will usually allow time increments that exceed the element-by-element values.

A fixed time incrementation scheme is also available in Abaqus/Explicit. The fixed time increment size is determined either by the initial element-by-element stability estimate for the step or by a time increment specified directly by the user. Fixed time incrementation may be useful when a more accurate representation of the higher mode response of a problem is required. In this case, a time increment size smaller than the element-by-element estimates may be used. When fixed time incrementation is used, Abaqus/Explicit will not check that the computed response is stable during the step. The user should ensure that a valid response has been obtained by carefully checking the energy history and other response variables.