Choosing between implicit and explicit analysis

For many analyses it is clear whether Abaqus/Standard or Abaqus/Explicit should be used. For example, as demonstrated in Nonlinearity, Abaqus/Standard is more efficient for solving smooth nonlinear problems; on the other hand, Abaqus/Explicit is the clear choice for a wave propagation analysis. There are, however, certain static or quasi-static problems that can be simulated well with either program. Typically, these are problems that usually would be solved with Abaqus/Standard but may have difficulty converging because of contact or material complexities, resulting in a large number of iterations. Such analyses are expensive in Abaqus/Standard because each iteration requires a large set of linear equations to be solved.

Whereas Abaqus/Standard must iterate to determine the solution to a nonlinear problem, Abaqus/Explicit determines the solution without iterating by explicitly advancing the kinematic state from the end of the previous increment. Even though a given analysis may require a large number of time increments using the explicit method, the analysis can be more efficient in Abaqus/Explicit if the same analysis in Abaqus/Standard requires many iterations.

Another advantage of Abaqus/Explicit is that it requires much less disk space and memory than Abaqus/Standard for the same simulation. For problems in which the computational cost of the two programs may be comparable, the substantial disk space and memory savings of Abaqus/Explicit make it attractive.

Table 1 lists the key differences between the analysis products, which are discussed in detail in the relevant chapters in this guide.

Table 1. Key differences between Abaqus/Standard and Abaqus/Explicit.
Quantity Abaqus/Standard Abaqus/Explicit
Element library Offers an extensive element library. Offers an extensive library of elements well suited for explicit analyses. The elements available are a subset of those available in Abaqus/Standard.
Analysis procedures General and linear perturbation procedures are available. General procedures are available.
Material models Offers a wide range of material models. Similar to those available in Abaqus/Standard; a notable difference is that failure material models are allowed.
Contact formulation Has a robust capability for solving contact problems. Has a robust contact functionality that readily solves even the most complex contact simulations.
Solution technique Uses a stiffness-based solution technique that is unconditionally stable. Uses an explicit integration solution technique that is conditionally stable.
Disk space and memory Due to the large numbers of iterations possible in an increment, disk space and memory usage can be large. Disk space and memory usage is typically much smaller than that for Abaqus/Standard.