How can I choose between Implicit or Explicit Analysis in ABAQUS for a simple rectangular composite structure with 2 layers of unidirectional lamina? I am trying to do a linear-static analysis to capture the tensile strain for the specimen.
The basic difference between implicit and explicit dynamics solutions is that an explicit solution takes account of the finite propagation speed (at the speed of sound) of dynamic effects through the material. To do that, you need a mesh which is fine enough to represent the spatial effects (e.g. a "stress wave" propagating through the structure), and time-steps of the same order of magnitude as the transit time of sound waves from each element to its neighbours. If the time steps exceed that size, the response will usually be unstable and the analysis will fail after a few time steps. The time step size is limited by the smallest element in the model, not by the average size.
Implicit solution methods smear out those local effects. The propagation of dynamic effects around the structure is controlled by the inertia (mass) of the structure, not by local speed of sound. You can think of an implicit solution method as assuming the speed of sound is infinite, or (equivalently) that any applied load affects all of the structure instantaneously.
The mesh for an implicit solution only needs to be fine enough to capture the overall deformation of the structure, and the time steps only need to be small enough to capture the frequency spectrum of the response that you are interested in.
Unless you need the fine detail from an explicit analysis, an implicit solution will usually run much quicker - possibly several orders of magnitude quicker.
For example if you were modelling the dynamics of a road vehicle for typical driving conditions, you are probably mainly interested in the low-frequency response to bumps in the road etc, and the propagation of stresss and strains from one end of the vehicle to the other as "stress waves" with a timescale of the order of 1ms is irrelevant. But if you want to model the deformation of the same vehicle in a crash, capturing the local high-speed behaviour of the structure as it deforms is important, and you need to do an explicit analysis. Typically, the time step size for explicit dynamics is of the order of a microsecond.
A static analysis is "implicit" by definition - the static response ignores any transient behaviour that occurs while the loads are being applied to the structure.
In Abaqus there is some commonality between the Explicit and Implicit (a.k.a. Standard) analysis procedures. For example, you might want to do a dynamics analysis where the loads are suddenly removed from a pre-loaded structure. In that case, you could first do an (implicit) stress analysis, and use the steady-state results as the initial conditions for an (explicit) dynamics analysis.
Note, none of the above mentioned linear or non-linear behaviour - both explicit and implicit methods can be either linear or nonlinear. But in "real world" applications, there are usually quicker ways to model the high speed linear dynamics response of a structure, so the models analysed with Abaqus Explicit are usually nonlinear.
In Abaqus, there are two primary analysis methods used for solving structural problems, namely Abaqus/Standard and Abaqus/Explicit (includes dynamic Explicit). Abaqus/Standard has static implicit and dynamic implicit and is suitable for solving smooth nonlinear problems.
However, the solution of these problems may converge with difficulty, because of the contact or material complexities which can cause a large number of iterations. Such analyses are more expensive in Abaqus/Standard due to the iteration which needs many sets of linear equations to be solved. Meanwhile, Abaqus/Explicit conducts the solution without iterating by explicitly advancing the kinematic state from the previous increment.
In fact, Explicit stands for explicit time integration. Although a given analysis may require a large number of time increments by using the explicit method, the analysis requires much less disk space and memory compared with Abaqus/Standard which requires many iterations. Hence, for problems in which the computational costs of the two programs are comparable, the disk space and memory savings of Abaqus/Explicit make it more attractive.