*2.2. Computational Model*

The commercial finite element package ABAQUS [27] was used to solve for the stresses, strains, and displacements that result from the application of laser peening on thin sheets of Al2024-T351. Based on previous work [11,25,30–33], all simulations were run using explicit time integration (ABAQUS/Explicit) to solve the dynamic system. As discussed in [25], using an explicit solver to model both the impact event and the subsequent return to equilibrium is quicker, more scalable, and uses less memory than performing the equilibrium analysis with an implicit solver. Each impact pulse was modeled using two distinct solution steps so that the computational parameters could be adjusted for improved efficiency and convergence. The first solution step, designated as the pulse phase, starts with the initial application of the pressure pulse and ends when no further plastic deformation occurs (2.5 μs was used). The second solution step, termed the equilibrium phase, introduces Rayleigh damping [34] into the model to return the system to a state of near-zero kinetic energy (approximately 10−<sup>6</sup> to approximate equilibrium: 100 μs was used). One pair of analyses is performed for each laser pulse.

Three-dimensional linear eight-node brick elements with reduced integration (C3D8R in Abaqus terminology) were used throughout, with a mesh size of 50 μm in the laser peened region. This mesh size was selected using the results of convergence studies that showed less than 2% di fference in predicted residual stresses with further refinement. External to the peened region the element size was increased gradually from 50 μm to 250 μm using mesh biasing to curtail computational costs.
