## 3 Numerical Simulation Study of Sub-Millimeter Liquid Droplets
### Computational Model Establishment and Verification  
The numerical calculations were conducted using the industrial simulation software ANSYS Fluent V20.2. It has been successfully applied to past aerodynamic fragmentation studies on liquid droplets under shock wave impacts [2726; 3234]. Turbulent flow simulations were conducted by applying the _k-w SST_ model in the context of unsteady Reynolds-averaged Navier-Stokes (RANS) equations. The solution method involved the use of a pressure-based coupled solver with the pressure-velocity coupling resolved through the PISO algorithm, which has been recognized for its efficiency in achieving convergence with fewer iterations. Spatial discretization of the pressure field was performed using the robust PRESTOI scheme, which is well suited for multiphase flow problems. The density, momentum, and turbulent kinetic energy were discretized with the third-order MUSCL scheme. The initial configuration of the sub-millimeter liquid droplets and the flow field was established with the Patch function. This function partitioned the computational domain into regions with uniform high- and low-pressure parameters to set the initial conditions for the propagating shock waves. The initial parameters on both sides of the shock waves were determined following the shock tube principles. Based on the flow conditions, a constant time step size of \(\Delta t=1\times 10^{-8}\) s was defined for the explicit transient simulations.  
Various grid densities were utilized to evaluate the grid independence in constructing the fluid domain, ensuring that the density had no impact on the computational outcomes. The non-dimensional displacement of the sub-millimeter droplets on the windward side was compared at a Mach number of 2.12 using various grid densities. CFD I utilized 1,686,528 cells, CFD II employed 2,502,892 cells, and CFD III featured 3,015,726 cells. Figure 10 demonstrates that there were no significant differences in the non-dimensional displacements of the sub-millimeter droplets over time for the three grid densities. To ensure both manageable computational demands and the complete capturing of the gas-liquid interface evolution, this study chose the grid density of CFD II for the subsequent three-dimensional numerical simulations of the sub-millimeter droplet aerodynamic breakup.  
In order to validate our numerical simulation method and ensure the accuracy of the subsequent computational results, we applied this method to calculate the dimensionless transverse deformation widths for two specific parameter conditions, C2 (Ma = 1.17 and \(d_{0}\) = 0.9) and D1 (Ma = 1.36 and \(d_{0}\) = 0.84), as defined by [PERSON] [26] for vertical airflow. The results are depicted in Figure 11. A comparison between these numerical simulation results and the experimental data highlighted the improved consistency when employing the numerical simulation method introduced in this paper. Nevertheless, due to the inherent uncertainties in the experimental measurements, there was no definitive value for the liquid phase volume fraction, \(\alpha_{I}\), that best fit the data. This variability contributed, to some extent, to the disparity between the numerical simulation results and the experimental outcomes.