## 2 Materials and Methods  
### Modeling and CFD Methodology  
The 3D model of the wavy-slit fin employed in this numerical analysis is illustrated in Figure 2a. The 3D model was created using Creo 6.0.6.0, and the geometric parameters of the fins are provided in Table 1.  
Figure 2: Modeling and meshing setup for CFD simulations. (**a**) 3D model of wavy-slit fin (**b**) Computational domain and boundary conditions (**c**) Grid system. To ensure sufficient flow development, convergence, and result accuracy, we extended the computational domain based on the reference length of 22.6 mm, which corresponds to the length of the region occupied by the heat exchanger within the computational domain, as outlined in [26]. The upstream was extended one time and the downstream two times this length. The configuration of the computational domain, including these extensions, was pretested and validated in a previously published study. For the boundary conditions in the numerical analysis, with the y-direction corresponding to the fin pitch direction as the reference, symmetry conditions were applied to both sides, and periodic conditions were imposed on the top and bottom. A velocity boundary condition was applied at the inlet, with the inlet velocity varying between 0.5 and 1.5 m/s, and the temperature was set to 284.95 K. The inlet turbulence conditions were specified using the intensity and length scale method, with a turbulence intensity of 1%, based on the experimental results of the suction fan that generates the airflow. The turbulence length scale was set to 1 mm, consistent with the characteristic length of the geometry. Pretesting showed that varying the turbulence length scale between 0.1 mm and 10 mm resulted in no significant differences in the simulation results, ensuring the robustness of the selected value. An atmospheric pressure condition was applied at the outlet (Figure 2b). The refrigerant flows within the tube, exchanging heat with the fins. Convective heat transfer boundary conditions were applied to the inner surface of the tube, with a heat transfer coefficient of 8000 W/m\({}^{2}\) and a temperature of 307.5 K. Additionally, the wall boundary condition was set to a no-slip condition. The physical phenomenon of the airflow under analysis was a 3D incompressible, steady-state-convection heat transfer problem. The governing equations are the time-averaged mass conservation equation, momentum equation, and energy equation [27]. - Continuity equation  
\[\frac{\partial}{\partial x_{\rm i}}(\rho U_{\rm i})=0 \tag{1}\]  
- Momentum equation  
\[\frac{\partial}{\partial x_{\rm j}}\big{(}\rho U_{\rm i}U_{\rm j}\big{)}=- \frac{\partial P}{\partial x_{\rm i}}+\frac{\partial}{\partial x_{\rm j}} \Bigg{(}\mu\left(\frac{\partial U_{\rm i}}{\partial x_{\rm j}}+\frac{ \partial U_{\rm j}}{\partial x_{\rm i}}\right)\Bigg{)}-\frac{\partial}{ \partial x_{\rm j}}(\rho\left\langle u_{\rm i}u_{\rm j}\right\rangle) \tag{2}\]  
- Energy equation  
\[\frac{\partial}{\partial x_{\rm j}}\big{(}\rho c_{p}U_{\rm j}T\big{)}=\frac{ \partial}{\partial x_{\rm j}}\Bigg{(}k\frac{\partial T}{\partial x_{\rm i}} \Bigg{)}-\frac{\partial\rho c_{p}\langle u_{\rm i}t\rangle}{\partial x_{\rm j}} \tag{3}\]  
The numerical analysis was conducted using the commercial software Ansys Fluent 2020 R1, which was used to perform incompressible Reynolds-averaged Navier-Stokes (RANS) simulations. The discretization method employed was the second-order upwind \begin{table}
\begin{tabular}{c c} \hline
**Design Parameters** & **Range (mm)** \\ \hline Fin pitch (\(F_{s}\)) & 1.25 \\ Transverse tube pitch (\(P_{\rm t}\)) & 16.7 \\ Longitudinal tube pitch (\(P_{\rm l}\)) & 10.3 \\ Collar outer diameter (\(D_{\rm c}\)) & 5.28 \\ Slit length (\(L\)) & 7.9–13.6 \\ Slit width (\(W\)) & 0.8–1.8 \\ Slit height (\(H\)) & 0.3125–0.8 \\ \hline \end{tabular}
\end{table} 
Table 1: Geometric dimensions of the fins. scheme, and pressure-velocity coupling was handled using the SIMPLE algorithm.