## 2 Materials
### 3D CFD Model  
A commercial Computational Fluid Dynamics (CFD) code, CONVERGE v.2.4.33 [49], was used to implement the numerical model of the cylinder. A summary of the main features of the numerical model is shown in Table 2. The most relevant physical models, numerical schemes, and mesh details are presented here. The basis of the model has been widely described in previous investigations [50].  
The computational domain obtained from the sketch of Figure 1 was meshed using a modified cut-cell Cartesian method directly in runtime. The base grid mesh (4 mm) was reduced in those regions where flow features have higher complexity. For instance, intake/exhaust ports were refined to 2 mm in cell size. Moreover, an adaptive mesh refinement (AMR) strategy was considered to increase the grid resolution in those regions where the sub-grid field is more prominent. The AMR cell size decreases to 0.25 mm when the sub-grid scale of velocity exceeds 1 m/s. A second-order central difference scheme was considered for spatial discretization, and a first-order scheme was considered for temporal discretization. The pressure-velocity coupling was solved by a modified Pressure Implicit with a Splitting of Operators (PISO) algorithm [54]. The in-cylinder turbulence was modeled in the frame of unsteady Reynolds-averaged Navier-Stokes (URANS) with the eddy-viscosity-based two-equation turbulence model (RNG k-\(\epsilon\) model), used widely in ICE applications [53].  
Regarding the boundary conditions, the piston, liner, and cylinder head wall temperatures were estimated from the experiments by a lumped thermal model. All instantaneous  
\begin{table}
\begin{tabular}{c c} \hline \hline \multicolumn{2}{c}{**Mesh Details**} \\ \hline Base size & 4 mm \\ \hline Cell size intake/exhaust ports & 2 mm \\ \hline Combustion chamber size & 1 mm \\ \hline Walls refinement & 0.5 mm \\ \hline Minimum cell size by AMR & 0.25 mm \\ \hline \hline \multicolumn{2}{c}{Numerical schemes} \\ \hline Spatial discretization & The second-order central difference scheme \\ \hline Temporal discretization & The first-order central difference scheme \\ \hline Momentum equation correction & PISO algorithm [51] \\ \hline \multicolumn{2}{c}{Physical models} \\ \hline Turbulence & URANS RNG k-e [52] \\ \hline Heat transfer & O’Rourke and Amsden [53] \\ \hline \hline \end{tabular}
\end{table}
Table 2: CFD model setup.  
signals at the intake/exhaust manifolds were obtained from the 1D model described in the previous section and provided as inflow/outflow boundary conditions. The wall heat transfer was estimated by the O'Rourke and Amsden model [55]. This approach is suitable for those simulations in which the turbulent boundary layer resolution is insufficient (i.e., in ICE simulations where the viscous sub-layer is not strictly resolved). The model calculates the wall heat-transfer from  
\[K\frac{\partial T}{\partial x_{i}}=\frac{\mu_{m}c_{p}F\Big{(}T_{f}-T_{w}\Big{)} }{Pr_{m}y}n_{i}, \tag{3}\]  
\[F=\left\{\begin{array}{c}1.0\ y^{\prime}<11.05\\ \frac{\Big{(}\frac{\
u P_{m}}{\
u_{t}}\Big{)}}{\frac{1}{k}ln(y^{\prime})+B+11. 05\Big{(}\frac{P_{m}}{\
u_{t}}-1\Big{)}}\ y^{\prime}>11.05,\\ y^{\prime}=\frac{\rho u_{\tau}y}{\mu_{m}}\,\end{array}\right. \tag{4}\]  
where \(k\) is the molecular conductivity, \(Pr_{m}\) is the molecular Prandtl number, \(Pr_{t}\) is the turbulent Prandtl number, \(T_{f}\) is the fluid temperature, \(T_{w}\) is the temperature of the wall, \(u_{\tau}\) is the shear speed, \(k\) is the [PERSON] constant (0.4187), and \(B\) is a constant that depends on the turbulence model.  
The convective heat transfer in fluid during scavenging is calculated using the above model to predict the heat transfer coefficient. This heat transfer coefficient will be used in subsequent studies.