## 2 Model Development and Simulation Method
### CFD Analyses and Boundary Settings  
The mesh generation should balance simulation reliability against the computer calculation process. For the cooling plate and flowing water domain, structural hexahedral mesh was adopted since the model configuration was regular, as shown in Figure 1. After mesh generation using Ansys ICEM, the tool \"mesh quality\" in Ansys Workbench was used to check whether the mesh quality was good enough, and it was found that the values of all designs were near to 1 (1 means the best and 0 means the worst in Ansys Workbench). Then grid independence was studied. Case 2 in Section 3.2 was used as an example, and its results are shown in Figure 2. With the growth of grid number, the pressure drop of the inlet and outlet in the cooling plate was changing. Until the number of grids increased to 0.126 million, the curves of supervised pressure drop became smooth and steady. In overall consideration of hardware equipment, calculating time, and simulation error the total number of grids was set to be about 0.126 million in simulations that were conducted. The quantity and quality of mesh met the calculation requirements well and the construction method could be applied to the other models.  
The FLUENT CFD solver was used to solve the governing equations for the conservation of mass, momentum, and energy for a Newtonian incompressible fluid. This study only considered the steady state condition, and the relevant equations are summarized as:  
\[\frac{\partial u_{i}}{\partial x_{i}}=0 \tag{3}\]  
\[\rho\frac{\partial\bigl{(}u_{i}u_{j}\bigr{)}}{\partial x_{i}}+\frac{\partial p }{\partial x_{i}}=\frac{\partial}{\partial x_{i}}(\mu\frac{\partial u_{j}}{ \partial x_{i}}) \tag{4}\]  
\[\rho\frac{\partial\bigl{(}u_{i}c_{p}T\bigr{)}}{\partial x_{i}}=\frac{\partial }{\partial x_{i}}(\lambda\frac{\partial T}{\partial x_{i}}) \tag{5}\]  
Figure 2: Grid independence of Case 2 in Section 3.2.  
where \(u\) and \(x\) represent the velocity and direction vectors in Cartesian space; \(\rho\) is the density; \(p\) is the pressure; \(\mu\) is the fluid viscosity; \(c_{p}\) is the specific heat capacity; \(T\) is the temperature; and \(\lambda\) is the thermal conductivity.  
Due to different channel widths in different designs, the \(Re\) number will be different, and is calculated by:  
\[Re=\frac{\rho ud_{h}}{\mu} \tag{6}\]  
where \(d_{h}\) is equivalent hydraulic diameter and is equal to 4_A/P_ in the rectangular channel. Here \(A\) is the cross section area of the channel, and \(P\) is the wet perimeter of the channel. According to this formula, the \(Re\) number of Figure 1a as well as Figure 1b was 2.443, and the others in Figure 1 were equal to 16.08. Hence, the simulation adopted a laminar flow model.  
The coolant temperature of the inlet was fixed at 360 K and its mass volume flow was 0.1664 kg\(\cdot\)s\({}^{-1}\). The top surface was set to be free convection with a coefficient of 10 W/m\({}^{2}\cdot\)K [22] and the surfaces of the solid and fluid were specified to be the interface. An adiabatic surface was applied to the other surfaces of the model. Aluminum and water were applied to the plate and coolant, respectively. At the outlet plane, the reference pressure (atmosphere pressure) was used here. For the coupling of the continuity and momentum equations, the solver used the Segregated/Implicit type, and adopted the SIMPLE algorithm to solve the coupled analyses of speed and pressure. This type of discrete equation adopts a second order upwind scheme. Convergence in all cases was declared only when both strict criteria were satisfied: (a) reduction in all residuals of five orders of magnitude at least; and (b) no observable change in surface temperature prediction for additional tens of iterations.