## 2 CFD Model Setup and Validation
### Grid Generation and Validation Study  
In this study, a cylindrical computational domain sized 14D in length and 5D in radius is adopted, in which D represents the diameter of the propeller, as depicted in Figure 3a. The inlet is located 4D upstream of the propeller center and the outlet 10D downstream. The mesh is generated in a hybrid form in which the stationary domain is filled with a structured mesh and the rotating domain with an unstructured mesh. Prism layers are placed on the propeller, hub, and duct with smooth transition normal to the walls, as shown in Figure 4. The first layer height is so small that the maximum y+ value on the propeller is less than 15. As it is difficult to maintain a uniform grid size near the wall, a scalable wall function is employed, which resolves the boundary layer with varied near-wall treatment based on local y+ values. To resolve the high velocity gradients in the clearance and gap, 15 prism layers are placed between the propeller tip and the duct inner surface for the DP, while 20 prism layers are placed between the rim and the duct inner surface for the RDT. The computational domain is divided into stationary and rotating fluid zones by conformal interfaces, and the propeller, hub, and duct are contained in the rotating zone. The Moving Reference Frame (MRF) approach is utilized to handle the relative motion of the propeller. In the MRF, the governing equations for the flow in the selected rotating zone are solved in a relative rotating frame. At the interfaces, appropriate transformations of the velocity vector and velocity gradients are performed to compute fluxes of mass, momentum, and other scalars. As the MRF is a steady-state approximation of the actual flow, the interactions between the stationary and rotating components are ignored. Therefore, it requires much less computational resources compared to other approaches, such as the sliding mesh model. Figure 3: Computational domain: (**a**) overall mesh; (**b**) boundary conditions. There are some hydrodynamic-related coefficients that are used in this study, and they are defined as follows:  
\[J=\frac{V_{a}}{nD}, \tag{4}\]  
\[K_{t}=\frac{T}{\rho n^{2}D^{4}}, \tag{5}\]  
\[K_{q}=\frac{Q}{\rho n^{2}D^{5}}, \tag{6}\]  
\[\eta=\frac{J}{2\pi}\frac{K_{t}}{K_{q}}, \tag{7}\]  
\[C_{p}=\frac{p-p_{\infty}}{\frac{1}{2}\rho v^{2}}, \tag{8}\]  
where \(V_{a}\) is the inflow velocity in m\(\cdot\)s\({}^{-1}\), \(n\) is the rotation rate of the propeller in s\({}^{-1}\), \(\rho\) is the fluid density in kg\(\cdot\)m\({}^{-3}\), \(D\) is the diameter of the propeller in m, and \(J\), \(K_{t}\), \(T\), \(K_{q}\), \(Q\), and \(\eta\) are the advance coefficient, total thrust coefficient, total thrust, total torque coefficient, total torque, and efficiency, respectively; \(C_{p}\) is the pressure coefficient, \(p\) is the local pressure in Pa, \(p_{\infty}\) is the free stream pressure in Pa, and \(v\) is the representative velocity of the propeller, which in this study is \(\pi\pi D\). As related experimental data for RDTs are scarce, a validation study is carried out to verify and validate the numerical model. The physical model used for validation with experimental data was obtained from the study of [PERSON] [11], in which open water tests were performed for a Ka47 ducted propeller under a wide range of advance coefficients. Three sets of meshes have been generated to perform a mesh sensitivity analysis, from a coarse to a fine mesh with cell numbers increasing by a certain growth ratio in each direction. Detailed mesh parameters are given in Table 2. As the flow in the rotational zone changes much more rapidly than in the stationary zone, more grid cells are placed in the former to resolve the complex flow field around the propeller. The grid growth ratio is kept almost constant to ensure a better evaluation of the discretization error.