Analysis of Wake Characteristics for Contra-Rotating Propellers by CFD

1 Analysis of Wake Characteristics for Contra-Rotating Propellers by CFD Sua Jeong1, Kwang-Jun Paik1, * Seong-Jin Eom1 1 Department of Naval Architecture and Ocean Engineering, Inha University, Incheon, South Korea Abstract. This study aims to evaluate the wake flow characteristics of a Contra-Rotating Propeller (CRP) system through high-resolution numerical simulations and analyze their influence on propulsion performance. A CRP, consisting of two coaxial propellers rotating in opposite directions, enhances propulsion efficiency by recovering residual rotational energy and attenuating vortex intensity in the wake flow. This configuration contributes to fuel savings and greenhouse gas reduction, providing a practical solution for meeting environmental regulations such as the International Maritime Organization (IMO)’s net-zero target for 2050. In this study, the Reynolds-Averaged Navier-Stokes (RANS) and Large Eddy Simulation (LES) models were applied to simulate the flow around a CRP system. Comparative analyses were conducted to examine differences in wake flow structures, thrust and torque characteristics, and tip vortex formation captured by each turbulence model. The vortex generation, development, and dissipation processes were visualized using Qcriterion and axial velocity fields, enabling a more detailed interpretation of the wake dynamics. The LES model, in particular, demonstrated superior capability in resolving fine-scale flow structures and capturing unsteady flow behavior, such as rotational energy recovery and vortex breakdown, which are difficult to predict with time-averaged models like RANS. All simulations were performed using STAR-CCM+ (version 18.06), and mesh convergence was validated using the Grid Convergence Index (GCI) method to ensure numerical reliability. The results confirm that LES is an effective tool for analyzing the complex hydrodynamic interactions inherent in CRP systems and provides valuable insights into wake flow physics. The findings of this study are expected to serve as a foundation for the design and optimization of CRP systems and contribute to the advancement of high-efficiency, eco-friendly ship propulsion technologies. Keywords: Contra-Rotating Propeller (CRP), RANS (Reynolds-Averaged Navier-Stokes), LES (Large Eddy Simulation), Energy Efficiency, Turbulent Flow Analysis, CFD 1 Introduction 1.1 Strengthening of IMO Environmental Regulations and the Need for Eco-Friendly Propulsion Systems In response to the increasing demand for environmental sustainability, the International Maritime Organization (IMO) adopted the IMO 2023 Greenhouse Gas Strategy, which establishes an ambitious target of achieving netzero greenhouse gas (GHG) emissions from international shipping by 2050. Furthermore, during the 83rd session of the Marine Environment Protection Committee (MEPC) held in April 2025, the IMO introduced mandatory regulations requiring vessels of 5,000 gross tonnage and above to maintain their annual Greenhouse Gas Fuel Intensity (GFI) below a specified threshold [1]. GFI is a comprehensive metric that not only reflects the carbon characteristics of marine fuels but also incorporates the overall energy consumption associated with ship construction, propulsion efficiency, and operational conditions. Consequently, mere fuel substitution is inadequate to ensure compliance with the revised regulatory framework. Instead, technological innovations that enhance ship propulsion system efficiency have become imperative, thereby accelerating global interest in eco-friendly propulsion technologies. Among such technologies, the contra-rotating propeller (CRP) system has emerged as a promising solution for improving propulsion efficiency. The CRP system employs two coaxial propellers rotating in opposite directions, wherein the aft propeller effectively recovers the rotational energy imparted by the forward propeller, reducing rotational losses and mitigating vortex strength [2]. This mechanism not only leads to substantial fuel savings but also contributes to the reduction of GHG emissions, positioning the CRP system as a viable and practical technology for compliance with emerging environmental standards. * Correspondence to: [email protected] 16th International Symposium on Practical Design of Ships and Other Floating Structures PRADS 2025 Ann Arbor, MI, USA, October 19th – 23rd 2025 2 However, the inherent proximity of the two counter-rotating propellers inevitably results in complex vortex structures and pronounced blade-to-blade interactions within the wake field. Consequently, accurate performance predictions of CRP systems remain challenging when relying solely on conventional simplified models or experimental methods. Accordingly, the present study aims to quantitatively evaluate the improvements in propulsion efficiency afforded by CRP systems and assess their potential to comply with the latest IMO and MEPC environmental regulations. 1.2 Characteristics of Contra-Rotating Propellers (CRP) The CRP system has been widely recognized as an effective solution for enhancing propulsion efficiency by recovering rotational energy losses and reducing vortex strength through the counter-rotation of the aft propeller, which cancels the residual swirl generated by the forward propeller. This mechanism contributes not only to fuel savings but also significantly reduces GHG emissions, thereby establishing the CRP system as a practical and viable technology for commercial ship applications. Nevertheless, the inherently close configuration of the two oppositely rotating propellers induces complex wake vortex structures and significant hydrodynamic interactions, presenting substantial challenges in accurately predicting the performance of CRP systems. As such, conventional simplified models and experimental methods are insufficient for precise performance evaluation. Moreover, the CRP system allows for the adjustment of various geometric and operational parameters, including blade number, diameter ratio, shaft spacing, and rotation speed ratio, all of which have a direct impact on propulsion efficiency and performance characteristics. Previous studies have reported that variations in these parameters can result in efficiency deviations of up to 5–10%, and even minor adjustments can lead to substantial changes in overall performance due to the strong hydrodynamic coupling between the two propellers [3]. Accordingly, a detailed analysis of the wake flow structures in CRP systems, capable of capturing subtle variations in efficiency, is essential for practical optimization and design refinement of CRP systems. 1.3 Necessity of CFD and Potential Flow Analysis In this context, high-fidelity computational methods based on Computational Fluid Dynamics (CFD) have been actively employed to overcome the limitations of conventional approaches. While analyses utilizing the ReynoldsAveraged Navier-Stokes (RANS) equations are effective for predicting overall flow structures, advanced turbulence modeling approaches such as Detached Eddy Simulation (DES) and Large Eddy Simulation (LES) have recently been adopted to capture detailed flow phenomena, including tip vortex dynamics, blade-to-blade interactions, and energy transfer mechanisms. Several studies have highlighted the superiority of LES in resolving tip vortices and turbulent structures, making it an indispensable tool for quantitative analysis of the complex wake flows characteristic of CRP systems. LES incorporates wall treatment models such as the Wall-Adapting Local Eddy-Viscosity (WALE) model to accurately capture near-wall boundary layer flows, while directly resolving the energy cascade and vortex breakdown processes in the wake region, allowing LES to reproduce much finer flow structures than those attainable with RANS [4]. When applied to wake flow analysis, LES enables the quantitative evaluation of flow field characteristics using various diagnostic tools, including energy spectrum analysis, Q-criterion-based vortex visualization, timeaveraged velocity fields, and turbulence intensity distributions, facilitating the identification of detailed turbulent structures that are difficult to resolve using RANS or potential flow methods. Although previous studies have extensively investigated the general performance and flow field characteristics of CRP systems, the present study specifically focuses on the precise analysis of changes in wake flow structures resulting from variations in propeller rotational speed. In the case of electric propulsion vessels, which allow realtime adjustment of propeller RPM, such optimization is crucial for improving propulsion efficiency under varying operational conditions and is also highly relevant in terms of complying with environmental regulations. Meanwhile, Paik et al. [5] conducted RANS-based simulations coupled with SPIV measurements to investigate the wake evolution and primary flow characteristics of CRP systems, while Paik [6] also employed RANS methods to analyze wake structures and performance variations. These studies demonstrated that while RANS methods are effective in evaluating the general flow characteristics, the inherent limitations of the average governing equations restrict their capability in resolving fine-scale vortex structures and turbulent flow phenomena, indicating the necessity for complementary high-resolution analysis. However, due to the high computational cost associated with LES, its application across all rotational speed conditions is impractical. Therefore, this study adopts a complementary approach combining RANS-based simulations and potential flow methods. High-fidelity wake flow analyses are conducted using LES at selected 3 optimized rotation speeds and propeller configurations, while broader parametric studies are performed using potential flow codes and RANS simulations to identify optimal operating conditions. Higher-order Boundary Element Method (BEM) approaches, such as the one developed by Paik, Suh, and Chun [7], have been widely applied for the performance evaluation of marine propellers under steady flow conditions. Although such methods have proven effective in general performance prediction, they remain limited in resolving the intricate wake vortex interactions present in CRP systems. Accordingly, this study employs multiple turbulence models, including RANS, DES, and LES, to conduct a detailed investigation of the wake flow characteristics of CRP systems and to quantitatively analyze variations in flow structures and propulsion performance induced by changes in rotational speed. The commercial CFD solver STAR-CCM+ was utilized for all simulations, and the reliability of the results was ensured through grid convergence verification using the Grid Convergence Index (GCI) [8]. It is anticipated that the outcomes of this study will provide valuable insights for the optimization of CRP designs through the quantitative analysis of complex wake flows, thereby contributing to the development of ecofriendly, high-efficiency ship propulsion systems. 2 Methodology 2.1 Numerical Methods In this study, a combined approach employing both Computational Fluid Dynamics (CFD) and potential flow methods was adopted to accurately predict the wake flow characteristics of a contra-rotating propeller (CRP) system under varying rotational speeds. This complementary strategy enabled the leveraging of the strengths of each method while compensating for their respective limitations. The CFD analyses were carried out using the commercial software STAR-CCM+ (Version 18.06), applying two turbulence modeling approaches as described in the following sections. 2.1.1 Numerical Methods : Potential For the initial performance prediction and wake flow analysis of the CRP system, a potential flow code developed by Paik et al. [7] was utilized. This method is based on the Vortex Lattice Method (VLM), which assumes inviscid and incompressible flow conditions, and solves the Laplace equation, given as Equation (1), as its governing equation: ∇2𝜙 = 0 (1) where 𝜙 is the velocity potential. Source distributions and vortex lattices were placed on the blade surfaces to model the entire flow field. The source distribution was adjusted to satisfy the Kutta condition at the blade trailing edge, ensuring smooth flow separation and enabling physically consistent modeling of the wake vortex strength. Additionally, to incorporate the interactions characteristic of CRP systems into the potential flow model, the flow field generated by the forward propeller was accounted for in the calculation of the aft propeller, thereby enabling the simulation of blade-to-blade interaction phenomena inherent to contra-rotating systems. Under this configuration, the aft propeller received the velocity field generated by the forward propeller as its inflow boundary condition, allowing the calculation of thrust, torque, and efficiency while considering the interference effects between the two propellers. 2.1.2 Numerical Methods : RANS The Reynolds-Averaged Navier-Stokes (RANS) model predicts the mean flow field by applying statistical averaging to the governing equations through Reynolds decomposition, wherein the turbulent fluctuation components are represented as averaged terms. While the RANS model exhibits limitations in capturing complex flow phenomena such as boundary layer separation and large-scale vortex structures, it offers the advantages of high computational efficiency and the capability to predict the overall flow field characteristics. The governing equations for incompressible Newtonian fluids are expressed using Einstein's index notation, as shown in Equation (2): 𝜕𝑢𝑖 𝜕𝑡 + 𝑢𝑗 𝜕𝑢𝑖 𝜕𝑥𝑗= − 1 𝜌 𝜕𝑝 𝜕𝑥𝑗+ 𝑣 𝜕2𝑢𝑖 𝜕𝑥𝑗 2 (2) 4 where 𝑢𝑖 is the flow velocity, 𝜌is the fluid density, 𝑝 is the pressure, and 𝑣 is the kinematic viscosity. By applying Reynolds decomposition to the velocity components and performing time-averaging, the governing equations can be reformulated as the Reynolds-Averaged Navier-Stokes (RANS) equations, given as Equation (3): 𝜕𝑢𝑖  𝜕𝑡 + 𝑢𝑗 𝜕𝑢𝑖  𝜕𝑥𝑗= − 1 𝜌 𝜕𝑝 𝜕𝑥𝑖+ 𝑣 𝜕2𝑢𝑖  𝜕𝑥𝑗 2−𝜕𝑢𝑖 ′𝑢𝑗 ′       𝜕𝑥𝑗 (3) In these equations, the last term on the right-hand side represents the Reynolds stress tensor, which must be modeled using an appropriate turbulence model. In the present study, the Shear Stress Transport (SST) 𝑘 − 𝜔 model was employed for propeller flow analysis. The 𝑆𝑆𝑇 𝑘 − 𝜔 model combines the strengths of the standard 𝑆𝑆𝑇 𝑘 − 𝜔 formulation in the near wall region with the 𝑆𝑆𝑇 𝑘 − 𝜀 model characteristics in the free stream region, enabling more accurate predictions of flow separation and vortex generation compared to conventional twoequation models. Although the RANS approach significantly enhances computational efficiency by averaging the entire flow field, its capability to resolve fine-scale vortices and turbulent structures is inherently limited by the turbulence model applied. 2.1.3 Numerical Methods : LES Large Eddy Simulation (LES) applies spatial filtering to the Navier-Stokes equations, enabling the direct resolution of large-scale turbulent eddies through numerical methods, while the effects of smaller subgrid-scale (SGS) eddies are modeled using appropriate subgrid-scale models. The governing equations for LES are the filtered Navier-Stokes equations, given as Equation (4): 𝜕𝑢𝑖  𝜕𝑡 + 𝑢𝑗 𝜕𝑢𝑖  𝜕𝑥𝑗= −1 𝜌 𝜕𝑝 𝜕𝑥𝑖+ 𝑣 𝜕2𝑢𝑖  𝜕𝑥𝑗 2−𝜕𝜏𝑖𝑗 𝜕𝑥𝑗 (4) where 𝜏𝑖𝑗 denotes the subgrid-scale (SGS) stress tensor, representing the effects of unresolved smaller eddies on the resolved flow field. In the present study, the Wall-Adapting Local Eddy-Viscosity (WALE) model was employed to compute the turbulent viscosity, providing accurate predictions even within near-wall boundary layers. The WALE model adjusts the turbulent viscosity locally not only in regions of high shear stress but also in areas dominated by strong rotational vortices, offering superior accuracy in wall-bounded flow regions compared to conventional LES wall treatment models. This capability enables the high-resolution simulation of boundary layer separation as well as the generation and dissipation of tip vortices, even in highly complex flow regions. By integrating CFD and potential flow analyses, a complementary approach was adopted in this study, wherein the potential flow method facilitated rapid parametric studies, while LES was applied for high-fidelity flow field analysis. This combined approach enabled comprehensive investigations of wake flow structures under various propeller rotational speed conditions, thereby supporting efficient and reliable performance assessments of the CRP system. 2.1.4 Nondimensionalization for Single Propeller and CRP System For the analysis of the CRP system conducted in this study, the performance coefficients were nondimensionalized based on the forward propeller, following the methodology proposed by Van Manen [9]. The key nondimensional performance parameters advance coefficient (𝐽), thrust coefficient (𝐾𝑇), and torque coefficient (𝐾𝑄) are defined by Equations (5) – (7), respectively: 𝐴𝑑𝑣𝑎𝑛𝑐𝑒 𝐶𝑜𝑒𝑓𝑓𝑖𝑐𝑖𝑒𝑛𝑡(𝐽)= 𝑉 𝑎 𝑛𝑓𝐷𝑓 (5) 𝑇ℎ𝑟𝑢𝑠𝑡 𝐶𝑜𝑒𝑓𝑓𝑖𝑐𝑖𝑒𝑛𝑡(𝐾𝑇)= 𝑇𝑓+ 𝑇𝑎 𝜌𝑛𝑓 2𝐷𝑓 4 (6) 𝑇𝑜𝑟𝑞𝑢𝑒 𝐶𝑜𝑒𝑓𝑓𝑖𝑐𝑖𝑒𝑛𝑡(𝐾𝑄) = 𝑛𝑓𝑄𝑓+ 𝑛𝑎𝑄𝑎 𝜌𝑛𝑓 3𝐷𝑓 5 (7) 5 where 𝑉 𝑎 is the inflow velocity, 𝑛𝑓 and 𝑛𝑎 are the rotational speeds of the forward and aft propellers, respectively, 𝐷𝑓 is the diameter of the forward propeller, and 𝑇𝑓, 𝑇𝑎, 𝑄𝑓, and 𝑄𝑎 represent the thrust and torque of the forward and aft propellers, respectively. All nondimensionalization was performed using the rotational speed and diameter of the forward propeller as the reference parameters. This approach was adopted to evaluate the overall propulsion performance of the CRP system based on the forward propeller characteristics. 2.2 Target Model For this study, a contra-rotating propeller (CRP) system developed by Hyundai Heavy Industries was selected as the reference model [10]. This CRP system was specifically designed for full-scale ship applications with the objective of maximizing propulsion efficiency and enhancing rotational energy recovery performance. The principal particulars of the analyzed CRP system are detailed in Table 1. Experimental fluid dynamics (EFD) data for this CRP system were obtained from model tests conducted at a scale ratio of 1/42.063 in the deep-water towing tank of the Hyundai Maritime Research Institute (HMRI). These tests, including open-water and self-propulsion experiments, have been reported in Min et al. [10] and provide the reference for the present CFD validation. Table 1. Principal particulars of the contra-rotating propeller system analyzed in this study Forward Propeller After Propeller Diameter 9.1 m 7.9 m Number of Blades 5 4 RPM 70.1 RPM 93.5 RPM Thrust Ratio 50 50 Separation Distance 2.06 m Inflow velocity 12.86 m/s 2.3 Computational Setup All CFD simulations were performed using the commercial software STAR-CCM+ (Version 18.06). For the RANS simulations, the Shear Stress Transport 𝑆𝑆𝑇 𝑘 − 𝜔 turbulence model was employed to resolve the timeaveraged flow field with particular emphasis on the accurate prediction of near wall boundary layer behavior. Throughout the entire blade surface, the dimensionless wall distance Y+ was maintained below 1.5, as shown in Figure 1. For the LES simulations, the Wall-Adapting Local Eddy Viscosity (WALE) model was adopted to explicitly resolve the major turbulent structures. The time step size for both RANS and LES simulations was determined in accordance with the International Towing Tank Conference (ITTC) recommended guidelines [11] to ensure numerical stability and result accuracy. The computational domain was discretized using an unstructured mesh approach. Additional mesh refinement was applied in the vicinity of the propeller blades and within the downstream wake region to adequately capture wake contraction phenomena, turbulent energy transfer, and the formation and decay of tip vortices. Figure 1. Computational mesh topology around the CRP propeller and downstream wake region used for CFD analysis. 6 2.4 Grid Convergence Index To ensure the reliability of the CFD results, grid convergence verification was performed following the procedures recommended by the International Towing Tank Conference (ITTC). The Grid Convergence Index (GCI) method, as proposed by Celik et al. [8], was employed to quantitatively assess discretization uncertainty. For this purpose, three levels of mesh resolution were prepared, and the sensitivity of the key performance parameters specifically, the thrust coefficient (𝐾𝑇) and torque coefficient (𝐾𝑄) was evaluated. The GCI method provides an estimate of the discretization error associated with the finest mesh and enables the calculation of the convergence ratio (𝑅𝐺), thereby facilitating the assessment of the grid independence of the numerical solution. In this study, the GCI analysis was conducted for the LES simulations, and the coarse mesh configuration obtained from the analysis was subsequently applied in the RANS simulations. The results of the grid convergence studies for the thrust and torque coefficients are summarized in Tables 2 and 3, respectively. Table 2. Grid convergence study of thrust coefficient (𝐾𝑇) using Grid Convergence Index (GCI) method Num. of Grid [M] 𝐾𝑇 𝑅𝐺 GCI Coarse 64.2 0.7498 0.102 0.137 % Medium 90.8 0.7571 Fine 128.4 0.7578 Table 3. Grid convergence study of torque coefficient (𝐾𝑄) using Grid Convergence Index (GCI) method Num. of Grid [M] 𝐾𝑄 𝑅𝐺 GCI Coarse 64.2 0.1463 0.133 0.185 % Medium 90.8 0.1478 Fine 128.4 0.1481 Figure 2. Grid convergence trend of thrust coefficient (𝐾𝑇) and torque coefficient (𝐾𝑄) with respect to the number of grids. As shown in Figure 2, the GCI values for both the thrust coefficient 𝐾𝑇 and torque coefficient 𝐾𝑄 were confirmed to be within approximately 0.1%, thereby verifying the grid convergence of the numerical simulations. Figure 3 shows the computational domain and boundary conditions used in this study. A cylindrical domain was arranged along the propeller axis, with an axial length of approximately 8D, so that the inflow and the generation and dissipation of the wake could be adequately reproduced. The inflow was set as an inlet, where a uniform inflow velocity and turbulence conditions were imposed, while the outflow plane was defined as an outlet with a pressurebased boundary condition. The outer wall of the domain was assigned a slip boundary condition. This condition assumes that the fluid slides along the wall without friction, modeling a state without viscous resistance, in which the tangential velocity component is allowed to flow freely while the normal velocity component is suppressed. Through this setting, the growth of viscous boundary layers and shear stresses near the wall are eliminated, ensuring that the outer boundary of the domain does not impose artificial effects on the flow. Figure 4 presents the actual mesh distribution around the propeller blades and the wake region. From the front view and the axial cross- 7 section, boundary-layer resolving prism layers are arranged near the blade surfaces, with a gradual transition in grid size. To accurately capture the generation, development, and trajectory of the tip vortices shed from the blade tips, local mesh refinement was applied along the predicted vortex path. This finely refined region was designed to ensure that the vortices formed in the wake are stably resolved without numerical dissipation or artificial attenuation, and the mesh was extended downstream to encompass the entire wake dissipation region. Figure 3. Computational domain and boundary conditions for propeller CFD analysis Figure 4. Computational mesh topology around the propeller blade and wake region 8 3 Results and Discussion In this study, the wake flow characteristics of a contra-rotating propeller (CRP) system were investigated through comparative simulations employing both RANS and LES approaches. These methods were used to calculate the axial velocity distribution and analyze the wake flow structures of the CRP system. In addition, the LES model was applied to compare the flow characteristics between the single forward propeller and the CRP configuration, with the objective of quantitatively demonstrating the efficiency benefits of the CRP system. 3.1 Comparison of Single Propeller Performance: EFD, CFD, and Potential Flow Analysis 3.1.1 Comparison of Single Propeller Performance Results Figure 5. Comparison of single forward propeller performance results from EFD, RANS and potential flow analysis. The performance results of the single propeller obtained from experimental fluid dynamics (EFD) tests conducted by Hyundai Heavy Industries were compared with those derived from CFD simulations and potential flow calculations. As shown in Figure 4, all three methods yielded closely aligned results and trends, with discrepancies within approximately 5%. This close agreement among the EFD, CFD, and potential flow results confirms the reliability of the numerical methods employed in this study. 3.1.2 Comparison of CRP System Propulsion Performance (POW) Results Figure 6. Comparison of CRP system propulsion performance (POW) results from EFD, CFD (RANS, LES), and potential flow analysis 9 As shown in Figure 6, when compared with the EFD results, the numerical analyses conducted using potential flow, RANS, and LES exhibited only minor discrepancies in the absolute values of thrust coefficient (𝐾𝑇) torque coefficient (𝐾𝑄), and efficiency (𝜂𝑂). However, the differences remained approximately 5%, and the overall agreement across the entire range of advance ratios was very good. Furthermore, the general trends obtained from each numerical approach were almost identical to those of the experimental results. These findings indicate that the numerical methods employed in this study provide reliable results, thereby ensuring sufficient validation for subsequent analyses of the wake flow field and vortex structure characteristics. 3.2 Comparison of CRP Wake Flow Structures: RANS and LES The wake flow structures of the CRP system were analyzed and compared based on simulations conducted using both RANS and LES approaches. In all cases, the flow fields were visualized using the nondimensional axial velocity component (𝑢/𝑈) as the reference parameter. (a) (b) Figure 7. Comparison of CRP wake flow structures from RANS and LES analysis, visualized by axial velocity 𝑢/𝑈 contours As shown in Figure 7, the comparison of CRP wake flow structures visualized by axial velocity (𝑢/𝑈) contours reveals distinct differences between the RANS and LES simulations. Figure 7(a) presents the results from the RANS simulation, where the wake flow exhibited a smoother and relatively simplified vortex structure as it progressed downstream. In contrast, Figure 7(b), which shows the LES simulation results, revealed more pronounced turbulent energy dispersion and finer vortex structures, representing a flow field that more closely resembles actual flow behavior. These observations indicate that the higher spatial and temporal resolution inherent to the LES approach enables the accurate capture of fine scale vortices within the wake, thereby allowing for a more detailed and realistic analysis of the wake flow structures. 3.3 Comparison of Propeller Flow and Wake Structures Using LES: Single Propeller vs. CRP System Based on the LES simulations, the wake flow structures of the single propeller and the contra-rotating propeller (CRP) system were compared and analyzed.