ABSTRACT
This study investigates the hydrodynamic performance of a high-speed planing craft from the Naples warped hard chine hull series using Computational Fluid Dynamics (CFD). Numerical simulations were performed by solving the Reynolds-Averaged Navier-Stokes (RANS) equations coupled with the k-ε turbulence model. A three-dimensional, unsteady, two-phase (air-water) turbulent flow was modeled. The vessel was simulated with two degrees of freedom (heave and pitch) to calculate resistance and trim. Dynamic meshing and a six-degree-of-freedom (6-DOF) rigid body solver were employed to couple the fluid flow with the vessel motion. Simulations were conducted for a Reynolds number greater than 3.5×10⁶ and a Froude number range of 0.52 to 1.65. The numerical results for resistance and trim were validated against existing experimental data, showing average errors of less than 3% and 9%, respectively. Additionally, the wave pattern and wake field behind the craft were analyzed at various speeds. The results confirm the high accuracy and capability of the RANS-based CFD method for hydrodynamic analysis of planing vessels.

1. INTRODUCTION
Over the past century, significant increases in the speed of transportation vehicles have been observed, except for commercial ships, where hydrodynamic resistance remains the primary limiting factor. This limitation is particularly severe for high-speed vessels. Planing craft operate in three distinct regimes: displacement, transition (semi-planing), and planing. In the planing mode, a significant portion of the vessel's weight is supported by hydrodynamic lift rather than hydrostatic buoyancy, leading to reduced wetted surface area and higher achievable speeds. Due to the complex, two-phase turbulent flow around planing hulls at high speeds, analytical solutions are impractical, and experimental methods are costly and limited. Consequently, Computational Fluid Dynamics (CFD) has emerged as an efficient and powerful tool for such analyses. Previous studies have applied RANS-based simulations to various planing craft configurations, including stepped hulls and tunnels, demonstrating the capability to predict resistance and trim. However, accurate
simulation requires careful consideration of dynamic mesh motion and free-surface capturing. This study aims to numerically investigate the hydrodynamic performance of a Naples-series planing craft using a dynamic meshing approach and two-degree-of-freedom motion, validating resistance and trim predictions against experimental data and analyzing the resulting wake and wave patterns.
2. MATERIALS AND METHODS
The fluid was assumed incompressible. The governing equations were the unsteady RANS equations for mass and momentum conservation. The standard k-ε turbulence model was employed to model the Reynolds stress tensor. The volume of fluid (VOF) method was used to capture the air-water interface.
The studied vessel is a planing craft from the Naples systematic series. Key principal dimensions include: length of 2.611 m, beam of 0.86 m, draft of 0.163 m, mass of 92.25 kg, and longitudinal center of gravity at 1.036 m. The computational domain was sized to prevent wave reflection: the outlet was placed 7.5 ship lengths downstream, and the water depth was 2.5 times the vessel length. A velocity inlet was specified at the inlet, and a pressure outlet at the downstream boundary. The craft was modeled as a symmetric half-body to reduce computational cost, with a symmetry plane applied at the centerline. A critical aspect of the methodology was the mesh strategy. Dynamic meshing was utilized to allow the vessel to move with heave and pitch (2-DOF). An overset mesh (or dynamic mesh region) was created around the hull, which moved with the vessel, while a background mesh remained stationary. To ensure high resolution of the free surface and wake, three refinement blocks with varying thicknesses were defined near the water surface. Additionally, three triangular blocks were placed behind the hull to capture the evolving wake pattern at different speeds. The final mesh consisted of approximately 991,671 cells after a grid independence study. Boundary layer resolution was ensured with eight prism layers around the hull. A time step of 0.001 seconds was selected following a time-step independence study. Simulations were performed using STAR-CCM+ 13.04 on a 16-core parallel processor.
3. RESULTS
The numerical results for total resistance were compared against experimental data for Froude numbers between 0.52 and 1.65 (speeds from 2.5 to 7.5 m/s). The results showed very good agreement. The average error was less than 3%, with a maximum error of 4.1% at the highest speed. The numerical simulation accurately captured the increasing trend of resistance with speed. The dynamic trim angle (the angle between the horizontal and the keel) was calculated at 11 different speeds. The results showed that trim increases with speed in the displacement and transition regimes, reaching a maximum at a Froude number of approximately 1.2. Beyond this point, in the full planing regime, the trim angle begins to decrease. Comparison with experimental data yielded an average error of 8.9%, confirming the capability of the dynamic mesh and 2-DOF approach to predict running attitude. Analysis of the wake field at speeds of 2.5, 4.5, and 7.5 m/s revealed that as speed increases, the wake becomes longer and narrower. The transverse wave length behind the hull increases while the width of the V-shaped wave pattern decreases. This is attributed to the increased velocity of the water jet exiting from under the transom, which concentrates the wake along the centerline. Visualization of the hull bottom at different speeds demonstrated a progressive reduction in the wetted surface area as speed increased. At the lowest speed (displacement mode), the wetted area was maximal. At the highest speed (planing mode), the wetted area was minimal, indicating that the hull is primarily supported by hydrodynamic lift, which reduces frictional resistance.
4. DISCUSSION AND CONCLUSION
This study successfully demonstrated the application of RANS-based CFD with dynamic meshing to predict the hydrodynamic performance of a Naples-series planing craft. The key conclusions are as follows:
1. The RANS numerical method coupled with the VOF multiphase model exhibits high capability in simulating the complex, two-phase turbulent flow around high-speed planing hulls.
2. Validation results confirmed that the average error for resistance prediction is below 3%, and for trim prediction is below 9%, indicating good engineering accuracy for practical applications.
3. The use of dynamic meshing and a two-degree-of-freedom (heave and pitch) motion is essential for accurately predicting the dynamic trim and equilibrium position of the vessel.
4. The simulation results effectively captured the physical trends of increased wake length and decreased wake width with increasing speed. The reduction in wetted surface area at higher speeds was also clearly visualized, explaining the reduction in resistance growth rate in the planing regime.
5. Future research should focus on extending this methodology to six-degree-of-freedom motions in irregular waves and investigating the effects of design modifications such as steps and spray rails.