Numerical Simulations and Experimental Tests for Tailored Tidal Turbine Design

Abstract

This paper outlines the design and testing of a horizontal-axis tidal turbine (HATT) at a scale of 1:20, employing numerical simulations and experimental validation. The design employed an in-house code based on the Blade Element Momentum (BEM) theory. As reliable lift and drag coefficients for this scale are not present in the literature due to the low Reynolds number of the airfoil, Computational Fluid Dynamics (CFD) simulations were conducted to generate accurate polar diagrams for the NACA 4412 airfoil. The turbine was then 3D-printed and the rotor tested in a subsonic wind tunnel at various fixed rotational speeds to determine the power coefficient. Fluid dynamic similarity was achieved by matching the Reynolds number and tip-speed ratio in air to their values in water. Three-dimensional CFD simulations were also performed, yielding turbine efficiency results that agreed fairly well with the experimental data. However, both the experimental and numerical simulation results indicated a higher power coefficient than that predicted by BEM theory. The CFD results revealed the presence of radial velocity components and vortex structures that could reduce flow separation. The BEM model does not capture these phenomena, which explains why the power coefficient detected by experiments and numerical simulations is larger than that predicted by the BEM theory.

1. Introduction

In recent decades, the disproportionate impact of fossil fuel combustion on climate change and human health has intensified global interest in renewable energy technologies. While solar and wind energy systems are currently the most advanced, marine energy technologies, including those based on tides, waves, and thermal and salinity gradients, are increasingly being explored to expand the portfolio of solutions required to achieve projected CO₂ emission reduction targets [1].

Among the various forms of marine energy, tidal energy represents the most mature technology, partly due to the adaptation of several technical features from the well-established wind energy sector. A key advantage of tidal energy is its greater predictability compared to wind energy, since it is primarily governed by astrophysical interactions within the Sun–Earth–Moon system. Typically, two high tides and two low tides occur daily. Nevertheless, meteorological disturbances may occasionally disrupt this regular cycle. Another significant benefit of tidal technology, compared to wind and solar, is its relatively low visual impact.

One of the main limitations of tidal energy is its geographic constraint: it can only be effectively harnessed in a limited number of locations worldwide. This is due to the need for coastal proximity and specific coastal and seabed configurations that allow the concentration of tidal energy within a confined area. Such conditions are typically found in narrow straits between closely spaced islands or in estuaries, where the contraction effect amplifies tidal flows. Additionally, tidal energy systems may interfere with existing marine activities such as shipping and fishing, making careful site selection and design essential, particularly near environmentally protected areas.

Tidal energy has been exploited for various purposes for centuries. Early implementations were rudimentary, consisting of tidal mills installed in channels where tidal currents flowed. Two main technological approaches are currently used to harness tidal energy. The first approach involves turbines placed directly in tidal currents to extract kinetic energy, without any additional infrastructure to guide or concentrate the flow. This system is known as a tidal stream generator, and the turbines are referred to as tidal stream turbines (TSTs). The second approach involves the use of a physical barrier to create a head difference between two sides of a structure. This head differential drives the turbines. Known as a tidal barrage, this system is typically employed in estuarine environments such as the well-known La Rance tidal power plant at the mouth of the La Rance River in France. However, tidal barrages often raise greater environmental concerns, as they can obstruct not only water flow but also the migration of aquatic organisms and the transport of sediments.

This paper focuses on tidal stream turbines, and in particular, on horizontal-axis tidal turbines (HATTs). The blade is the most critical component of a tidal turbine because its design largely determines how much power can be harnessed from the flow. The primary design objective is to achieve high efficiency across a broad range of flow conditions, which requires a high lift coefficient combined with a low drag coefficient.

Compared to wind turbines, tidal turbines are subject to significantly higher mechanical stresses due to the much greater density of water—approximately 800 times that of air. This necessitates a thicker blade profile near the root to ensure sufficient structural integrity [2]. To address this challenge, blade profiles originally developed for wind turbines, featuring relatively high thickness, are often adapted, provided they do not induce excessive suction-side pressure that could lead to cavitation. Over the past decades, several research institutions—including the National Renewable Energy Laboratory (NREL), the Risø National Laboratory for Sustainable Energy at the Technical University of Denmark, and Delft University of Technology—have contributed extensively to the development of airfoil profiles suitable for turbine blades [3]. These airfoils have been further refined by various researchers to enhance specific performance aspects. For instance, Coiro et al. [4] developed the GT1 hydrofoil based on the NREL series, achieving a high lift coefficient along with improved cavitation resistance. Goundar et al. [5] studied an alternative profile based on the S1210 airfoil, known as the HF-SX. Although this profile has a higher lift coefficient than the original, its drag coefficient is slightly higher. Again, Goundar et al. [6] introduced a new hydrofoil profile based on the HF10XX series for use at a specific site in Fiji. The resulting turbine has hydrofoils with a thickness that decreases linearly from the root to the tip, achieving a maximum power coefficient of 0.47. Grasso [7] used an algorithm of sequential quadratic programming to develop hydrofoils for tidal turbines, denoted as G-Hydra-A and G-Hydra-B. The latter in particular showed an improved efficiency when compared to the DU96-W-180 and NACA 4418 blade sections. A multipoint optimization applied to the base airfoil NACA 63815 was carried out by Luo et al. [8], resulting in an improved airfoil with a better lift–drag ratio and reduced susceptibility to cavitation. Singh et al. [9] combined two hydrofoils (S814 and DU91-W2-250) to obtain a new hydrofoil, denoted as MNU26, having good hydrodynamic characteristics.

The extensive literature on hydrofoil selection and optimization emphasizes the importance of choosing the right profile for a tailored tidal turbine design in order to maximize performance and minimize hydrodynamic issues. Aside from the specifics of the airfoils, which are beyond the scope of this work, the design and optimization of tidal turbine blades relies on Blade Element Momentum (BEM) theory for draft phases and Computational Fluid Dynamics (CFD) for fine-scale analysis, and optimization and validation through water tunnel experiments. For example, Batten et al. [3] provided an overview of the design procedure of a turbine using the NACA 63-8xx airfoil series, while Sale et al. [10] adapted a wind turbine optimization code for a stall-regulated tidal turbine rotor, coupling a genetic algorithm with BEM. Jia et al. [11] performed a CFD large-eddy simulation of a HATT to investigate how vortex generators could control the unsteadiness characteristics induced by turbulent flow. It was found that the selected vortex generators were able to reduce fluctuations due to unsteady hydrodynamics compared to smooth blades. De Jesus Henriques et al. [12] studied experimentally the effect of waves superimposed on a steady current to verify their hydrodynamic impact on the performance of a tidal turbine. Although the wave caused an oscillation of the power harnessed by the turbine, the averaged power remained to be unaffected. Hanzla and Banerjee [13] studied the impact of intense turbulence on a tidal turbine, demonstrating that rotor torque fluctuations increased by a factor of 4.8 compared to irrotational flow. This resulted in a decrease in the peak power coefficient.

This study focuses on designing a 1:20 scale model of a three-bladed HATT. The aim is to clearly streamline the design and testing methodology, which is based on integrating low-Reynolds-number polars derived from CFD, wind tunnel validation, and accurate 3D numerical simulations of the entire turbine. Wind tunnel validation was chosen, as setting up an experimental campaign in a wind tunnel is undoubtedly more practical than in water channels.

The NACA 4412 airfoil was chosen because of its good lifting properties and low drag coefficient. However, the hydrodynamic coefficients for this airfoil at the scale of the turbine could not be found in the literature. This is because the flow is characterized by low Reynolds numbers, for which reliable drag and lift coefficients are unavailable, partly because it is difficult to measure very low forces. Therefore, CFD simulations of the flow around the airfoil were carried out, exploiting the approach proposed by Mauro et al. [14], to estimate the drag and lift coefficients at the different operative Reynolds numbers and angles of attack (AoAs) of the rotor blades. After obtaining the hydrodynamic polars, the blade design was carried out using an in-house BEM code [15]. Then, a 3D CAD model of the rotor was generated and 3D-printed for testing in the wind tunnel, owned by the University of Catania, to determine its performance under fluid dynamic similarity conditions.

The turbine was simulated using the ANSYS Fluent CFD code. The resulting power coefficients were then compared with those obtained through wind tunnel experiments. The fairly good agreement between the numerical and experimental data confirmed the reliability of the methodology proposed. Additionally, the numerical simulation results revealed key flow phenomena not reproduced in the BEM model, such as stall delay, which impact turbine efficiency.

2. Materials and Methods

This section provides an overview of the Blade Element Momentum (BEM) theory and the Computational Fluid Dynamics (CFD) approach used in this study. It also describes the experimental facility setup.

The BEM is a computationally efficient method for analyzing the interaction between fluid flow and a turbine. Although much simpler than approaches based on the numerical solution of the Navier–Stokes equations, BEM provides sufficiently accurate results for most engineering applications. This makes it particularly suitable for fast-draft design and verification in off-design conditions.

The BEM theory combines two fundamental concepts: blade element and momentum theory. The turbine blade is divided into small annular rings, each of width dr. These rings collectively span the entire swept area of the rotor. The aerodynamic force acting on each segment is evaluated based on local flow conditions and local lift and drag coefficients. Momentum theory, on the other hand, applies the conservation of linear momentum to the stream tubes passing through each annular element. In this context, the rotor is modeled as a porous actuator disk that induces a pressure drop between its upstream and downstream sides. The freestream velocity far upstream is denoted by $U_0$ and the axial velocity at the actuator disk by $U_1$. Due to continuity, the axial velocity must remain constant across the disk, such that $U_1=U_1^{+}=U_1^{-}$, where the superscripts − and + denote the upstream and downstream faces of the actuator disk, respectively. According to Glauert’s formulation [16], the model consists of a system of equations linking the following dimensionless quantities:

$$a={\displaystyle \frac{U_0-U_1}{U_0}}, a^{\prime }={\displaystyle \frac{\omega }{2 \Omega }}, tan\left(\varphi \right)={\displaystyle \frac{1-a}{{\lambda }_r\left(1+a^{\prime }\right)}},$$

(1)

where $\Omega$ is the angular velocity of the rotor, ω is the angular velocity of the fluid induced by its interaction with the rotor, and $\varphi$ is the angle between the relative velocity and the plane of the rotor, with ${\lambda }_r$ defined as

$${\lambda }_r={\displaystyle \frac{\Omega r}{U_0}}.$$

(2)

In Equation (1), $a$ and $a^{\prime }$ are denoted as the axial and tangential induction coefficients, respectively, which depend on the radial position $r$. The force and torque acting on the annular ring are expressed using the force coefficients $C_l$ and $C_d$. These quantities are then equated to the force and torque obtained from the momentum and moment of momentum equations, thus yielding the following expressions for the induction coefficients:

$$a={\displaystyle \frac{\sigma C_N}{4Fsin{\left(\varphi \right)}^2+\sigma C_N}},$$

(3)

$$a^{\prime }={\displaystyle \frac{\sigma C_T}{4Fsin\left(\varphi \right)cos\left(\varphi \right)-\sigma C_T}},$$

(4)

where $\sigma$ is the solidity of the turbine, defined as $\sigma =c{N}_b/\left(2\pi r\right)$, $c$ is the chord, $N_b$ the number of blades, $C_N=C_{l}cos\left(\mathsf{\varphi }\right)+C_{d}sin\left(\mathsf{\varphi }\right)$, $C_T=C_{l}sin\left(\mathsf{\varphi }\right)-C_{d}cos\left(\mathsf{\varphi }\right)$, and $F$ is the Prandtl tip loss coefficient, which is given by

$$F={\displaystyle \frac{2}{\pi }}arccos\left[exp\left({\displaystyle \frac{N_b\left(r-R\right)}{2rsin\left(\varphi \right)}}\right)\right],$$

(5)

where $R$ is the radius of the turbine. It can be shown that the local thrust coefficient $C_{NN}$ of the axial force, $dN$, acting on the blade element of width, $dr$, defined as

$$C_{NN}={\displaystyle \frac{dN}{\frac{1}{2}\rho U_0^{2}2\pi rdr}},$$

(6)

is given by the expression $C_{NN}=4Fa\left(1-a\right)$ for $dN$, evaluated on the basis of the momentum equation. However, experimental data show that the thrust coefficient $C_{NN}$ follows the previous equation only for axial induction factors $a$ < 0.4. For $a$ > 0.4, the value of $C_{NN}$ exceeds the prediction of this equation, as the momentum theory is no longer valid under these conditions. A correction to account for this nonlinear behavior was proposed by Glauert [16]. However, when tip losses are included in the model (i.e., when the Prandtl tip loss factor $F$ < 1), Glauert’s correction introduces a numerical discontinuity in $C_{NN}.$ This discontinuity can lead to instability in the iterative solution of the BEM equations. To avoid this issue when tip losses must be considered, for $a>0.4$, it is recommended to use the alternative equation proposed by Buhl [17], which ensures numerical stability and continuity in the solution. This equation can be expressed as follows:

$$a={\displaystyle \frac{18F-20-3\sqrt{C_{NN}\left(50-36F\right)+12F\left(3F-4\right)}}{36F-50}},$$

(7)

where $C_{NN}$, determined using the Blade Element theory, is given by the following equation:

$$C_{NN}={\displaystyle \frac{U_1^2}{U_0^2{\mathrm{s}\mathrm{i}\mathrm{n}\left(\varphi \right)}^2}}\sigma \left[C_{l}cos\left(\varphi \right)+C_{d}sin\left(\varphi \right)\right].$$

(8)

An additional improvement has been made to the evaluation of the tangential induction coefficient $a^{\prime }$. The annular force is estimated using the conservation of energy flux between the upwind and downwind sides of the rotor, resulting in an expression containing $a^{\prime }$. Equating this expression with that of the normal force obtained from momentum theory yields the following expression [18]:

$$a^{\prime }={\displaystyle \frac{1}{2}}\left(\sqrt{1+{\displaystyle \frac{4}{{{\lambda }_r}^2}}a\left(1-a\right)}-1\right).$$

(9)

Equation (9) has been found to be more accurate than Equation (4), as demonstrated by a comparison with experimental data [15]. Therefore, Equation (9) has been used in the present application.

As concerns Computational Fluid Dynamics (CFD), it is known that it is extensively employed in a wide range of engineering and research applications as a valuable tool for supporting design, analysis, and optimization processes. Specifically, in the field of tidal and wind turbines, the adoption of three-dimensional CFD models provides a complementary approach to the preliminary design phase, typically based on one-dimensional models, by enabling the validation of their outcomes and offering a more accurate and detailed characterization of the fluid dynamic behavior. In this regard, M. Nachtane et al. [19], in their review, emphasized the fundamental contributions of CFD to the design and optimization of tidal turbines, as well as to the further analysis of specific issues affecting rotor performance. Li et al. [20] implemented CFD models to thoroughly analyze and evaluate the optimal design of a horizontal axis tidal current turbine blade. Alipour et al. [21] used a CFD approach based on the finite volume method, employing Ansys Fluent software, to investigate the effects of curvature, thickness, and blade pitch angle on an experimental tidal turbine.

In light of the findings reported in recent literature, and with the aim of preliminarily evaluating the performance and verifying the fluid dynamic behavior of the rotor designed using the in-house one-dimensional BEM code, a CFD model was implemented. The process begins with the creation of the 3D CAD geometry of the rotor using the twist and taper parameters obtained from the BEM design. The adopted methodology is grounded in the authors’ prior experience in the field of Horizontal Axis Wind Turbines (HAWTs) [22,23] and follows the CFD workflow provided by Ansys Fluent. Specifically, a suitable computational domain was generated in Ansys SpaceClaim 25_R1, which guaranteed optimal results in HAWT simulations. The dimensions and details of the computational domain, as well as the boundary types used, are shown in Figure 1.

The computational domain was divided into two coaxial cylinders: an inner cylinder and an outer cylinder. The inner cylinder contained the turbine and was rotated at turbine velocity in order to implement the steady Moving Reference Frame (MRF) model. This approach incorporates source terms into the momentum equations within the inner cylinder to account for rotational effects. Often referred to as the ‘frozen rotor’ approach, this steady-state method is widely validated in the literature [21,22,23] for simulating horizontal axis rotors under steady, controlled conditions. It offers an optimal compromise between accuracy and computational cost compared to unsteady sliding mesh models, which typically require significantly more CPU time to converge. Furthermore, the steady RANS approach coupled with the MRF model has proven capable of capturing essential time-averaged flow features, including those driven by local unsteadiness at low TSRs, while minimizing the impact on accuracy and reducing the computational cost.

The outer cylinder was used to apply the far-field boundary conditions.

The generation of the computational grid was carried out using the watertight workflow available in Ansys Fluent Meshing. The tool is equipped with advanced meshing algorithms capable of generating high-quality unstructured polyhedral meshes within a significantly reduced time frame, also benefiting from the possibility of parallel meshing across multiple CPU cores. Fluent meshing also provides full control over the grid refinement through local sizing functions to ensure proper resolution of geometrical and local flow features. In particular, a curvature size function was used to adequately refine leading edge regions, while different surface size functions were applied to control maximum cell dimensions on the blunt trailing edge, on the tip surfaces, on the root-to-hub geometrical transition region, and on the hub. A last-ratio inflation algorithm was utilized to ensure accurate resolution of the boundary layer with the height of the first mesh close to the body, having a thickness ${\delta }^{+}$ value always below 1.

A grid sensitivity study was carried out to minimize spatial discretization errors and to obtain an optimal compromise between accuracy and computational cost. Three grid refinement levels were compared across three tip-speed ratio (TSR) conditions: the minimum (0.56), the on-design (3.35), and the maximum ones (4.79). Details of the different grids are presented in

Table 1. Mesh details for the different grids used in the sensitivity study.

Mesh Details	Coarse	Ref-1	Ref-2
Curvature min size [mm]	0.08	0.04	0.02
Curvature max size [mm]	4	2	1
Curvature angle [deg]	12	12	12
Max face sizing hub [mm]	8	5	2.5
Max face sizing trailing edge [mm]	0.04	0.04	0.04
Max face sizing tip [mm]	0.1	0.1	0.1
First layer height (y+ ≈ 1) [mm]	0.02	0.02	0.02
Number of prism layers [-]	10	15	20
Minimum orthogonal quality	0.1	0.12	0.12
Cells count	8.4 M	11.3 M	24.9 M
Time to generate [min]	8	13	33

, while results of the independency study are shown in the chart of Figure 2. Here, the computed torque for the three TSRs is reported in logarithmic scale to better highlight the trends due to the large differences in the values, as a function of the number of cells correspondent to coarse, Ref-1, and Ref-2 grids reported in Table 1. The slight differences between the Ref-1 and Ref-2 grids (below 2%) for all TSR conditions demonstrate that the first mesh refinement represents an optimal compromise between accuracy and cell count. Therefore, all subsequent calculations were conducted using the Ref-1 grid. Qualitative details of the Ref-1 mesh are depicted in the image of Figure 3.

Due to the very low operative Reynolds numbers of the rotor (below 10⁵), the laminar to turbulent transition must be incorporated within the viscous model framework to adequately predict laminar bubbles and early separation phenomena.

For turbulence closure, the Generalized k-ω (GEKO) turbulence model [24] was used. This Ansys’ proprietary viscous model is based on the two-equation k-ω formulation and features four free coefficients, tunable within given limits without negative effect on the underlying calibration. The GEKO model provides the option of adding an intermittency transport equation to obtain a local correlation transition model [25]. The key advantage of the GEKO model is in its ability to adjust eddy viscosity (EV) within the boundary layer via the $C_{sep}$ coefficient, which is essential for controlling flow separation. In this work, the $C_{sep}$ coefficient was tuned according to a previous work by the authors [14].

The RANS Ansys Fluent pressure-based steady-state solver was utilized. According to the authors’ knowledge [4,5], the combination of the pseudo-transient advanced implicit under-relaxation formulation is an effective choice for the pressure–velocity coupling approach adopted in this study. This approach enhanced solver stability and robustness, leading to faster convergence.

A comprehensive report of the Ansys Fluent solver settings is reported in

Table 2. Solver settings and boundary conditions.

Inlet boundary conditions	Velocity inlet (0.5–6 m/s); TI = 0.1%; TVR = 10
Outlet boundary conditions	Pressure outlet, gauge pressure 0 Pa; TI = 1%; TVR = 10
Rotational speed	320 rpm
Fluid	Water (ρ = 998.2 kg/m3; μ = 0.001003 Pas)
Solver type	Incompressible, steady state, pressure based, pseudo-transient coupled solver
	Time-step method: automatic
	Length scale method: conservative
	Time scale factor = 1
Discretization methods	Least squares cell-based method for gradients
	Second order upwind discretization for convective terms
Rotation model	Moving Reference Frame (MRF)
Turbulence model	RANS Generalized k-ω + intermittency equation
Initialization method	Hybrid
Convergence criteria	Locally scaled residuals < 10−4, steady behavior of torque monitor
Time to convergence	<4 h (<800 iterations)

. Water with standard properties was used as fluid, while the flow speed at the inlet was set to cover a wide range of TSRs, from 0.56 to 6.7. The calculations were carried out on a Lenovo P620 workstation equipped with one CPU AMD Threadripper Pro W5995X with 64 physical cores for parallel computing and 512 Gb of RAM memory. Each simulation converged in less than 800 iterations, corresponding to computation time below 4 h.

To validate the numerical design methodology and the CFD analysis proposed, the rotor was extensively tested in the wind tunnel owned by the University of Catania. This was a closed-loop subsonic wind tunnel with a 0.5 × 0.5 × 1.2 m test section. The flow speed could be varied in the range 0–30 m/s, with a maximum turbulence intensity of 0.4%. More details are reported in [26]. Figure 4 shows an accurate representation of the wind tunnel layout alongside a photograph of it. The turbine model was installed at the center of the test section, mounted on a rigid support structure. The rotor was directly coupled to a brushless servomotor (Panasonic MADHT1505; nominal power: 50 W, manufacturer Panasonic Automation Control Division, Japan), which served both as an actuator and as a generator. The servomotor operated in closed-loop mode, enabling precise control of the rotational speed and real-time estimation of the torque via internal current feedback. The torque measurement range was ±0.16 Nm, with an associated expanded uncertainty of ±0.0092 Nm. Rotational speed was measured using an integrated encoder with a maximum operational limit of 6000 rpm and an uncertainty of ±6.92 rpm. The airflow velocity upstream of the rotor was measured using a hot-wire anemometer (VT 115), equipped with a stainless-steel probe (manufacturer of hot-wire anemometer and probe: Sauermann Group, Montpon-Ménestérol, France). This instrument provided instantaneous and averaged readings, automatically compensated for temperature and pressure. In the working range of 5–21 m/s, the extended uncertainty on the airflow velocity was estimated to be ±0.2 m/s.

Images of the rotor mounted on the test rig are presented in Figure 5.

A fixed turbine speed approach was adopted to assess the performance of the turbine. Three different rotational speeds were imposed (1500 rpm, 3000 rpm, and 4200 rpm), while the air stream velocity was varied in the range of 5–21 m/s to obtain different tip-speed ratios (TSRs). The experimental procedure consisted of the steps shown below.

• No-load torque measurement: The servomotor was operated without the turbine at fixed rotational speeds in the range of 500–5500 rpm to determine the torque required to overcome internal losses, including mechanical friction, bearing resistance, and viscous effects. The no-load torque curve was established as a function of rotational speed.
• Turbine testing: With the turbine coupled to the motor/generator, system torque measurements were performed at fixed rotational speeds while varying the air stream velocity.
• Determination of turbine torque: For each test condition (i.e., combination of motor speed and air velocity), the effective turbine torque was determined as the difference between the measured no-load torque and the load torque at a fixed turbine speed.
• Performance calculation: Based on the measured values of air velocity, turbine rotational speed, and torque, the power output as a function of air velocity was calculated. The turbine power coefficient $C_p$ and torque coefficient $C_q$ were then evaluated as functions of the TSR.

3. Results and Discussion

3.1. BEM Fluid Dynamic Design of the Rotor

BEM theory can be used to design a turbine by optimizing the twist and chord length of the blades, or to evaluate the performance of an existing configuration. An iterative approach is required in both cases due to the coupling between aerodynamic forces and induced velocities.

The process of designing a tidal turbine rotor is similar to that for wind turbines. As mentioned in the Introduction, selecting the appropriate airfoil for the blade requires particular care based on the operating conditions of the rotor, as it is not trivial. However, the general design methodology remains independent of the chosen hydrofoil profile. Instead, the design must be tailored to the desired outcome: either maximizing efficiency at a specific design flow condition or maximizing annual energy production based on the probability density function of tidal current speeds.

Thanks to its calculation speed, BEM codes allow the designer to easily and quickly address both the targets. In this work, the authors decided to design the blades to maximize the on-design rotor efficiency, which in turn resulted in ensuring a radial distribution of the local AoA on the blade, such as to maximize the lift to drag ratio in all the blade sections. Therefore, the starting point for such design is to collect airfoil polars for the operative Reynolds number ranges and to determine the AoA (${\alpha }_{max}$) which maximizes the lift-to-drag ratio.

The radius of the rotor was set to 0.1 m, which was the largest size that could be accommodated by the wind tunnel test section without causing a blockage in the airflow. Once the rotor dimensions have been defined, the most important aspect of designing small-scale turbines is the low Reynolds number value due to the small radius, as reliable data on lift and drag coefficients for airfoil profiles in these conditions is scarce in the literature. This is because, at low Reynolds numbers, the forces are small and difficult to measure without introducing large percentage errors. However, such data are essential for designing the turbine and for making a preliminary assessment of its efficiency using BEM. Therefore, a preliminary study was carried out using CFD to obtain airfoil polars for the operative range of Reynolds numbers of the blades. The methodology used is reported in the work of Mauro et al. [14]. In this study, the numerical results were compared with the experimental measurements of Reuss et al., 1995 [27] and with the experimental results of Somers et al., 1997 [28]. Fairly good agreements were obtained between the CFD results and the abovementioned experimental data. Although these literature results were characterized by a higher Reynolds number (Re = 10⁶) than the present numerical simulations, the fairly good agreement gives us confidence in the correctness of the adopted numerical procedure and of the polars computed in the present study. The reliability of the CFD approach used to simulate the entire turbine, as shown in the following, can provide further evidence to support the accuracy of the polars, given that this approach is analogous to that used for the 2D numerical simulations aimed at obtaining the polars.

The CFD simulation results for the NACA 4412 airfoil at Reynolds numbers of 5 × 10⁴, 7.5 × 10⁴, and 10⁵ are plotted in Figure 6. As can be seen, the trends in lift and drag coefficients as a function of angle of attack are very similar for all three cases. In particular, the lift coefficient exhibits significant nonlinear behavior due to the effect of the low Reynolds number, which induces flow separation bubbles. The curve at a Reynolds number of 7.5 × 10⁴ has been selected for the design. This is justified by the observation that, for the TSR giving rise to the maximum of the power coefficient, the Reynolds number of the blade varies from 5.7 × 10⁴ near the hub to 7.5 × 10⁴ at the blade tip.

The angle of attack ${\alpha }_{max}$, which gives the maximum ratio between the lift and drag coefficients, has been found to be 4°, corresponding to the force coefficients $C_l$ = 0.71 and $C_d$ = 0.042. Regarding the radial distribution of the chord $c$, Equation (10) was used [29]:

$$c\left(r\right)={\displaystyle \frac{1}{N_b}}{\displaystyle \frac{16\pi \mathrm{r}}{{\mathrm{C}}_{\mathrm{l}}}}{\left[\mathrm{s}\mathrm{i}\mathrm{n}\left({\displaystyle \frac{{\varphi }_1}{3}}\right)\right]}^2, {\varphi }_1=\mathrm{atan}\left({\displaystyle \frac{1}{{\lambda }_r}}\right),$$

(10)

where ${\varphi }_1$ is the angle between the relative velocity and the plane of the rotor. Then, twist angle ${\theta }_1$ is given by

$${\theta }_1\left(r\right)={\varphi }_1\left(r\right)-{\alpha }_{max}.$$

(11)

These formulae were derived by maximizing the power coefficient, taking into account the effect of wake rotation but disregarding drag and tip losses. Due to these limitations, it cannot be guaranteed that these equations maximize the power coefficient. We investigated whether a more efficient turbine configuration than that obtained using Equations (10) and (11) can be obtained by using Equation (10) so to determine the chord distribution, and the BEM model to calculate the angle $\varphi$ between the relative velocity and the rotor plane, so that the twist angle $\theta$ of the blade is given by

$$\theta \left(r\right)=\varphi \left(r\right)-{\alpha }_{max}$$

(12)

Although this approach is empirical, we found that it improves the power coefficient of the turbine compared to using Equations (10) and (11) to determine both c(r) and the twist angle. In fact, using the BEM model to compute the power coefficient, the turbine designed using the present approach has a maximum $C_p$ of 0.32, whereas that designed using Equations (10) and (11) for the chord and the twist angle has a maximum $C_p$ of 0.24. This is why we ultimately opted for this procedure to design the blades.

Therefore, according to the adopted procedure, the distribution of the chord is determined outside the BEM code, while the relative flow angle $\varphi$, the twist angle $\theta$, and the induction coefficients are calculated using the BEM code, with the force coefficients assuming the values that maximize their ratio. Further details of the procedure can be found in reference [15].

The design water flow speed is 1 m/s, which is typical of tidal currents. After several applications of the BEM code, it was found that the maximum power coefficient was achieved at a rotational speed of 320 RPM.

Figure 7 shows the radial distribution of the twist angle and the chord obtained using the proposed BEM design. The rotor was then reproduced in CAD and 3D-printed in PLA for testing in a wind tunnel. Figure 8 shows the CAD model in STL format and the 3D-printed rotor.

3.2. Comparison Between Experimental and CFD Results

As mentioned previously, the wind tunnel tests were performed under conditions of fluid dynamic similarity between water and air. Although the application of the similarity principle to wind tunnel experiments has several precedents, we provide a brief overview of how this similarity was imposed for the sake of completeness. However, it is worth noting beforehand that this study considers turbine efficiency in an unbounded fluid. In this context, the most significant dimensionless parameters are the Reynolds number and the tip-speed ratio. The Froude number may also be important if the fluid boundary includes a free surface. However, there are several cases in which, despite the presence of a free surface, the Froude number is irrelevant. To understand why this occurs, it is helpful to consider that the blockage ratio is typically the first parameter evaluated when assessing the influence of the boundary. This is defined as the ratio of the area swept by the rotor to the total cross-sectional area. Previous studies [30] have shown that, for a blockage ratio of less than 20%, the power coefficient is not significantly dependent on the Froude number based on the turbine diameter or the water depth. Similarly, it is not significantly dependent on the ratio of the hub depth to the turbine diameter. For a blockage ratio greater than 20%, however, there could be an effect of the Froude number, which should be considered in addition to the Reynolds number. The Froude number may also be relevant in cases of significant density stratification, which can lead to internal waves in the sea. However, this does not happen often or severely enough to be considered a significant factor. Therefore, the dimensionless parameters that most often play a role in the fluid dynamics of a turbine are the Reynolds number and the tip-speed ratio. This demonstrates that the present study can be applied to turbines operating in water, given that the Froude number is not always significant. However, we acknowledge that failing to investigate the effect of the free surface is a limitation of the present study, as it could be important in certain situations.

Starting from the on-design conditions in water, the similarity in air was obtained through the following reasoning. By imposing Reynolds number equality, and being $U_w$ and $U_a$ for the water and air velocity, respectively, and ${\nu }_w$ and ${\nu }_a$ for the water and air kinematic viscosity, we obtain the following:

$${\displaystyle \frac{U_{w}c}{{\mathrm{\nu }}_w}}={\displaystyle \frac{U_{a}c}{{\mathrm{\nu }}_a}},$$

(13)

where $c$ is the chord at a generic radial position. Therefore, the velocity ratio must be equal to the kinematic viscosity ratio, as follows:

$${\displaystyle \frac{U_a}{U_w}}={\displaystyle \frac{{\mathrm{\nu }}_a}{{\mathrm{\nu }}_w}}.$$

(14)

Considering the dynamic viscosity and density of air and water, imposing the TSR equality and being the actual design conditions in water, $U_w$ = 1 m/s and 320 rpm, the similarity in air leads to $U_a$ = 13.2 m/s and 4200 rpm. Tests and CFD simulations were therefore carried out at a fixed rotational speed of 4200 rpm and by varying the flow speed in such a way to cover a wide range of TSRs. Then, rotational speeds of 1500 and 3000 rpm were tested as well to evaluate the influence of the rotational speed on the rotor performance and to explore a wide range of operating conditions. For the same reason, a further set of CFD simulations were performed at 3000 rpm.

Preliminarily, since the numerical simulation setup discussed previously was studied for water flow, it was checked whether it was also appropriate for air flow under the imposed similarity condition. Figure 9 shows a comparison of the power coefficient obtained at 320 rpm using water and at 4200 rpm using air under the imposed similarity condition. As can be seen, CFD produces the same result in both cases.

The wide set of data, including the results obtained with the BEM code, are compared in the charts of Figure 10, where power and torque coefficients are reported as a function of TSR. Also shown are data from the experiments conducted by Doman et al. (2015) [31] and Seo et al. (2016) [32] on small-scale turbines using water as the working fluid. A fairly good agreement is observed between the present experimental results and the numerical CFD simulations, particularly at low TSRs.

At higher TSR values, however, the experimental data exhibit greater dispersion, as highlighted by the large error bars, likely due to the increased relative error in torque measurements at low torque levels, which is related to the lower limit of accuracy of the electric motor–generator. In fact, higher TSRs at fixed rotational speed were achieved by reducing the air velocity, which consequently decreased the torque produced by the turbine.

The uncertainty in the experimental measurement of the $C_p$ value is estimated to be ±4% for a TSR of around 3 and ±20% for a TSR greater than 5. Therefore, the experiments do not provide reliable information for TSR values greater than 5. At low TSRs, the measurement uncertainty is very small, resulting in a high level of agreement between the results obtained at 1500 and 3000 rpm. For this reason, no error bars are shown for 1500 rpm and low TSR values at 3000 rpm in Figure 10.

Figure 10 also shows the power and torque coefficients obtained using the BEM theory. As can be seen, the BEM results differ significantly from those obtained through experimentation and CFD. The only area of agreement is the TSR value, at which the maximum value of the coefficients are attained. Generally, the BEM theory computes smaller power coefficients than the actual value, except for very large TSRs. This is due to the rotational effect, which significantly alters the hydrodynamic behavior of the blade profile compared to a non-rotating case. Indeed, the rotational effect can reduce the extent of flow separation on the suction side of the blade, resulting in an increased lift coefficient and a decreased drag coefficient compared to the 2D case used in the BEM model. This phenomenon is known as centrifugal pumping or stall delay, which is typically associated with rotating blades. The present authors have demonstrated this phenomenon in [23], where the values of $C_l$ and $C_d$ were determined using 3D CFD simulations. Specifically, determining the force coefficients as in [23] requires the blade to be split into several elements, and the 3D CFD simulations of the entire turbine to be run while the forces acting on these elements are stored. The 3D induction and lift/drag coefficients can then be obtained using an inverse blade element momentum model. In light of the in-depth analysis carried out in the aforementioned study, the underestimation of the BEM model appears to be due to its inadequacy in considering the effect of rotational augmentation.

Figure 10 confirms the effectiveness of the proposed design methodology. According to the CFD results, the efficiency of the rotor exceeds 40% for a fairly wide range of TSRs (2.5 < TSR < 4) and 30% for TSRs between 2 and 5. Furthermore, Figure 10 supports the validity of the implemented CFD model, which can therefore be reliably used to gain deeper insight into the fluid dynamics of the tidal rotor, to support future design optimizations, or to scale the system up to real-scale applications without the need for complex and costly full-scale experimental testing.

Figure 10 also shows, for comparison, the results of testing in water two other small-scale turbines reported in the literature. The three-blade turbine tested by Doman et al., 2015 [31] has a radius of 0.381 m, with the blades made up by of the NREL S814 hydrofoil. The tests were carried out at a fluid velocity of 1 m/s and a rotational velocity ranging from 67 to 161 rpm. The turbine tested by Seo et al., 2016 [32] has a radius of 0.2 m; its blade cross-section profile uses the NACA 63-418 hydrofoil. Tests on this turbine were carried out at a fluid velocity of 1.436 m/s and a rotational velocity of 240 rpm. Figure 10 shows that the tip-speed ratio at which the maximum $C_p$ value is achieved is similar for all the considered turbines. The high TSR value at which the power coefficient turns negative is also comparable between the turbine in [31] and in the present turbine. Naturally, the exact $C_p$ values differ due to the different hydrofoils employed. While it is not claimed that the present turbine is the best possible design, the comparison shows that it is generally more efficient than the other two. Only in the high-TSR range does the turbine in [31] have a higher power coefficient than the current design; the turbine in [32], however, always has a lower coefficient.

3.3. Analysis of the CFD Results

This section uses CFD results to analyze the complex 3D flow around the turbine rotor. This provides insights into the flow field and vortex structure, which affect the efficiency of the rotor. Specifically, Figure 11 shows the local flow field at different radial blade sections in terms of relative velocity vectors for three significant TSRs.

At large tip-speed ratios (TSR = 4.79), the flow appears well aligned with the chordwise direction, indicating a radial distribution of relatively low AoAs, corresponding to a low-load condition. Under on-design conditions (TSR = 3.35), the blade exhibits an optimal pitch of approximately 5–6° along its span. No flow separation regions are observed, confirming the effectiveness of the blade twist distribution obtained using the BEM code, by imposing the maximization of the $C_l/C_d$ ratio. The behavior at lower TSR values (TSR 1.68 in this example) proves particularly interesting. At such high inflow velocities (2 m/s), the AoA should theoretically lead to large portions of the blade experiencing stall conditions, resulting in extended regions of flow separation. However, this phenomenon is observed only at r = 95% in Figure 11, i.e., near the blade tip. At r = 25% and r = 60%, the flow remained largely attached, with only very limited separation regions visible. This behavior is clearly linked to the 3D effects induced by blade rotation, as previously discussed, and, for TSR = 1.68, results in an 80% increase in the power coefficient compared to that provided by the BEM model. However, the rotational effect is not only evident at low TSRs, but across most of the analyzed range, as can be seen in Figure 10.

Figure 12 corroborates this analysis, which considers the rotational effect. In all cases, Figure 12 shows a certain radial flow component along the blade span. At medium and high TSR, this flow consists primarily of a weak radial motion confined to the boundary layer. In contrast, at lower TSRs, a centrifugal vortex develops, which effectively entrains the boundary layer, thereby maintaining flow attachment even in regions where, due to the high angles of attack, flow separation would otherwise be expected. This leads to a substantial pressure drop on the suction side of the blade, particularly at low TSR, due to the development of an intense helical vortex.

Since these phenomena affect the force distribution along the blade in ways that differ from the predictions of the 1D BEM theory, they must be carefully considered in the aeroelastic design of the blades.

To demonstrate that the swirling streamlines generated by the centrifugal effects depicted in Figure 12 consist of vortex structures, the $Q$-criterion is employed [33], whereby vortex structures are localized in the regions where the second invariant of the velocity gradient tensor $Q$ is positive. Figure 13 shows the isosurfaces of $Q$ = 100 s⁻² on the leeward side of the turbine for values of TSR equal to 1.68, 3.35 and 4.79. The isosurface is colored according to the helicity density values obtained by taking the scalar product of vorticity and velocity.

For all TSRs, the $Q$-criterion indicates that vortices are shed from the blade tips and are arranged concentrically around the turbine rotor. In addition, three root vortices emerge around the turbine hub. For large TSRs, no vortices are observed on the leeward side of the blades for most of their extension. On the other hand, for TSR = 1.68, there is a wide region on the lee side of the blade affected by vortices. The helicity density is particularly high in this region (see the blue areas), suggesting that the streamline entanglement shown in Figure 12 for TSR = 1.68 corresponds to a vortex with a high helicity density.

4. Conclusions

This work presents a comprehensive methodology for the design, numerical modeling, and experimental validation of a small-scale horizontal-axis tidal turbine (HATT). This methodology is based on low-Reynolds-number polars derived from CFD, wind tunnel validation, and accurate 3D numerical simulations of the entire turbine. The main findings and contributions of the study can be summarized as shown below.

• A tailored design methodology was implemented using a fast in-house BEM code, enabling efficient optimization of blade geometry.
• A CFD-based approach was employed to estimate aerodynamic coefficients for the NACA 4412 airfoil in the low-Re regime, addressing the lack of reliable data in the literature for small-scale tidal applications.
• Three-dimensional numerical simulations using Ansys Fluent provided insight into complex flow features, such as stall delay and centrifugal pumping, which are not captured by one-dimensional models.
• Experimental tests were performed in a wind tunnel under fluid dynamic similarity conditions, allowing for a direct comparison with CFD results and confirming the efficiency of the rotor over a wide range of TSRs.
• A fairly good agreement was found between experiments and CFD simulations, particularly in the low-TSR range.
• The BEM results show lower power and torque coefficients than the experimental and CFD results, primarily due to centrifugal pumping. However, there is agreement on the TSR value at which the maximum coefficient values are attained.
• The study demonstrates also the potential of wind tunnel testing as a practical and reliable alternative to water flume testing for small-scale tidal turbine prototypes.

This work provides a validated framework that can be used for future design optimizations and scaled-up tidal turbine development, while significantly reducing the need for complex and expensive full-scale experimental campaigns.