^{1}

^{1}

^{*}

The principal objective of this work was to investigate the 3D flow field around a multi-bladed horizontal axis wind turbine (HAWT) rotor and to investigate its performance characteristics. The aerodynamic performance of this novel rotor design was evaluated by means of a Computational Fluid Dynamics commercial package. The Reynolds Averaged Navier-Stokes (RANS) equations were selected to model the physics of the incompressible Newtonian fluid around the blades. The Shear Stress Transport (SST)
*k*-
*ω* turbulence model was chosen for the assessment of the 3D flow behavior as it had widely used in other HAWT studies. The pressure-based simulation was done on a model representing one-ninth of the rotor using a 40-degree periodicity in a single moving reference frame system. Analyzing the wake flow behavior over a wide range of wind speeds provided a clear vision of this novel rotor configuration. From the analysis, it was determined that the flow becomes accelerated in outer wake region downstream of the rotor and by placing a multi-bladed rotor with a larger diameter behind the forward rotor resulted in an acceleration of this wake flow which resulted in an increase the overall power output of the wind machine.

The escalation of the global energy demand has led countries to consider renewable energy sources more seriously. In the 2019 released version of the International Energy Outlook, the U.S. Energy Information Administration projects that the world energy consumption will grow by nearly 50% between 2018 and 2050 [

Over the past two decades, the traditional experimental methods of studying wind turbine fluid dynamics have decreased [

The work presented in this paper is a numerical study of the flow characteristics around a multi-bladed rotor wind turbine, a novel concept patented by the Thunderbird Power Corp [

A high-solidity windmill generates more torque at low-tip speeds compared to a modern horizontal axis wind turbine [

the torque and power outputs of the wind turbine with different rotational speeds and varying wind velocities. In order to evaluate the proper location of the subsequent rotors, velocity profiles of the rotor wake were thoroughly investigated.

Fluid motion can be described by a set of differential equations, namely the mass and momentum conservation equations, known widely as Navier-Stokes Equations (NSE). In the absence of gravity, for an incompressible Newtonian fluid, the NSE reads as Equations (1) and (2), respectively.

∂ U i ∂ x i = 0 , (1)

∂ U i ∂ t + U j ∂ U i ∂ x j = − 1 ρ ∂ P ∂ x i + ν ∂ 2 U i ∂ x j ∂ x j + F i ρ , (2)

where x i denotes the position vector, ρ stands for the fluid density, P is the pressure, U is the fluid velocity and ν is the kinematic viscosity. External body forces, denoted by F, act on a section of the fluid and were evaluated from the fluid rotational forces, such as the Coriolis and centrifugal forces. Osborne Reynolds developed a proposal for eliminating the turbulence unsteady fluctuations by averaging the flow quantities which lead to the so-called Reynolds Averaged Navier-Stokes (RANS) equations for the mean flow, Equations (3) and (4).

∇ ⋅ u = 0 (3)

∂ u ∂ t + ( u ⋅ ∇ ) u = − 1 ρ ∇ p e f f + ν ∇ 2 u − 2 Ω × u − ∇ ⋅ u ′ u ′ ¯ (4)

The stress tensor term in the momentum equation (Equation (4)), u ′ u ′ ¯ , corresponds to the effects of turbulence on the mean flow and results in a closure problem in the RANS equations. The semi-empirical standard k-ε model introduces two equations (Equations (5) and (6)), involving turbulent kinetic energy, k, and turbulent dissipation, ε, to RANS which closes the system.

∂ ∂ t ( ρ k ) + ∂ ∂ x i ( ρ k u i ) = ∂ ∂ x j [ ( μ + μ t σ k ) ∂ k ∂ x j ] + P − ρ ε (5)

∂ ∂ t ( ρ ε ) + ∂ ∂ x i ( ρ ε u i ) = ∂ ∂ x j [ ( μ + μ t σ ε ) ∂ ε ∂ x j ] + C 1 ε ε k P − C 2 ε ρ ε 2 k (6)

P is the production of k, μ t is the eddy-viscosity and are defined respectively as in Equations (7) and (8),

P = − ρ u ′ i u ′ j ¯ ∂ u j ∂ x i , (7)

μ t = ρ C μ k 2 ε (8)

The k-ε model assumes the flow to be fully turbulent and is reliable for high Reynolds regions only. The k-ω model, on the other hand, utilizes the transport equations for k (Equation (9)) and turbulence frequency, ω (Equation (10)), to solve the turbulent viscosity.

∂ ∂ t ( ρ k ) + ∂ ∂ x i ( ρ k u i ) = ∂ ∂ x j [ ( μ + μ t σ k ) ∂ k ∂ x j ] + G k − Y k + S k , (9)

∂ ∂ t ( ρ ω ) + ∂ ∂ x i ( ρ ω u i ) = ∂ ∂ x j [ ( μ + μ t σ ω ) ∂ ω ∂ x j ] + G ω − Y ω + S ω , (10)

where G is for the production terms, Y the dissipation and S represents the user-defined source expressions. The k-ω model showed better agreements with the real flow behavior for the viscous sublayer regions and hence was chosen over the k-ε model. Coupling the k-ε and k-ω models with a blending function introduces the k-ω Shear Stress Transport (SST) model [

For the rotating fluid domains, such as flow around rotating blades and impellers, it was possible to simulate the unsteady nature of the problem in a steady-state manner, where the mesh motion was such that it followed the motion of the geometry. This approach was more time efficient compared to the unsteady analysis and reduced the amount of computational power needed and was a good method for conducting preliminary studies of turbomachinery problems. In this study, a steady-state Single Moving Reference Frame (SRF) method was utilized to analyze the flow domain where the RANS equations, (Equations (3) and (4)) were solved in a rotating frame of reference to simulate the steady-state condition and an additional source term was applied to the flow equations throughout the domain. The equations of energy, momentum, continuity and transport of species were solved in a segregated manner based on pressure-based solver algorithm which was ideal for incompressible flows and resulted in memory and time efficiencies.

In the present study, a simplified version of the original patented multi-bladed rotor was modeled by a SOILDWORKS CAD package. Since the blades were evenly placed around the rotor at 40 degree intervals, one-ninth of the whole rotor was chosen to be studied and the effects of the remaining blades were taken into account through applying a periodic boundary condition where it was required. Analyzing the effects of other parts of the wind turbine, including the hub, tower and arms was beyond the scope of this work. For the current design the rotor diameter was set to 3.5 ft and it consisted of 18 identical sail with each of them have a length of 6.3 inches.

Defining a domain to any problem introduces errors to the flow solution as the boundaries should naturally be at an infinite distance from the object. However, this distance was limited in practice. The dimensions of computational domain must be large enough to predict the turbulence phenomenon, pressure and velocity distribution to a reasonable degree. For this study, the domain was a single rotatory region where the free stream flow entered the flow domain at a distance of 1.5 L upstream of the rotor and exited 2 L distance downstream of the rotor, where L stands for length of the sail. The entire domain was one-ninth of a cylinder with a diameter of 1.3 D, with D being the rotor diameter. The geometry of computational fluid domain is illustrated in

Considering the rotation of the rotor in the clockwise direction, the frame motion was activated in the model setup with its axis of rotation being set in the flow direction, rotating as the negative of rotational velocity of the rotor. The inlet velocity boundary condition was used for the upstream surface of the domain by changing the magnitude of the wind velocity. The downstream surface boundary condition was set to be the outlet gauge pressure. As the upper and lower surfaces of the computational domain had no impact on the flow solution, they were adjusted as symmetry boundaries. Periodic boundary conditions were used for the side surfaces as the crossing flow from these faces are identical with each other. Lastly, the surface around the sails were set to no-slip boundaries. The turbulence intensity and viscosity ratio remained as software defaults at 5% and 10%, respectively.

The governing equations, Equations (3) and (4), were solved in the rotating frame of reference at the same speed as the rotor rpm. The fluid domain was discretized into approximately 440 thousands cells using the meshing software included in the ANSYS Fluent package. The solution to the problem reached to a stable condition for this number of elements and this behavior was shown in the grid independency study (

Fluid | Air |
---|---|

Constant Temperature | 298.15 [K] |

Constant Density | 1.18415 [kg/m^{3}] |

Constant Dynamic Viscosity (μ) | 1.85508e-5 [kg/ms] |

Reference Pressure | 101,325 [Pa] |

Flow conditions | Steady state |
---|---|

Scheme | Coupled |

Gradient | Least Square Cell Based |

Pressure | Standard |

Momentum | Second Order Upwind |

Turbulent Kinetic Energy | First Order Upwind |

Specific Dissipation Rate | First Order Upwind |

For this analysis, the incoming free flow was parallel to the ground in the negative Z direction. Flow visualizations were done with four different wind velocities of 5, 10, 15 and 25 MPH which convert into approximately 2.2, 4.5, 6.7 and 11 m/s. The tip speed ratio of the turbine was kept constant at 0.7 which historically results in the highest achievable power coefficient for the American multi-bladed horizontal axis wind turbine. Sectional torque for each case was attained and was multiplied by factor of 9 to get the overall rotor torque, as the simulations were done through a one-ninth portion of the rotor. The rotor power was calculated by multiplying the torque value with the rotational speed of the rotor.

For a better understanding of the flow behavior in the wake region, several planes in parallel and perpendicular positions to the axis of rotation were created. The parallel plane was placed along the periodic surface of the computational domain, covering an axial distance of 3.5 L. Three perpendicular planes were assigned at distances of 0.4 L, 0.75 L and 1.25 L behind the rotor plane, as shown in

Figures 11-14 illustrate the axial flow characteristics of the wake behind the rotor at wind speeds of 5, 10, 15 and 25 MPH, respectively. The regions with highest axial velocities are circled with white color for the first set of incoming velocities.

As observed in the above figures, it was evident that there was a consistent flow behavior for all cases where the axial flow velocity increased in the outer regions behind each rotor sail, which was an expected trend as a result of the disk rotation. This increase in axial velocity tended to decrease as the flow traveled further downstream from the rotor. The drop in the axial velocity magnitude in the rotor disk’s shadow regions resulted due to the rotor power extraction from the free flow. The low velocity wake flow also recovered at far distances downstream from the rotor plane.

By studying the pressure contours on the blade surface it showed that the surfaces which face the wind have higher pressure magnitudes compared to the rear surfaces, as expected. This pressure difference between both sides of the rotor sails caused lift in the direction of the rotor rotation. A closer look at the pressure-side of the blade showed the front edges, which are facing in the direction of rotation, have a higher pressure with respect to rest of the sail surface. However, the opposite holds true for the suction side of sails where the edges that faced the rotation direction are the regions with lower pressure. In

As mentioned earlier, the tip speed ratio throughout this analysis was kept at a fixed value of 0.7 and, therefore, the rotational speed increases linearly as the oncoming wind velocity increases. This behavior is shown in

Considering the limitations in maximum cell number of the fluid solver’s Academic Teaching license, the grid independency analysis was carried out to study the stability of the main output of the flow solution for the chosen number of mesh elements. It was showed that the fluctuations of the sectional torque were very minor for cell number of around 400,000 (

Considering the novelty of the evaluated rotor design, there was no available experimental data to be compared with the calculated result. However, the reported values for power coefficient in

A high-solidity windmill generates more torque at low-tip speeds compared to modern horizontal axis wind turbines [

A more comprehensive study analyzing the effects of varying the number of blades, varying the sail geometries and evaluating the addition of rotors should be conducted. Considering the deficiencies of applying the steady-state modeling approach for flows with an unsteady nature, a study to apply an unsteady simulation algorithm in order to better evaluate different performance behaviors should be considered.

The authors declare no conflicts of interest regarding the publication of this paper.

Mamaghani, N.A. and Jenkins, P.E. (2020) Computational Fluid Dynamics Analysis of Multi-Bladed Horizontal Axis Wind Turbine Rotor. World Journal of Mechanics, 10, 121-138. https://doi.org/10.4236/wjm.2020.109009