**4. Computational fluid dynamics of a Darrieus hydrokinetic turbine**

A computational domain is a region in the space in which the numerical equations of the fluid flow are solved by CFD. In order to solve the physics of the flow field around the blade, dividing the flow domain in a set of small subdomains (rotating and stationary domains) is required, which implies the generation of a mesh of cells, also defined as control volumes. Three fundamental aspects to evaluate the accuracy and the resolution time of a simulation are the geometry and size of the cells coupled to the numerical method used to solve the governing equations. The mesh size must be sufficiently small to provide an accurate numerical approximation, but it cannot be so small that the solution is impractical to be obtained with the available computational resource. Thus, the mesh is usually refined in the regions of interest around the main obstacles affecting the flow [83]. In the particular case of the vertical axis hydrokinetic turbines, these obstacles are the blades.

The mesh can be structured or unstructured. In the first case, the mesh consists of quadrilateral cells in 2D or hexahedral cells in 3D. In turn, the unstructured mesh usually consists of triangles in 2D and tetrahedral in 3D, but cells of the mesh can adopt any form. Structured mesh usually implies shorter time resolution; nevertheless, the unstructured meshes may better represent the geometry. Yasushi [84] presents a discussion about the development of efficient computational analysis using unstructured mesh. On the other hand, Luo and Spiegel [85] propose a

#### *Computational Fluid Dynamic Simulation of Vertical Axis Hydrokinetic Turbines DOI: http://dx.doi.org/10.5772/intechopen.89184*

method to generate a hybrid mesh (coupling structured and unstructured mesh). In some occasions, the hybrid meshes consist of quadrilateral or hexahedral elements generated in layers near the wall surfaces to capture the boundary layer and of triangular or tetrahedral elements that fill the remainder of the domain. Several concepts related to mesh generation are found in [86], and a detailed discussion about the influence of the mesh in CFD applications is presented by Thompson et al. [83].

The CFD package, ANSYS Fluent version 18.0, was used for all the simulations performed in this study. 2DCFD model with less computational cost than 3D model was utilized to represent the vertical hydrokinetic turbine and the water domain. Based on the review of relevant works [78, 87–89], the use of a 2D model has been reported to be enough for revealing the factors that influence the performance of the turbine and the majority of factors affecting the flow physics surrounding the vertical axis hydrokinetic turbine, such as the hydrofoil profile, *B*, *σ*, and *D*. In the 2D numerical study of this work, the effects from supporting arms were not taken into consideration. URANS equations were solved using the SIMPLE algorithm for pressure velocity coupling [34, 37, 90, 91].

The vertical hydrokinetic turbine studied was a three-bladed Darrieus rotor with a NACA 0025 blade profile. *c* was set at 0.33 m with *R* equal to 0.75 m. And central axis with a *D* of 0.025 m was placed in the rotation axis. As previously discussed, the mesh is a critical part of a CFD simulation for engineering purposes. It has to be coarse enough so that the calculation is affordable but also fine enough so that each important physical phenomenon is captured and simulated. In this sense, the domain mesh was created around each hydrofoil, and the surrounding water channel geometry was defined based on studies of the boundary extents. There is an inner circular rotating domain connected to a stationary rectangular domain via a sliding interface boundary condition that conserves both mass and momentum. The domain extents were also selected from a series of sensitivity tests to determine the appropriate distance of the walls, inlet and outlet boundaries from the *R* rotor. The domain extends three upstream and 8*R* downstream of the center of the turbine and two 5*R* laterally to either side of the turbine. The circular rotating domain has an overall diameter of two 8*R*. Because the computational domain is 2D, the turbine blades were implicitly assumed to be infinitely long.

Unstructured meshes were applied to both the rotor away from the near surface region and the outer grids. Finer meshes were used around the blades and regions in the wake of the blades. Particularly, regions at the leading and trailing edge and in the middle of blade were finely meshed in order to capture the flow field more accurately. The outer mesh was coarsened in regions expanding away from the rotor in order to minimize the central processing unit (CPU) time. The different mesh zones used for the present simulations are illustrated in **Figure 8**, while various mesh details are shown in **Figure 9a** and **b**. A number of simulations were

**Figure 8.** *Illustration of the* 2D *numerical domain.*

**Table 1**. In order to calculate those parameters, the flowchart shown in **Figure 7** can

**4. Computational fluid dynamics of a Darrieus hydrokinetic turbine**

A computational domain is a region in the space in which the numerical equations of the fluid flow are solved by CFD. In order to solve the physics of the flow field around the blade, dividing the flow domain in a set of small subdomains (rotating and stationary domains) is required, which implies the generation of a mesh of cells, also defined as control volumes. Three fundamental aspects to evaluate the accuracy and the resolution time of a simulation are the geometry and size of the cells coupled to the numerical method used to solve the governing equations. The mesh size must be sufficiently small to provide an accurate numerical approximation, but it cannot be so small that the solution is impractical to be obtained with the available computational resource. Thus, the mesh is usually refined in the regions of interest around the main obstacles affecting the flow [83]. In the particular case of the vertical axis hydrokinetic turbines, these obstacles are the blades. The mesh can be structured or unstructured. In the first case, the mesh consists of quadrilateral cells in 2D or hexahedral cells in 3D. In turn, the unstructured mesh usually consists of triangles in 2D and tetrahedral in 3D, but cells of the mesh can adopt any form. Structured mesh usually implies shorter time resolution; nevertheless, the unstructured meshes may better represent the geometry. Yasushi [84] presents a discussion about the development of efficient computational analysis using unstructured mesh. On the other hand, Luo and Spiegel [85] propose a

be followed.

*Design procedure of a vertical axis hydrokinetic turbine.*

*Computational Fluid Dynamics Simulations*

**Figure 7.**

**178**

#### **Figure 9.**

*(a) Detail of the area mesh around the blades and (b) detail of the rotor mesh around the interface area.*


with 298,878 nodes and 1.58% error on *Cp* (**Table 3**). In this regard, further refinement might not improve the numerical results. The numerical results obtained from

**Mesh Nodes** *y***<sup>+</sup> Maximum power coefficient** *Cpmax* **Error (%)** Mesh 1 143,672 0.246 0.56 10.71 Mesh 2 167,896 0.221 0.64 14.28 Mesh 3 187,630 0.283 0.63 1.56 Mesh 4 298,878 0.261 0.62 1.58

*Computational Fluid Dynamic Simulation of Vertical Axis Hydrokinetic Turbines*

*DOI: http://dx.doi.org/10.5772/intechopen.89184*

The modeling of vertical axis hydrokinetic turbines can be done in steady state or transient modes depending on the objectives of the research and the available computational resources. If computational resources are scarce, relatively simple, steady flow models can be used to model the turbine blades in different azimuthal positions [96]. A more common approach is the transient modeling of the moving

In this work, transient analyses were carried out to characterize the performance of the investigated NACA 0025 hydrofoil profile. Performances are described in terms of *P*, *T*, and *Cp*, which are calculated according to Eq. (31). Because the flow over Darrieus turbine is a periodic one, sufficient temporal resolution is necessary to ensure proper unsteady simulation of the vertical axis hydrokinetic turbine and to obtain an independent solution on the time step. Different time step sizes Δ*t* that are equivalent to specific rotational displacements along the azimuth were tested. The chosen time step size was Δ*t* ¼ 0*:*1°, which properly captures the vortex shedding. Time step convergence was monitored for all conserved variables, and it was observed that acceptable levels of residuals (less than 1 � <sup>10</sup>�6) were attained after six rotations of the hydrokinetic turbine. This means that periodic convergence was

*Cp* <sup>¼</sup> *<sup>P</sup>*

*Cp* variation over a range of TSR values was studied for the selection of the best TSR, leading to the optimal performance of NACA 0025 hydrofoil profile, which was used in the blade geometrical design. The power versus azimuthal position of different TSRs during rotation is shown in **Figure 10**. The instantaneous power generated by the turbine is equal to the product of the turbine *ψ* and *T* acting on it. A nearly sinusoidal curve was obtained with three positive maxima at each turn and three positive minima (when TSR is equal to 1.75) or negative minima (when TSR is equal to 0.50, 1.00, 2.00); meaning that during a revolution, there are periods of time where the turbine produces torque on the fluid. It is observed that *Cp* increases and decreases approximately until 50 and 120° azimuthal position, respectively, i.e., the main power production occurs between 0 and 120° azimuthal positions for the first blade when TSRs are 1.75 and 2.00. In the figure, it can be seen that the maximum torque for the first blade is achieved at the azimuth angle around 50°. After the peak, the drag begins to increase as the blade enters into a dynamic stall, and the drag starts to be dominant up to a *θ* of 120°. Then, the second blade repeats the motion of the first blade, and the power production is completed with the same motion of the third blade for one rotation of the turbine. Plot of *Cp* versus TSR

<sup>0</sup>*:*5*ρAV*<sup>3</sup> (31)

mesh 4 were compared with several results available in the literature.

blades through the use of URANS approach [19, 97–99].

also achieved:

**181**

**Table 3.**

*Mesh convergence study.*

#### **Table 2.**

*Flow conditions in* CFD *analysis.*

carried out in order to determine how the mesh quality affected the CFD results. In this sense, the torque was calculated for each grid using the Fluent solver. The objective was to select the most appropriate mesh that can guarantee low computational costs and good result accuracy. It is widely known that the region near the blade plays an important role on the hydrokinetic operation, since it has the highest gradient of static pressure and velocity. Additionally, the near wake flow, which can extent up to downstream of the blade, has a great effect on the power [56, 92, 93]. It is well known that a refinement in the boundary layer and a sensitivity study of *y*<sup>þ</sup> are very important, since both of them have an effect on the turbine hydrodynamics. Therefore, a common parameter to identify the subparts of the boundary layer is the dimensionless distance from the wall *y*<sup>þ</sup> [94], defined by *y*<sup>þ</sup> ¼ Δ*yu*<sup>þ</sup> ð Þ *=v* , where Δ*y* is the distance of the first node from the wall, *u*<sup>þ</sup> is the wall shear velocity, and *v* is the kinematic viscosity. In this regard, the near-wall region can be roughly subdivided into three layers: the viscous layer *y*<sup>þ</sup> ð Þ <5 , the buffer layer ð Þ 5<*y* þ <30 , and the fully turbulent layer *y*<sup>þ</sup> ð Þ >30 [95]. Therefore, the quality of the mesh was also checked, as well as the *y*<sup>þ</sup> values around the blades, which is important for the turbulence modeling.

Symmetrical boundary conditions were defined at the top plane and in the bottom plane. Additionally, a uniform pressure on the outlet boundary was set, and a uniform velocity on the inlet boundary with a magnitude of 1.5 m*=*s was used for the TSR and the corresponding *ψ*, as shown in **Table 2**. *k* � *ω* shear stress transport (SST) turbulence model was employed for turbulence modeling since it showed better performance for complex flows including adverse pressure gradients and flow separations like occurs in vertical axis hydrokinetic turbines. The no-slip boundary condition was applied on the turbine wall blades. To simulate the rotation of the rotor, the circular turbine mesh with embedded blades allowed the relative movement to the outer inertial fixed domain. An interface wall was introduced between the fixed and rotating domains. The origin of the reference frame is the center of the rotor. The simulation methods used in this study are similar to the methods used in other numerical studies. Here, the rotational speed of the turbine axis is specified by user input.

To solve the viscous sublayer of the turbulence model used, the values of *y*<sup>þ</sup> generally must be less than 1. Subsequently, several meshes were made by increasing the refinement of the computational domain near the blade, achieving a good resolution of the boundary layer. The mesh 4 reached a convergence of the results


*Computational Fluid Dynamic Simulation of Vertical Axis Hydrokinetic Turbines DOI: http://dx.doi.org/10.5772/intechopen.89184*

#### **Table 3.**

carried out in order to determine how the mesh quality affected the CFD results. In this sense, the torque was calculated for each grid using the Fluent solver. The objective was to select the most appropriate mesh that can guarantee low computational costs and good result accuracy. It is widely known that the region near the blade plays an important role on the hydrokinetic operation, since it has the highest gradient of static pressure and velocity. Additionally, the near wake flow, which can extent up to downstream of the blade, has a great effect on the power [56, 92, 93]. It is well known that a refinement in the boundary layer and a sensitivity study of *y*<sup>þ</sup> are very important, since both of them have an effect on the turbine hydrodynamics. Therefore, a common parameter to identify the subparts of the boundary layer is the dimensionless distance from the wall *y*<sup>þ</sup> [94], defined by *y*<sup>þ</sup> ¼ Δ*yu*<sup>þ</sup> ð Þ *=v* , where Δ*y* is the distance of the first node from the wall, *u*<sup>þ</sup> is the wall shear velocity, and *v* is the kinematic viscosity. In this regard, the near-wall region can be roughly

*(a) Detail of the area mesh around the blades and (b) detail of the rotor mesh around the interface area.*

**λ 0.5 1.00 1.75 2.00 2.50** *ψ* ð Þ rad*=*s 0.997 1.994 3.489 3.987 4.984

subdivided into three layers: the viscous layer *y*<sup>þ</sup> ð Þ <5 , the buffer layer

important for the turbulence modeling.

**Figure 9.**

**Table 2.**

*Flow conditions in* CFD *analysis.*

*Computational Fluid Dynamics Simulations*

axis is specified by user input.

**180**

ð Þ 5<*y* þ <30 , and the fully turbulent layer *y*<sup>þ</sup> ð Þ >30 [95]. Therefore, the quality of the mesh was also checked, as well as the *y*<sup>þ</sup> values around the blades, which is

Symmetrical boundary conditions were defined at the top plane and in the bottom plane. Additionally, a uniform pressure on the outlet boundary was set, and a uniform velocity on the inlet boundary with a magnitude of 1.5 m*=*s was used for the TSR and the corresponding *ψ*, as shown in **Table 2**. *k* � *ω* shear stress transport (SST) turbulence model was employed for turbulence modeling since it showed better performance for complex flows including adverse pressure gradients and flow separations like occurs in vertical axis hydrokinetic turbines. The no-slip boundary condition was applied on the turbine wall blades. To simulate the rotation of the rotor, the circular turbine mesh with embedded blades allowed the relative movement to the outer inertial fixed domain. An interface wall was introduced between the fixed and rotating domains. The origin of the reference frame is the center of the rotor. The simulation methods used in this study are similar to the methods used in other numerical studies. Here, the rotational speed of the turbine

To solve the viscous sublayer of the turbulence model used, the values of *y*<sup>þ</sup> generally must be less than 1. Subsequently, several meshes were made by increasing the refinement of the computational domain near the blade, achieving a good resolution of the boundary layer. The mesh 4 reached a convergence of the results

*Mesh convergence study.*

with 298,878 nodes and 1.58% error on *Cp* (**Table 3**). In this regard, further refinement might not improve the numerical results. The numerical results obtained from mesh 4 were compared with several results available in the literature.

The modeling of vertical axis hydrokinetic turbines can be done in steady state or transient modes depending on the objectives of the research and the available computational resources. If computational resources are scarce, relatively simple, steady flow models can be used to model the turbine blades in different azimuthal positions [96]. A more common approach is the transient modeling of the moving blades through the use of URANS approach [19, 97–99].

In this work, transient analyses were carried out to characterize the performance of the investigated NACA 0025 hydrofoil profile. Performances are described in terms of *P*, *T*, and *Cp*, which are calculated according to Eq. (31). Because the flow over Darrieus turbine is a periodic one, sufficient temporal resolution is necessary to ensure proper unsteady simulation of the vertical axis hydrokinetic turbine and to obtain an independent solution on the time step. Different time step sizes Δ*t* that are equivalent to specific rotational displacements along the azimuth were tested. The chosen time step size was Δ*t* ¼ 0*:*1°, which properly captures the vortex shedding. Time step convergence was monitored for all conserved variables, and it was observed that acceptable levels of residuals (less than 1 � <sup>10</sup>�6) were attained after six rotations of the hydrokinetic turbine. This means that periodic convergence was also achieved:

$$C\_p = \frac{P}{0.5\rho A V^3} \tag{31}$$

*Cp* variation over a range of TSR values was studied for the selection of the best TSR, leading to the optimal performance of NACA 0025 hydrofoil profile, which was used in the blade geometrical design. The power versus azimuthal position of different TSRs during rotation is shown in **Figure 10**. The instantaneous power generated by the turbine is equal to the product of the turbine *ψ* and *T* acting on it. A nearly sinusoidal curve was obtained with three positive maxima at each turn and three positive minima (when TSR is equal to 1.75) or negative minima (when TSR is equal to 0.50, 1.00, 2.00); meaning that during a revolution, there are periods of time where the turbine produces torque on the fluid. It is observed that *Cp* increases and decreases approximately until 50 and 120° azimuthal position, respectively, i.e., the main power production occurs between 0 and 120° azimuthal positions for the first blade when TSRs are 1.75 and 2.00. In the figure, it can be seen that the maximum torque for the first blade is achieved at the azimuth angle around 50°. After the peak, the drag begins to increase as the blade enters into a dynamic stall, and the drag starts to be dominant up to a *θ* of 120°. Then, the second blade repeats the motion of the first blade, and the power production is completed with the same motion of the third blade for one rotation of the turbine. Plot of *Cp* versus TSR

**Figure 10.** *Power output for different TSRs.*

shows positive values of TSR close to 1.75, meaning that fluid is providing torque to the turbine. Beyond 1.75 TSR, *Cp* is negative, indicating that the turbine, rotating at a constant *ψ*, exerts torque on the fluid. This can be explained because a high TSR implies a high turbine angular speed and, in such as case, kinetic energy contained in flow is not enough to deliver torque to the turbine and make it to rotate with the same *ψ*.

**Figure 11** shows pressure contours at *θ* are equal to 0° and 30°. The contour plot shows that there is an increase of pressure from the upstream side to the downstream side across the blade. Additionally, the pressure in the outer area of the profile is observed to be larger (intrados) than that of the inner zone (extrados). The difference of pressure and velocity causes the overall lift for the turbine. The pressures are negative near the ends of the blade but positive at the exit of the

*The contours of pressure magnitude for the rotor (a) θ* ¼ *0*° *and (b) θ* ¼ *30*°*.*

*Computational Fluid Dynamic Simulation of Vertical Axis Hydrokinetic Turbines*

*DOI: http://dx.doi.org/10.5772/intechopen.89184*

In order to perceive the effect of TSR on the turbine performance, the average *Cp* achieved for different TSRs can be found. *Cp* is not constant because the torque and velocity are not constant in a Darrieus turbine. Hence, the average *Cp* per cycle is calculated as the product of the average values of these terms per cycle. TSR and *Cp* are in a direct relationship when the TSR is between 0.5 and 1.75. However, TSR and *Cp* have an opposite tendency for TSR greater than 1.75. The maximum value of *Cp* was achieved when TSR was 1.75; the value of the average *Cp* was 44.33% per cycle. Similar results were obtained by Dai et al. [22] for NACA 0025 blade profile. Additionally, Lain and Osorio [102] used experimental data of Dai and Lams work [22] and developed numerical models. They performed analysis on CFX solver, DMS model, and Fluent solver and achieved efficiencies of 58.6, 46.3, and 52.8%, respectively, when TSR was 1.745. Results observed by using Fluent solver

The design and simulation of a vertical axis hydrokinetic turbine were presented in this work. The most common modeling method for vertical axis hydrokinetic turbine is CFD. The numerical simulations allow analyzing many different turbine design parameters, providing an optimal configuration for a given set of design parameters. Before the simulations can be performed, the determination of the optimal grid and time step sizes required must be conducted. Finer grids and smaller time steps might give a more accurate solution, but they increase the computational cost. Thus, finding optimal values is also required. For this purpose, the turbulence model generally used is *k-ω* shear stress transport (SST) turbulence

The TSR is a significant parameter that affects the performance of hydrokinetic turbines. Consequently, the performance of the turbine was investigated with a simplified 2D numerical model. From the 2D model, *Cp* was computed for various TSRs. During a turbine revolution, the blade of the turbine may experience large, as

computational domain.

**Figure 11.**

were quite accurate.

**5. Conclusions**

model.

**183**

In the literature, optimum values of TSR for a Darrieus turbine were reported. For example, Kiho et al. [100], using a Darrieus turbine diameter of 1.6 m, found that the highest efficiency was achieved at 0.56 at 1.1 m*=*s V and two TSRs. In turn, Torri et al. [101] also found that the peak *Cp* of a three-blade straight vertical axis hydrokinetic turbine was about 0.35 at a TSR of around 2. However, Dai et al. [22] performed numerical and experimental analyses with four sets of a three-bladed rotor where blades were designed with NACA 0025 with four different *c* values. These four sets of rotors were tested in a tank at different *V* and *R*. The highest *Cp* was achieved by the rotor with a *c* of 162.88 mm, *R* of 450 mm, and TSR of 1.745. Furthermore, authors investigated the same rotor at different *V* and found 1.2 m*=*s as the most effective velocity. They concluded that larger rotors are more efficient, while flow velocity has little effect on the turbine efficiency. **Figure 10** shows that there is a high fluctuation with each revolution. The fluctuation decreases when *λ* is equal to 1.75.

The same tendencies of *Cp* are found in the case of TSR of 1.75 and 2.00, as it can be seen in **Figure 10**. The variation amplitude of *Cp* is lower when TSR is equal to 1.75. This result confirms that the blade with TSR of 1.75 has better performance than any other TSRs. When TSR is equal to 1.75, the maximum *Cp* is 0.62, and the variation amplitude of *Cp* is near 0.37. On the other hand, when TSR is 2.00, the turbine achieved a maximum *Cp* near 0.61 and an amplitude of only 0.83. Therefore, a turbine with a TSR of 1.75 has advantages over a turbine with a TSR of 2.00 in terms of the reduced fluctuation of its torque curve. *Cp* decreases for lower values of TSR because at low values of TSR, the flow surrounding the blade is separated, implying low lift and high drag. As a result, transferred torque from fluid to turbine decreases. In general, the fluctuations in *Cp* and, therefore, in *T* can produce a high amount of vibration in the turbine. The effect of these vibrations directly influences the fatigue life of the turbine blades and that of the generated power.

*Computational Fluid Dynamic Simulation of Vertical Axis Hydrokinetic Turbines DOI: http://dx.doi.org/10.5772/intechopen.89184*

**Figure 11.**

shows positive values of TSR close to 1.75, meaning that fluid is providing torque to the turbine. Beyond 1.75 TSR, *Cp* is negative, indicating that the turbine, rotating at a constant *ψ*, exerts torque on the fluid. This can be explained because a high TSR implies a high turbine angular speed and, in such as case, kinetic energy contained in flow is not enough to deliver torque to the turbine and make it to rotate with

In the literature, optimum values of TSR for a Darrieus turbine were reported. For example, Kiho et al. [100], using a Darrieus turbine diameter of 1.6 m, found that the highest efficiency was achieved at 0.56 at 1.1 m*=*s V and two TSRs. In turn, Torri et al. [101] also found that the peak *Cp* of a three-blade straight vertical axis hydrokinetic turbine was about 0.35 at a TSR of around 2. However, Dai et al. [22] performed numerical and experimental analyses with four sets of a three-bladed rotor where blades were designed with NACA 0025 with four different *c* values. These four sets of rotors were tested in a tank at different *V* and *R*. The highest *Cp* was achieved by the rotor with a *c* of 162.88 mm, *R* of 450 mm, and TSR of 1.745. Furthermore, authors investigated the same rotor at different *V* and found 1.2 m*=*s as the most effective velocity. They concluded that larger rotors are more efficient, while flow velocity has little effect on the turbine efficiency. **Figure 10** shows that there is a high fluctuation with each revolution. The fluctuation decreases when *λ* is

The same tendencies of *Cp* are found in the case of TSR of 1.75 and 2.00, as it can be seen in **Figure 10**. The variation amplitude of *Cp* is lower when TSR is equal to 1.75. This result confirms that the blade with TSR of 1.75 has better performance than any other TSRs. When TSR is equal to 1.75, the maximum *Cp* is 0.62, and the variation amplitude of *Cp* is near 0.37. On the other hand, when TSR is 2.00, the turbine achieved a maximum *Cp* near 0.61 and an amplitude of only 0.83. Therefore, a turbine with a TSR of 1.75 has advantages over a turbine with a TSR of 2.00 in terms of the reduced fluctuation of its torque curve. *Cp* decreases for lower values of TSR because at low values of TSR, the flow surrounding the blade is separated, implying low lift and high drag. As a result, transferred torque from fluid to turbine decreases. In general, the fluctuations in *Cp* and, therefore, in *T* can produce a high amount of vibration in the turbine. The effect of these vibrations directly influences the fatigue life of the turbine blades and that of the

the same *ψ*.

**Figure 10.**

*Power output for different TSRs.*

*Computational Fluid Dynamics Simulations*

equal to 1.75.

generated power.

**182**

*The contours of pressure magnitude for the rotor (a) θ* ¼ *0*° *and (b) θ* ¼ *30*°*.*

**Figure 11** shows pressure contours at *θ* are equal to 0° and 30°. The contour plot shows that there is an increase of pressure from the upstream side to the downstream side across the blade. Additionally, the pressure in the outer area of the profile is observed to be larger (intrados) than that of the inner zone (extrados). The difference of pressure and velocity causes the overall lift for the turbine. The pressures are negative near the ends of the blade but positive at the exit of the computational domain.

In order to perceive the effect of TSR on the turbine performance, the average *Cp* achieved for different TSRs can be found. *Cp* is not constant because the torque and velocity are not constant in a Darrieus turbine. Hence, the average *Cp* per cycle is calculated as the product of the average values of these terms per cycle. TSR and *Cp* are in a direct relationship when the TSR is between 0.5 and 1.75. However, TSR and *Cp* have an opposite tendency for TSR greater than 1.75. The maximum value of *Cp* was achieved when TSR was 1.75; the value of the average *Cp* was 44.33% per cycle. Similar results were obtained by Dai et al. [22] for NACA 0025 blade profile. Additionally, Lain and Osorio [102] used experimental data of Dai and Lams work [22] and developed numerical models. They performed analysis on CFX solver, DMS model, and Fluent solver and achieved efficiencies of 58.6, 46.3, and 52.8%, respectively, when TSR was 1.745. Results observed by using Fluent solver were quite accurate.

### **5. Conclusions**

The design and simulation of a vertical axis hydrokinetic turbine were presented in this work. The most common modeling method for vertical axis hydrokinetic turbine is CFD. The numerical simulations allow analyzing many different turbine design parameters, providing an optimal configuration for a given set of design parameters. Before the simulations can be performed, the determination of the optimal grid and time step sizes required must be conducted. Finer grids and smaller time steps might give a more accurate solution, but they increase the computational cost. Thus, finding optimal values is also required. For this purpose, the turbulence model generally used is *k-ω* shear stress transport (SST) turbulence model.

The TSR is a significant parameter that affects the performance of hydrokinetic turbines. Consequently, the performance of the turbine was investigated with a simplified 2D numerical model. From the 2D model, *Cp* was computed for various TSRs. During a turbine revolution, the blade of the turbine may experience large, as well as rapid variation, in *Cp*. A *Cp* maximum of 62% was achieved when TSR was equal to 1.75. The value of the average *Cp* was 44.33% per cycle. Though Darrieus turbine is very simple to be constructed, it has some disadvantages when compared to axial turbines since they exhibit a lower power coefficient and a variation in the torque produced within the cycle, leading to periodic loading on the components of the turbine.
