Fluid Dynamics Simulation of an NREL-S Series Wind Turbine Blade

Abstract

Wind turbine blades are known for their complex geometry and difficult-to-predict characteristics. So, this chapter aims to look in depth at theory, design, modeling, and simulation of a 1.2 MW wind turbine blade (35 m). Computational fluid dynamics (CFD) will be used to simulate the blade. The design tip speed ratio (TSR), the center point of the design, is optimally chosen as 7. The various parameters like torque vs TSR, Cp, and Ct vs TSR will be found for varying pitch angles. Simulations will be performed on the blade, and the results will be compared with those obtained from blade element & momentum (BEM) theory. Along with this, QBlade and XFoils results are compared with a much more accurate CFD simulation. To conclude, the accuracy of various methods will be compared and evaluated.

1. Introduction

Wind turbines have been around for more than a century now. Moreover, the idea of harvesting energy from wind has existed for even longer. Charles F. Brush invented the first automatic wind turbine for power generation in 1887. That does not mean that the technology has stagnated or remained unchanged. Since then, many scientists have improved the early designs, typically made out of wood and later aluminum. These days, the materials used are as exotic as the design, involving manufacturing processes, such as resin-transfer molding to create fiber-reinforced composites [1]. Even the designs themselves have changed radically. We have vertical axis wind turbines (VAWT) and horizontal axis wind turbine (HAWT) [1, 2]. Both have pros and cons, but for this chapter, HAWT will be the main focus owing to their relative popularity, high efficiency, and simplicity. Figure 1 shows HAWT and VAWT for comparison.

Figure 1.

HAWT and VAWT side by side (image from iStock/purchased for use).

Renewable energy is projected to hit 31% of all energy generation by 2035 across the world. Out of this, a quarter will be from wind power alone [3] with a high projected growth rate. However, the wind turbine blade is one complex piece of engineering that requires its own attention. It is a significant portion of the entire cost of the machine. The blades are indeed immense and have subtle curves. The fundamental aim of this chapter will be to see how these curves affect the wind turbine blade performance. The theory of the blades will be explained first, followed by design in CAD. Then the blade performance will be estimated roughly using the blade element and momentum (BEM) theory. Then, extensive simulations will be performed in ANSYS Fluent to determine the exact characteristics. The same will be verified and validated by our earlier estimates obtained by BEM theory.

The chapter has been designed concisely and easy to follow, so that it will be comprehensible for newcomers yet contain essential data for the experts. It is divided as follows: Firstly, we will look at BEM and perform the initial estimation of blade characteristics. The exact “curves” of the blades will be determined using simple equations solved in MATLAB. We will use NREL-S Series Airfoils (the “curves”), namely, S815, S825, and S826 for root, primary & tip portions, respectively. The geometry will require specific parameters of the airfoils. Here, QBlade and XFoils will prove particularly handy for determining these parameters and assist in blade design. This step will be followed by CFD logic and ANSYS Fluent working methods. Particular attention will be given to Navier-Stokes Equation in rotational domain and how it differs from the common coordinate form. After this, the CAD modeling will be touched on briefly as it is highly software dependent. After that, the Fluent simulations will be performed, and the various performance parameters will be noted. Finally, the results obtained will be compared with the estimates produced earlier.

2. Theory

The first requirement of any simulation is the initial estimation of quantities of interest. This calculation will give an idea about the expected results and will act as a prerequisite for the last step: verification and validation. Without this, the simulation might produce some other results that need not always be correct.

2.1 One dimensional momentum

One-dimensional momentum theory is one of the oldest theories of wind turbines. Much literature is dedicated to the same. It relates the velocities upstream, at the turbine blades, and downstream with a mathematical induction factor “a.” The induction factor is essential and has some implications for the wind turbine as a whole. The exact derivation may be seen in [2, 4]. The formulae alone will be listed here.

Let the velocity of wind upstream be u; at the turbine be y; and downstream be v; then:

$$y=\frac{\left(u+v\right)}{2}$$E1

The maximum power that can be generated from the wind is:

$$P_{\mathit{\text{wind}}}=0.5\rho u^{3}A$$E2

The maximum torque that can be extracted from the wind is:

$$T_{\mathit{\text{wind}}}=0.5\rho u^{2}A$$E3

It is convenient to use a non-dimensional power coefficient (Cp) and torque coefficient (Ct) as it is a ratio from $0<C<1$. They are defined as:

$$C_p=\frac{P_{\mathit{\text{out}}}}{P_{\mathit{\text{wind}}}}$$E4

$$C_t=\frac{T_{\mathit{\text{out}}}}{T_{\mathit{\text{wind}}}}$$E5

“a” is the mathematical induction factor defined as:

$${\mathbf{C}}_{\mathbf{p}}\mathbf{=}\mathbf{4}\mathbf{a}{\left(\mathbf{1}-\mathbf{a}\right)}^{\mathbf{2}}$$E6

$${\mathbf{C}}_{\mathbf{t}}\mathbf{=}\mathbf{4}\mathbf{a}\left(\mathbf{1}-\mathbf{a}\right)$$E7

These are the two primary verification and validation formulae. Through Fluent simulation, the velocity distribution and torque/power will be found separately. Notice how the induction factor links them. One can use Eq. (6) to compute the induction factor as a ballpark figure. Eq. (7) can then be used to provide theoretical Ct. But Ct can be directly found through Eq. (5) using Fluent. By comparing these two values, we can check for the correctness of our results.

The maximum power coefficient (percentage) that can be delivered by a wind turbine is 59.3%, and the induction factor must be less than 0.5. Anything above that is impossible or has no practical significance. This limit in power coefficient is known as Betz Limit, and it arises because some energy needs to be present in the wind to move past the turbine blades to prevent local wind accumulation. The same can be figured out by finding the maximum value of Eq. (6). Verification and validation will be performed in the end using these points. Large deviations can be expected as this theory does not account for turbulence and is a significant approximation of the underlying physics.

2.2 Blade element momentum

A wind turbine blade is known for its characteristic twist as one moves along the body. This twist is the characteristic angle defined by $\beta$. An airfoil provides max lift only for a particular angle of attack. That is easy in an airplane , exhibiting translational motion where one adjusts the pitch angle for maximum lift. However, a wind turbine exhibits rotational motion. The fundamental problem is that any two points on the circle’s radius never move at the same speed. Since the angle of attack is computed keeping the net velocity wind vector as a reference, the angle with this must remain constant. If one looks at this velocity vector, it has a k component of wind velocity (incoming wind) and an i component of the rotational velocity. The net velocity vector is:

$$V_{\mathit{\text{relativetoblade}}}=u_{\mathit{\text{wind}}}\widehat{k}+\mathit{r\omega }\widehat{i}$$E8

One can see that as we move across the blade, the net velocity vector will change and is, in fact, a function of radii. The only way to make a constant angle with this vector at all points is to compensate with a twist angle of our own. Hence, the characteristic curve.

BEM theory will help us with the exact mathematical formulae to compute this twist angle and hence, will be the starting point of our design. For exact derivation, please refer to [1, 2, 3, 5, 6, 7].

The local-speed ratio for arbitrary radii r and with incoming wind velocity u from the center is defined as:

$${\lambda }_r=\frac{\mathit{r\omega }}{u}$$E9

Note the local speed ratio changes as one moves along the blade. The angle made by the horizontal and the net velocity vector (as defined earlier) is:

$$\varphi =\frac{2}{3}{tan}^{-1}\frac{1}{{\lambda }_r}$$E10

Here, the angles can be written as below for zero pitch. Also, $\alpha$ was assumed to be equal to 5.25 degrees. Please refer to Figure 2 for visualizing the exact angles.

Figure 2.

Airfoil angles (image referred from [1]).

$$\alpha =\varphi -\beta$$E11

The chord length of the airfoil is given by:

$$c=\frac{8\mathit{\pi r}}{{\mathit{BC}}_l}\left(1-cos\varphi \right)$$E12

where B is the number of blades (3 in our case), Cl is the lift coefficient, and r is the radii from the center. However, one can notice that except for Cl, the net blade length and the rotational speed $\omega$, everything else is defined and can easily be computed. Many approaches, such as calculating axial and tangential induction factors have been developed [3, 5]. This method suffers from the limitation that the airfoil data must be present, and the airfoil must be uniform. Neither is applicable in our case, as NREL has not released airfoil data separately, and the root, primary, and tip are composed of totally different airfoils. The net blade length can be determined from previous designs for a chosen power level. Furthermore, 35 meters from the hub center to the tip was assumed to be sufficient. NREL has mentioned the maximum obtainable lift coefficient for each of the three airfoils. These values were averaged, and a slightly lower figure of 1.3 was chosen for Cl, and Cd was chosen as 0.1. Finally, the wind turbine was designed for an optimal TSR of 7. The TSR and blade length give an omega of 2.42 rad/sec.

The chord length and twist angle give us everything to design our blade in CAD. As a cross verification, XFoils and QBlade will be used to generate performance curves. Tables 1 and 2 give the variation of twist angle and chord length as one moves across the blade.

Distance from center	Twist anglea
4	29
8	16
12	9
16	6
20	5
24	3
28	2
30	0.025
35	0

Table 1.

Twist angle vs distance from center.

^a

Approximate values.

Distance from center	Chord lengtha
4	4.4
8	3.4
12	2.6
16	2
20	1.8
24	1.4
28	1.2
30	1.1
35	1

Table 2.

Chord length vs distance from center.

^a

Approximate values.

QBlade will take the various airfoil parameters and generate curves, such as Cl vs TSR, Cd vs TSR, and Cl/Cd vs TSR. These are the three curves of interest. Our earlier value of Cl can be cross-checked with this software-generated graph. It is worth noting that QBlade does assume varying airfoils across the blade. The blade itself is designed through a selection tab for different airfoils. After this, the simulation is performed using highly simplified models for turbulence and airfoils. Later, CFD simulations will verify and produce highly accurate results.

3. QBlade and XFoils simulation

QBlade and XFoils are open-source software for the prediction of wind turbine performance. The models generated and performance curves have been shown in the figures below:

We get a maximum power coefficient close to the Betz limit (59.2%, approximately) at the expected TSR of 7. The power coefficient that was obtained verifies our design to some extent. Figure 3 shows the plot of various airfoil curves used for this chapter. Figure 4 shows the QBlade simulation results.

Figure 3.

Airfoil shapes superimposed on one another.

Figure 4.

QBlade simulation graphs.

4. Computational fluid dynamics and fluent

The fluid equations can be solved either in differential form or integral form. The differential form is obtained by applying conservation laws to a fluid particle in an Eulerian frame of reference. The integral form is obtained by applying conservation laws to a control volume.

The following are the differential form of fluid equations:

$$\frac{\partial u}{\partial x}+\frac{\partial v}{\partial y}=0$$

$$\rho \left(u\frac{\partial u}{\partial x}+v\frac{\partial u}{\partial y}\right)=-\frac{\partial p}{\partial x}+\mu {\nabla }^{2}u$$

$$\rho \left(u\frac{\partial v}{\partial x}+v\frac{\partial v}{\partial y}\right)=-\frac{\partial p}{\partial y}+\mu {\nabla }^{2}v$$E13

There is also the integral form of fluid equations, as listed below:

$${\int }_S\left(v.n\right)\mathit{dS}=0$$

$${\int }_S\rho \left(v.\widehat{n}\right)\overrightarrow{V}\mathit{dS}=-{\int }_S\rho \widehat{n}\mathit{dS}+{\overrightarrow{F}}_{\mathit{\text{visc}}}$$E14

The integral form of fluid equations is mainly preferred since conservation is always valid for any control volume or mesh “chunk.” Conservation does not apply to each element in the differential form; hence, in industry, the integral form is preferred. Our software for CFD simulation is ANSYS Fluent, which uses the integral form for solving the problem. Both these equations of integral form are valid for any region or arbitrary shape of a control volume. However, Fluent will produce numeric solutions satisfying these equations for only a particular shape of control volume defined during the meshing step. Meshing breaks the 3D geometry into smaller “chunks” processed as individual control volumes.

The solution methodology introduces errors when solving these equations in Fluent. Two types of errors are introduced, namely, discretization and linearization errors. Discretization error occurs because we assume the value at the interface of adjoining cells is nothing but the average of each of those cell center values. Figure 5 shows the control volumes and cell centers for a typical uniform meshing. Uniform rectangular chunks will not be the case for complex geometry, as the geometry will be broken into tetrahedrons. The averaging algorithm is also more exotic and will not be covered here.

Figure 5.

Discretization I.

However, on solving these equations, we end up with a set of nonlinear algebraic equations. These can be solved only by Newton-Raphson (NR) method by assuming a guess value for each cell center. NR will continually iterate until the error falls below a particular threshold. NR method leads to another source of error known as linearization error. The ultimate aim is to reduce both errors as much as possible.

The mesh geometry plays an important role here. More “chunks” leads to less discretization error but more linearization error and vice versa. Hence, in Fluent, it is essential to hit the sweet spot for all geometry. Here, we conclude the inner working of Fluent for the translational or inertial frame of reference. In the next section, the Navier-Stokes equation will be modified for the rotational frame of reference.

5. Navier-Stokes in rotational domain

Navier-Stokes/fluid equation(s) are well known by most in the translational domain. However, as described earlier, a wind turbine exhibits rotational motion, and the fluid equations take a different form. At the outset, it is evident that extra forces will act on the fluid particle due to the rotational motion when viewed from the inertial frame of reference. These forces will have to be accounted for in the integral form of fluid equations as used by Fluent.

A vector is assumed to rotate with a radial velocity $\mathrm{\Omega }$ [8]. From the perspective of the vector, the vector itself is static. However, from the inertial frame of reference, the vector is rotating. For a small time-period “t”, the angle subtended by the new vector position with the old vector is:

$$\theta =\mathrm{\Omega \Delta }t$$E15

The magnitude of change in the new vector from the old vector (position-wise) forms a sector of a circle [8]. This gives a net length of:

$$\mathrm{\Delta }{i}_{\mathit{new}}-\mathrm{\Delta }{i}_{\mathit{old}}=r\mathrm{\Omega \Delta }t$$E16

Notice that the triangle formed by these three vectors is a right-angle triangle for a small change in vector in a short period “t.” The (change in vector)/(new vector) = sin ($\varphi$)

Hence, we can write the net vector change with magnitude and direction as the following [8]. Note that the change vector is perpendicular to both the old vector as well as the rotational axis

$$\mathrm{\Delta }\widehat{i}=\mid \widehat{i}\mid sin\left(\varphi \right)\mathrm{\Omega \Delta }t\frac{\overrightarrow{\mathrm{\Omega }}\times \widehat{i}}{\mid \overrightarrow{\mathrm{\Omega }}\times \widehat{i}\mid }$$E17

By definition of cross product:

$$\mid \overrightarrow{\mathrm{\Omega }}\times \widehat{i}\mid =\mid \widehat{i}\mid \mathrm{\Omega }sin\left(\varphi \right)$$E18

Therefore, substituting this in the previous equation

$$\frac{d}{\mathit{dt}}\widehat{i}=\overrightarrow{\mathrm{\Omega }}\times \widehat{i}$$E19

This was for a stationary vector. One can extend the analogy to a vector rotating in a rotating frame of reference. As imaginable, the sum of the rate of change of individual vector rotation and the frame rotation will be the rate of change of net rotation [8, 9]. However, the rate of change in frame rotation has been defined earlier. Hence, we obtain Chasle’s theorem [9].

$$\frac{d\overrightarrow{A}}{\mathit{dt}}=\frac{{\mathit{dA}}_i}{\mathit{dt}}+\overrightarrow{\mathrm{\Omega }}\times \overrightarrow{A}$$E20

where ($\frac{{\mathit{dA}}_i}{\mathit{dt}}$) term is the vector rotation as seen by the observer in the rotating frame of reference [9].

For Navier-Stokes, the fluid velocity “u” is rotating and is viewed from a stationary frame of reference. Hence, by applying Chasle’s theorem on the fluid velocity “u.”

$${\left(\frac{d{\overrightarrow{u}}_{\mathit{\text{inertial}}}}{\mathit{dt}}\right)}_{\mathit{\text{inertial}}}={\left(\frac{d{\overrightarrow{u}}_{\mathit{\text{inertial}}}}{\mathit{dt}}\right)}_{\mathit{\text{rotational}}}+\overrightarrow{\mathrm{\Omega }}\times {\overrightarrow{u}}_{\mathit{\text{inertial}}}$$E21

Re-substituting Chasle’s theorem twice in this equation, we obtain the final equation and assume constant velocity flow:

$${\left(\frac{d{\overrightarrow{u}}_{\mathit{\text{rotational}}}}{\mathit{dt}}\right)}_{\mathit{\text{rotational}}}=2\overrightarrow{\mathrm{\Omega }}\times \overrightarrow{u}+\overrightarrow{\mathrm{\Omega }}\times \left[\overrightarrow{\mathrm{\Omega }}\times \overrightarrow{x}\right]$$E22

It is interesting to note that the following is known as Coriolis acceleration.

$$2\overrightarrow{\mathrm{\Omega }}\times \overrightarrow{u}$$E23

The following is the centrifugal acceleration. These two equations put together define the Navier–Stokes in the rotational domain.

$$\overrightarrow{\mathrm{\Omega }}\times \left[\overrightarrow{\mathrm{\Omega }}\times \overrightarrow{x}\right]$$E24

The exact equation that will be solved in Fluent for our wind turbine is as follows. One can note the similarities between the earlier two equations and this:

$$\frac{\partial \rho }{\partial t}+\nabla .\rho {\overrightarrow{v}}_r=0$$

$$\nabla .\left(\rho {\overrightarrow{v}}_r{\overrightarrow{v}}_r\right)+\rho \left(2\overrightarrow{\mathrm{\Omega }}\times {\overrightarrow{v}}_r+\overrightarrow{\mathrm{\Omega }}\times \overrightarrow{\mathrm{\Omega }}\times \overrightarrow{r}\right)=-\nabla p+\nabla {\tau }_r$$E25

The next section will be brief and devoted to CAD modeling of blade.

6. CAD model of blade

The CAD model of the blade can be made using any 3D CAD software. ANSYS Fluent supports many types of 3D file formats and can import a solid-works project directly. ANSYS also has an inbuilt geometry design software named space-claim, and an old one named design-modeller. The actual CAD design steps are out of the scope of this chapter. Fusion360 was used to design the blade model, and the same was imported as a (.stp) STEP file into ANSYS. Figure 6 shows the blade geometry as a sketch and a body.

Figure 6.

CAD model of blade.

It is crucial to note that we are NOT modeling the blade, but rather the fluid surrounding it. Imagine a cylinder (rather a sector of a 3D cylinder spanning 120 degrees) where the blade is left hollow. The actual geometry is the air surrounding the blade, not the blade itself. It is the subtraction of the blade from the cylinder geometry. It is understandable that as air cannot penetrate the blade, that region is left hollow. One may refer to the following figures for the blade design.

One can see the blade’s outline in the 3D sector (120 degrees) of a cylinder in Figure 7. The subtracted geometry will be used for simulation and imported into ANSYS. The following section will discuss the simulation setup, the mathematical model used, Fluent, boundary conditions, and solution iterations.

Figure 7.

CAD model for simulation.

7. ANSYS fluent setup: a quick glance

This section will examine how the simulation was run in ANSYS. The various sub-sections will look at different steps in the execution order. Fluent will need a lot of data and setup before running the simulation and getting results. Before running the simulation, all properties, boundary conditions, and a few other parameters must be defined. One can note that there is symmetry in a wind turbine blade. It repeats every 120 degrees, normal to the rotational axis. We can save much time by simulating only this 120-degree portion and then repeating the graphical “Instances” every 120 degrees. This will be seen in the final results subsection.

Any ANSYS Fluent project will go through the same five steps:

• Geometry Import: Here you import the geometry (Figure 8).

• Meshing: Geometry is broken into smaller “chunks” for use as control volume by Fluent (Figure 9).

• Fluent Setup: Setup all the necessary stuff like mathematical models, boundary conditions, interfaces, and other parameters (Figure 10).

• Solution Iteration: Model is solved till the solution converges and the error falls below the desired margin.

• Results: View your results interactively and graphically (Figure 11).

Figure 8.

Geometry import.

Figure 9.

Meshing of the geometry.

Figure 10.

Fluent options.

Figure 11.

Results in CFD-Post. Notice the 3-bladed turbine generated from a 1/3rd portion.

7.1 Geometry import and meshing

7.1.1 Fluent setup

The step described in this section is the major one, where one defines the mathematical model to be solved, the accompanying boundary conditions, and the interface setup.

7.1.2 Mathematical model

The primary model to be set up is the turbulence model. SST k-omega was used for this chapter. There are multiple turbulence models in Fluent, each with pros and cons. The next step is to choose the fluid properties (air was selected). Then one needs to set the cell-zone conditions. Here, the rotational frame of reference must be set. The speed of rotation of the frame is the speed of blade rotation. For multiple simulations, this will take on multiple values. For TSR of 7, it is 2.42 rad/sec.

7.1.3 Boundary conditions

Here, we set the boundary values; the inlet wind velocity is set as 12 m/sec along the z-axis. The fluid was selected to be air. The outlet was set to have a constant atmospheric pressure of 1 atm. Fluent uses the gauge pressure system, where the values are computed at the center-point of 1 atm. This system improves the floating point accuracy. Period 1 and period 2 were set as interfaces. The blade itself was set as a wall with no-slip condition.

7.1.4 Need for interfaces

Since we have used a 1/3rd geometry setup, we need to declare the adjoining faces as interfaces. This setup will cause Fluent to assume that the geometry repeats. The settings include the periodic angle setup, which will be set at 120 degrees.

7.2 Results

This is the final step post solution iterations. When the errors have fallen below the tolerance value, the simulation is stopped. Finally, the results can be seen in CFD-Post.

8. Results: CFD-Post

8.1 Velocity streamlines

Here, the velocity streamlines for various pitch angles (0,3,5, and 10 degrees) and TSR (5,6,7,8, and 9) are presented. Streamlines track the path of the wind as it flows across the blades. The least obtained velocity was 7.27 m/sec. This velocity (7.27 m/sec) is essential as it directly affects how much energy is extracted from the wind [10] shows some velocity streamlines for non-separated flow, as the turbine is optimized. Our results indicate non-separated flow at optimal TSR. Figure 12 shows the velocity streamlines for various turbine blade configurations. The five rows of the image are the TSR 5, 6, 7, 8, and 9, and the four columns are pitch angles of 0, 3, 5, and 10 degrees. Every image at location {TSR, Pitch} corresponds to that particular input condition.

Figure 12.

Velocity streamlines for varying pitch and TSR.

8.2 Pressure contours at root of the blade: CFD-Post

The pressure contours are directly responsible for torque generation by the blade. Typically, the bottom portion should have high pressure, followed by the top side, which has low pressure. This net pressure difference creates lift at an angle. A portion of this lift will assist in blade rotation. One can note that as the pitch angle is high and TSR is increased, the low and high-pressure regions shift, and the blade will stop generating torque, or if pitching is increased further, it will generate reverse torque. This unique feature can make the blade stop rotating in stormy or very high TSR conditions by moving the blade to this appropriate zero torque angle. One can also note that the blade produces maximum torque when the angle of attack is close to 5 degrees, which depends on TSR and pitch angle. The two contours shown here are for the root (S815), Figure 13 and tip (S826), and Figure 14 of the blade. The five rows of the image are the TSR 5, 6, 7, 8, and 9, and the four columns are pitch angles of 0, 3, 5, and 10 degrees. Every image at location {TSR, Pitch} corresponds to that particular input condition [10] shows pressure contours where the wake (region of low pressure) is visible at the tail end of the airfoil. However, the blade as a whole is not simulated, and this produces slightly differing pressure contours in our case but is still consistent with our results.

Figure 13.

Pressure contours of blade root (S815) for varying pitch and TSR.

Figure 14.

Pressure contours of blade tip (S826) for varying pitch and TSR.

9. Results: Torque & Cp

In this section, the numerical results of the generated torque and power coefficient will be presented here. As per our earlier section on one-dimensional momentum theory, the power present in the wind for a wind speed of 12 m/sec and a blade length of 31 m (from root to tip alone, the root to hub center is 4 m) is:

$$P_{\mathit{\text{wind}}}=0.5\ast 1.225\ast {12}^{3\ast }\pi \ast {31}^2=3193764.336W$$E26

The results are presented in Table 3. The following can be noted from the tabular results:

• The maximum obtained power coefficient is 0.421 for 0-degree pitch and 9 TSR. This value is slightly higher than the one obtained for the pitch of 5 degrees, TSR 7, which is our optimal angle of attack (approximately 5.25). The twist angle was computed, and 5.25 degrees was subtracted to give the twist for a 0-degree pitch [11, 12] provides a maximum computed Cp for a 2 MW blade as 0.4436 (not through CFD). Although with minor deviations, our values are still very close.

• The 5-degree pitch gives the most consistent high Cp ($<$ 0.3) for varying TSR. This result is in line with our calculation.

• One hits near zero torque for 10-degree pitch and TSR 8. The correct angle to stop the blade will be around 10 degrees for higher TSR (not simulated).

• The 15-degree pitch gives positive torque only for extremely low TSR of $<$ 5.

• Pitching is a way to control torque generation and plays a significant role in large turbines, unlike small turbines. It is an effective means to control the system as a whole. Graphs in ref. [7] clearly show an increase followed by a decrease in Cp as the pitch angle is linearly increased.

Pitch	TSR	$\mathrm{\Omega }$	Torquea	Net power	Cp
0	5	1.71	136537	700434.81	0.219313242
0	6	2.06	164431	1016183.58	0.318177384
0	7	2.42	168523	1223476.98	0.383083049
0	8	2.74	157794	1297066.68	0.40612473
0	9	3.09	145060	1344706.2	0.421041147
3	5	1.71	170936	876901.68	0.274566808
3	6	2.06	188062	1162223.16	0.363903857
3	7	2.42	175964	1277498.64	0.399997779
3	8	2.74	160838	1322088.36	0.413959272
3	9	3.09	136504	1265392.08	0.396207092
5	5	1.71	136537	700434.81	0.219313242
5	6	2.06	187062	1156043.16	0.361968836
5	7	2.42	165373	1200607.98	0.375922533
5	8	2.74	143951	1183277.22	0.370496097
5	9	3.09	110525	1024566.75	0.320802239
10	5	1.71	158776	814520.88	0.255034747
10	6	2.06	120066	742007.88	0.232330192
10	7	2.42	52646	382209.96	0.119673814
10	8	2.74	3828	31466.16	0.009852374
15	5	1.71	69318	355601.34	0.111342386

Table 3.

Pitch, TSR vs Torque (in N-m), Net Power (in W), and Cp.

^a

1/3rd of total torque generated as the simulation was performed for a single blade.

10. Verification & validation

One can compare the Cp obtained with that predicted by the one-dimensional momentum theory. The induction factor for a Cp (maximum) of 0.421 is 0.121869

$$C_p=4a{\left(1-a\right)}^2=0.3759$$E27

Substituting the induction factor below,

$$C_t=4a\left(1-a\right)=0.428068$$E28

The actual torque coefficient was calculated assuming the net blade length of 35 m to account for tip/hub losses. The computed value below is indeed very close, verifying our solution.

$$C_t=\frac{T_{\mathit{\text{out}}}}{0.5\rho u^{2}A}=\frac{165373}{339261.3}=0.487450234$$E29

Now, let us finally compare our solution with QBlade and XFoils. Below is the Cp vs TSR Curve (Figure 15). We can see some deviation from the QBlade data and CFD. This deviation is probably due to extra turbulence caused by the rotor hub, which was accounted for in CFD but was left empty in QBlade. The energy dissipation and turbulence cause a lower figure to appear in CFD.

Figure 15.

Cp vs TSR for QBlade and CFD.

11. Conclusion

The chapter looked in-depth at the theory behind wind turbines, including solving equations and the various theories describing wind turbines in general. QBlade and XFoils were used to get a basic idea about the performance curves. Navier–Stokes equation was derived in rotational form, and the equations to solve for wind turbines by Fluent were listed. A brief look at the CAD design of the blade was given. Then, the complete procedure to perform an ANSYS simulation was explained, including Fluent Setup. Then, the results were presented graphically and numerically, and inferences were drawn. Finally, verification and validation were performed, verifying the simulation’s correctness.

The main aim of the chapter was to provide the exact methodology to go from a theory in paper to results in Fluent. Every aspect of wind turbine design was covered in this chapter. The correctness of various theories and even QBlade & XFoils was compared to Fluent. Multiple simulations were performed in Fluent, with each 30 min simulation yielding a single row of tabular results. Finally, pitching inference was drawn for huge blades. Results were reported in a graphical and user-friendly manner without going into raw data. Verification and Validation, the most tricky and essential step, was successful for the simulation, and the errors were within bounds.

Acknowledgments

Major thanks for this chapter, as well as my inspiration, goes to Rajesh Bhaskaran from Cornell University. Please note that I am not affiliated in any way with that university. I just attended an online course on “A Hands-on Introduction to Engineering Simulations” in eDX in 2019. Since then, I was always fascinated by these giant machines and their curved blades.

Furthermore, no small part goes to the Dell R710, Dual Hexa-Core 3.3 GHz Xeon Processor-based server that gave me the raw power to run Fluent. Without it, so many tabular entries would have been impossible.

I am highly thankful to all my teachers, my parents, and others who have helped me along the way, without whom achieving this goal would have been impossible.

Abbreviations

TSR	Tip Speed Ratio
HAWT	Horizontal Axis Wind Turbine
VAWT	Vertical Axis Wind Turbine
CFD	Computational Fluid Dynamics
Cp	Power Coefficient
Ct	Torque Coefficient
a	Axial Induction Factor
BEM	Blade Element & Momentum Theory
NREL	National Renewable Energy Laboratory
a	Axial Induction Factor
u	Upstream Wind Velocity
v	Downstream Wind Velocity
y	Wind Velocity close to turbine
Pwind	Maximum Power present in the wind
Twind	Maximum Torque that can be extracted from the wind
λr	Local Speed Ratio
ϕ	Angle made by the horizontal and the net velocity vector
α	Angle of Attack
β	Characteristic Twist Angle
c	Chord Length
B	Number of Blades
Cl	Lift Coefficient
Cd	Drag Coefficient
Ω	Radial Coefficient
ρ	Density of Air
t	Time Period
v→r	Velocity Vector at that point
r→	Position Vector at that point
p	Pressure at that point
τr	Torsional Force at that point