Structural and Modal Analysis of a Small Wind Turbine Blade Considering Composite Material and the IEC 61400-2 Standard

Abstract

IEC 61400-2 establishes the Simplified Load Method for designing low-power wind turbine blades without considering dynamic loads in the simplified load methodology. This paper analyzes the load hypotheses established by the standard, also considering the natural frequencies in a 900 W blade. The research methodology begins with the design parameters, the application of the BEM Method, and the use of the QBlade software. Then, the load hypotheses of the standard are defined. Finally, the structural design and the modal and structural analysis of the blade were conducted using FEM-based software. The results show that the minimum participation factors are found on the z-axis and the maximum on the x- and y-axis, and their magnitudes decrease when the natural frequency increases. In general, the principal maximum stresses are located in the middle section of the blade, in the external fiberglass layer, both on the intrados and extrados sides. In conclusion, structural scenarios were established to relate the participation factors of the modal analyses with the load hypotheses. The critical scenarios are at natural frequencies below 280 Hz.

1. Introduction

According to the Mexican Wind Energy Association (AMDEE), Mexico has 7317 MW of installed wind capacity to date [1]. The design methodology for wind turbines, including low-capacity wind turbines (with rotors smaller than 200 m²), requires several theories and standards, such as the Blade Element Moment (BEM) methodology, which uses the one-dimensional moment theory, and the blade element theory are applied to determine the geometric and aerodynamic characteristics of the rotor. On the other hand, several authors also use vortex theory to estimate rotor aerodynamics. For example, Arramach, J. et al. [2] proposed a mathematical model for predicting the performance of a wind turbine rotor based on BEM theory. They varied wind speeds to consider centrifugal pumping losses caused by radial flow along the blades. The numerical results were validated with experimental data, such as power and torque curves, and agreement with the mathematical models. De Freitas Pinto, R.L. and Furtado Gonçalves, B.P. [3] presented an analysis on the aerodynamic optimization of the drag effects of a horizontal axis turbine based on the BEM theory, proposing a nonlinear programming problem with equality and inequality constraints, with an optimal relationship of the blade tip operating speed and the maximum power coefficient. The authors concluded that the Betz limit was not reached in real turbines, even in the absence of aerodynamic drag. Sang, S. et al. [4] analyzed the dynamic effects of installation and pendulum motion of a wind turbine due to constant and variable real wind speed acting on the blade. They modified the BEM theory model to simulate the aerodynamic load and load distribution of wind turbine blades. The authors concluded that the load calculation methods can provide theoretical validity for decision-making in wind turbine control.

Nowadays, the most conventional materials for wind turbine blade design and manufacturing are composite materials such as glass fibers or carbon fibers and epoxy, which give them advantages in physical and mechanical properties compared to other materials. Mangestiyono, W. et al. [5] performed mechanical tests on fiberglass specimens according to the longitudinal configuration along the blade, having a thickness equal to that of the blade’s root. Tensile tests were performed, obtaining the tensile strength of each layer used in the blade and, as a result, determining that the blade is capable of operating. Torregrosa, A.J. et al. [6] optimized the orientation of the fibers of the layers of the composite materials used (fiberglass and carbon fiber) in a blade with an S809 aerodynamic profile, with an eight-layer configuration of the composite material, based on the BEM theory. By making a structural analysis of said blade with the finite element method, they demonstrated that the power coefficient depends only on the specific speed.

Mechanical vibrations are another critical aspect to consider when designing wind turbine blades. Zaradnik, R. et al. [7] proposed finite element models to estimate the stress incidence curves on the natural vibration frequencies of wind turbine blades. These stresses are caused by centrifugal and aerodynamic forces, which vary the blade length and wind speed. The authors concluded that the blade’s natural frequencies increase as a result of the stress distribution of the aerodynamic loads on the blade. Wang, L. et al. [8] analyzed the vibrations and damping of a 10 kW carbon fiber wind turbine blade with viscoelastic damping treatment. The system included a carbon fiber layer and a viscoelastic damping layer, the latter varying its thickness to analyze the vibration modes and fatigue cases, reducing the amplitude of the blade vibrations by adding a viscoelastic damping layer. Ganeriwala, S.N. et al. [9] show the results of modal tests performed on a wind turbine blade with different induced cracks. The authors obtained the vibration modes of the blade affected by a crack, generating changes in its modal structural parameters (modal frequencies and damping) with larger cracks. They conclude that if the first seven vibration modes of the blades are calculated, they may be sufficient for failure prediction. Xu, J. et al. [10] analyzed the influence of rotation speed on the natural frequencies of wind turbine blades with nominal powers of 100 kW, 1.5 MW, and 2.3 MW, as well as the growth of the frequency with increasing rotation speed, by establishing a multibody method. They concluded that the influence of rotation must be considered, and control strategies must be used to avoid resonance. Bachhania, K. et al. [11] performed a modal analysis and a forced vibration analysis on a wind turbine blade, using conventional Aluminum and MMC Aluminum alloys as material for the Finite Element Method, using Ansys student version software, showing that there were no critical speeds in the operating range of the analyzed turbines. Soyoz, S. et al. [12] performed a modal analysis of a 900 kW wind turbine, which, in turn, obtained graphs of buckling curves and the values of the vibration modes by performing a finite element analysis. The results showed a significant dispersion related to the different wind speeds considered, observing that the wind load has a significant effect on the determination of structural failures.

Obviously, analyzing the stresses and deformations of the blades is essential to ensuring the rotor’s structural safety. Thomas, T.T. et al. [13] proposed an “I” type spar for a 250 kW wind turbine blade, with a length of 20 m and with a S810 (NREL) profile, varying the design materials (carbon fiber and fiberglass), performing simulations in a finite element software, and obtaining their performances at the loads subjected. Eldeeb, A.E. et al. [14] studied the effect of blade stiffness change due to cracks during rotation at any speed, considering the impact of increasing centrifugal stiffness and reducing stiffness due to cracks. The authors observed that all vibration modes increased during rotation due to the effect of centrifugal stiffness. Hand, B. et al. [15] performed the structural analysis based on the finite element method of a vertical axis onshore wind turbine blade of an approximate 97 m diameter, subjecting it to critical loads, and obtaining the structural deformations within the permissible limit.

Based on the literature review, this research aims to establish a relationship between the participation factors derived from the modal analysis of a 900 W blade with the simplified load method of the IEC 61400-2 Standard [16]. This standard only establishes load hypotheses under static conditions, and it is important to take into account dynamic load conditions, which is why, in search of this relationship, scenarios are proposed that are either critical, permissible, or acceptable according to the values of the directional deformations and the participation factors. To achieve the main objective, a structural analysis is first carried out based on the fiberglass and epoxy composite material to achieve the highest mechanical performance, making a laminate configuration of the fiberglass threads, and taking two types of laminate and orientation of the fiberglass threads (uniaxial and biaxial), with a total stacking of seven layers distributed along the blade. Another important aspect addressed in this research is the vibrations in the blades of wind turbines, so a modal analysis is performed, obtaining the main vibration modes and, in turn, the participation factors corresponding to said modes. Finally, a static structural analysis is performed to study the stress concentrations (principal stresses) and deformations of a proposed wind turbine blade, layer by layer and section by section.

2. Materials and Methods

Figure 1 presents the general methodology of this research, which begins with determining the blade design variables. Subsequently, the aerodynamic design based on the BEM method is carried out, which is verified using the QBlade software based on the same BEM theory and the vortex theory. Next, the blade was modeled using the finite element method in the ACP composite materials module of the ANSYS software. Then, the modal and structural analyses are carried out in the same software, considering the Load Hypotheses of the IEC 61400-2 standard (the red arrow is a standard load). Finally, the operating scenarios are developed with the results of the analyses.

The blades studied belong to a small horizontal axis wind turbine, with a rotor radius of 0.82 m. The methodology used for the aerodynamic design of the blades is based on the BEM theory [16,17,18,19,20,21]. According to the International Standard IEC 61400-2: 2015 [16] and the specifications required for the installation site, the following design variables were considered:

• rated power, $P=900 \mathrm{W}$,
• wind speed, $v=12.5 \mathrm{m}/\mathrm{s}$,
• tip speed ratio, $\lambda =8$, and
• dynamic viscosity, $\mu =1.7\times {10}^{-5} \mathrm{k}\mathrm{g}/(\mathrm{m}·\mathrm{s})$

The selected airfoil was the SG 6043, part of a family of three profiles (SG 6041, SG 6042, and SG 6043), called primary airfoils [22]. The airfoil was chosen considering the low operating Reynolds Numbers ($Re<1\times {10}^5$).

The QBlade software (a specialized tool for designing wind turbine blades) [23] was used to compare the aerodynamic performance and results obtained from the BEM theory. This software uses the vortex theory and the BEM theory [24]. The theoretical power (the design power called by standard) of the rotor as a function of the tip speed ratio, when the tip speed ratio is $\lambda =8$, achieves 1195 W, 30% above the expected design power. This tip speed ratio value is taken because it ensures that the power remains practically constant and within the range recommended for fast wind turbines [21].

Once the blade has been designed for optimum operation, the rotor efficiency at all expected tip speed ratios must be determined. From these, the overall rotor efficiency can be determined [21]. The usual method of presenting power efficiency is the dimensionless $C_P-\lambda$ curve [25]. The power coefficient has a value approximately of 0.32, when $\lambda =8$, and the rotational speed is approximately $\mathsf{\Omega }=950 \mathrm{r}\mathrm{p}\mathrm{m}$, for the design point of this proposal.

In QBlade, the aerodynamic forces acting on a rotor can be modeled using the liftline free vortex wake (LLFVW) method. Like the BEM method, the LLFVW model calculates the blade forces using polar two-dimensional sectional airfoil data. The LLFVW model improves simulation results, especially in cases where the BEM method’s assumptions are violated. These include unsteady operation, large blade deformations, and high tip speed ratios where the turbulent wake state is approached [23]. Figure 2 shows the numerical simulation based on the line-of-lift free vortex wake (LLFVW) method obtained in QBlade. A power of $P=959 \mathrm{W}$ was obtained at a wind speed of $v=12.5 \mathrm{m}/\mathrm{s}$, and a power coefficient of $C_P=0.53$.

2.1. Material Selection

A composite material can be defined as a system of materials consisting of a mixture or combination of two or more micro or macro constituents that differ in form and chemical composition and are essentially insoluble in each other [26]. In other words, a composite material consists of a reinforcement (fibers) and a matrix (resins). The matrix transmits the loads to the fibers, which bear most of the applied load or force. It also prevents the propagation of cracks, determines the physical, electrical, and chemical properties, delimits the temperature that the composite material supports, and provides the finish and the ability of the composite material to adapt to molds. Meanwhile, reinforcement, which can take the form of fibers or particles, complements the properties that the matrix lacks. Fiber-reinforced composites, which incorporate resistant fibers in a softer and more ductile matrix, produce greater fatigue resistance and a better Young’s modulus [27].

Some of the advantages of parts made of composite materials are their physical properties, such as weight reduction, impact resistance, rigidity, the fact that they are chemically inert, thermal stability, resistance to corrosion and wear, etc. [26].

The fibers used and their arrangement determine the stiffness of the composite material made from them, their laminar proportion, and the direction of their arrangement [28]. For the above reasons, fiberglass, the most common blade material on the market, was chosen for the blade simulations. The values of Barnes et al. [29] are taken for the material’s physical properties in the simulation, where the authors perform a structural analysis on wind turbine blades. These magnitudes of the physical properties are shown in

Table 1. Physical properties of epoxy fiberglass [29].

Property		±45° Angle Ply Glass/Epoxy	Unidirectional Glass/Epoxy
$E_1$	Longitudinal modulus, GPa	25	39
$E_2$	Transverse modulus, GPa	25	8.3
$E_3$	Transverse modulus, GPa	18	8.3
$G_{12}$	Shear modulus, GPa	6.3	4.1
${\nu }_1$	Poisson’s ratio	0.38	0.26
${\overline{\sigma }}_{1t}$	Tensile strength, MPa	511	1062
${\overline{\sigma }}_{1c}$	Compressive strength, MPa	628	610
${\overline{\sigma }}_{2t}$	Tensile strength, MPa	511	31
${\overline{\sigma }}_{2c}$	Compressive strength, MPa	628	118
${\overline{\sigma }}_{3t}$	Tensile strength, MPa	28	31
${\overline{\sigma }}_{3c}$	Compressive strength, MPa	138	118
${\overline{\tau }}_{12}$	In plane shear strength, MPa	790	72
$\rho$	Density, kg/m3	1900	1900

.

Fiberglass is a common type of fiber used for reinforcement. It can be found in the form of threads without any orientation or in arrangements as if they were a grid, where the fibers can be oriented at 0°, ±45°, or ±90°. These forms are also known as unidirectional, bidirectional, and tridirectional arrangements. The unidirectional or uniaxial are represented as threads in one direction only, the bidirectional or biaxial are seen as interlaced or woven in two directions, and the tridirectional or triaxial are found oriented in the form of a braid, usually found as −45°, +45°, and 90° [30].

2.2. Simple Model in FEM

The blade was modeled hollow, with biaxial fiberglass with a thickness of 0.6 mm; for the uniaxial, the thickness corresponds to 0.7 mm [29]. The boundary conditions in the blade embedded in the root were considered, and the simplified load method of the international standard IEC 61400-2 was applied. Regarding the FEM simulation, the dominant type of element is hexahedron, with a total of 1,482,972 elements and an average mesh size of 3 mm. To verify the mesh quality, Figure 3 shows the mesh convergence graph (element size vs. total deformation) of the simulation of hypothesis A, Fz of the first intrados layer. Figure 4 shows the relative percentage error (element size vs. relative percentage error) in which it can be verified that this parameter was below 0.5% with mesh sizes from 5 to 0.8 mm, a parameter that remained in the same range in all cases of simulation of the load hypotheses. Figure 5 shows details of the model mesh in the root zone. The results of the load hypotheses are shown in

Table 2. Wind turbine blade stresses obtained from the simplified load method (load hypothesis) of IEC 61400-2 International Standard.

Load Hypothesis		Stress (MPa)
		Maximum Principal	Von Mises
FAz	Force in z	37.67	33.75
MAx	Moment in x	1.59	1.03
MAy	Moment in y	2.69	1.96
FEz	Force in z	30.86	27.65
MBy	Moment in y	0.85	0.98
MCy	Moment in y	415.27	300.72
MHy	Moment in y	158.64	140.32

.

Figure 6 shows the relationship between the coordinate systems used in the IEC 61400-2 standard and the finite element software to clarify the simulation results.

2.3. FEM Simulation Software for Composite Materials

In order to correctly set up an FEM (Finite Element Method) simulation using composite materials, it is necessary to consider their composite nature, i.e., the directionality of the mechanical properties and the need to define the laminates. The Ansys Composite PrepPost (ACP) software is a tool for modeling composite laminates (Pre). It allows to generate FEM models with different lamination regions defined layer by layer, as well as correctly determining the stacking sequences to cover the entire structure [31].

2.4. Setting up Fiberglass Layers in the Software

The blade design proposes a configuration consisting of seven layers (one uniaxial layer and six biaxial layers) distributed along its length, which is approximately 82 cm. The uniaxial layer is exposed to the elements, and the remaining biaxial layers are distributed toward the interior of the blade geometry. The blade geometry is divided into five parts or sections (as shown in Figure 7, root, joint, body, tip, and edges), so the configurations of the fiberglass fabric layers are easily adapted and located. Also, according to the wing profile, the blade is divided into extrados and intrados. The root and joint sections have seven layers (one uniaxial and six biaxial). The body part of the blade has four layers (one uniaxial and three biaxial). The tip part has two cumulative layers (one uniaxial and one biaxial). As for the edge section (see detail in Figure 7), the number of layers depends on which section the edge is located. The configuration of the fiberglass fabrics is shown in

Table 3. Fiberglass layer configuration on the blade.

Element Sets	Stack-Up (Layer Configuration)	Fabric Type (Fiberglass)
Root	Seven layers	One Uniaxial/six Biaxial
Joint	Seven layers	One Uniaxial/six Biaxial
Body	Four layers	One Uniaxial/three Biaxial
Tip	Two layers	One Uniaxial/one Biaxial

.

2.5. Modal Analysis

All wind turbine blade prototypes undergo an experimental test procedure as part of the blade design and manufacturing process to ensure they meet the actual design requirements. In addition to the experimental tests comprising normal and extreme load capacity tests and fatigue strength tests, it is common practice to complement them with tests of the blades’ basic dynamic properties, such as natural frequencies and damping properties, as these are essential for the dynamic behavior and structural integrity of the entire wind turbine [32].

In the modal analysis, no excitations or loads external to the structure are needed. Therefore, the blade is assumed to be a cantilever with a single fixed support at the root (Figure 8), simulating and calculating the blade’s natural frequencies and participation factors [33].

2.6. IEC 61400-2 International Standard

The objective of the IEC 61400-2 standard is to provide guidelines for small horizontal-axis wind turbines (swept areas less than 200 m²). It addresses requirements for this type of wind turbine (quality, safety, design, etc.). The design loads of the standard must be obtained using one or a combination of three methodologies: (1) the simplified load methodology, (2) the Simulation model, and (3) the Real load model. The simplified load methodology is a limited set of load hypotheses with direct formulas and simplified external conditions. These hypotheses are the load hypothesis A (normal operation), which refers to fatigue loads; the load hypothesis B (orientation), which deals with rotational moments and forces; load hypothesis C (orientation error); the load hypothesis E (maximum rotation speed); and finally, the load hypothesis H (extreme wind load).

To apply this methodology, certain requirements must be met in the configuration of the wind turbine, which are as follows: it must have a horizontal axis, it must have cantilever blades, a fixed hub, the rotor must have two or more blades, the rotor can be upwind or downwind with constant or variable speed, and it must have a fixed pitch. Since the blade and rotor designed in this research meet the requirements above and this methodology does not consider dynamic loads, it was selected for the study.

3. Results

3.1. Modal Simulation and Analysis in FEM

Under the modal analysis configuration, a maximum number of vibration modes can be specified. In this case, once the initial conditions for the modal analysis were established, 15 vibration modes were determined. Figure 9 shows the deformation due to the first vibration mode (13.24 Hz).

Figure 10 shows the natural frequencies of the blade’s 15 vibration modes, which occur between 13 Hz and 934 Hz. The first vibration mode is the main one, and the following are combinations of the previous ones [33].

In modal analysis, the participation factor is the amount of mass moving in the same direction as the excitation (${\gamma }_i$); see Equation (1).

$${\gamma }_i={\left\{\varphi \right\}}_i^T\left[M\right]\left\{D\right\}$$

(1)

where $\varphi$ is the transpose of the vibration mode, $M$ is the mass matrix $m$, and $D$ is the excitation direction vector [34].

In addition to knowing the natural frequencies of the blade, it is important to know in which direction the participation factor is most relevant in each vibration mode. The above is done to determine whether the participation factor of a vibration mode on a particular axis coincides with the axis where a load hypothesis of the standard is applied. This is to determine possible critical deformation and failure scenarios.

The resulting participation factors per coordinate axis ($x$, $y$, and $z$) corresponding to each of the 15 vibration modes are shown in Figure 11. Each participation factor is calculated in each of the coordinate axes. The negative sign in some of the participation factors is that they are contrary to the direction in the reference axis.

In Figure 11 and Figure 12, the participation factors resulting from the modal analysis of the blade can be observed. In both graphs, the axis with the minimum values of the participation factors is the z-axis compared to the x- and y-axes. In Figure 12, the magnitudes of the factors tend to decrease as the natural frequency increases. The most significant factors are found among the first eight vibration modes.

Figure 12 illustrates that, with respect to the x-axis, the participation factor’s maximum value occurs in the third vibration mode, and its minimum value occurs in the sixth vibration mode. For the y-axis, the participation factor’s maximum value occurs in the first vibration mode, and the factor’s minimum value is found in the second vibration mode.

3.2. Structural Analysis According to IEC 61400-2 by Using FEM Software

Before the structural simulation in the FEM software, the magnitudes of the load hypotheses are calculated according to the IEC 61400-2 Standard, verifying that the derived stresses comply with the minimum safety factor established by the Tsai Wu failure theory [35]. The load hypotheses are simulated, and the principal maximum deformations and stresses per section and fiberglass layer are obtained.

Figure 13 shows, applying load hypothesis A, the deformations in the following: Figure 13a: the total deformation, Figure 13b: the directional deformation on the x-axis, Figure 13c: the directional deformation on the y-axis, and Figure 13d: the directional deformation on the z-axis.

Table 4. Wind turbine blade deformation under different load hypotheses.

Load Hypothesis 1		Directional Deformation (m)
		$\mathit{x}$	$\mathit{y}$	$\mathit{z}$	Total
1	AFz	0.02042	0.00010	0.00068	0.02078
2	AMx	0.01799	0.00001	0.00022	0.01814
3	AMy	0.00008	0.00786	0.00027	0.01329
4	BMy	0.00016	0.01522	0.00052	0.00027
5	CMy	0.00150	0.08585	0.00178	0.15634
6	EFz	0.01673	0.00008	0.00055	0.01703
7	HMy	0.00187	0.10658	0.00221	0.19410

¹ The first letter refers to the type of load hypothesis, the second letter is F if it is a force or M if it is a moment, and the third letter refers to the coordinate axis with respect to where the load hypothesis is applied.

shows the directional and total deformations by load hypothesis, observing that the most critical deformations occur when applying hypotheses C and H, respectively. Considering the following terminology: the first letter refers to the hypothesis, and the second letter refers to “$F$” if it is a force and “$M$” if it is a moment. Finally, the last letter indicates the axis to which the hypothesis will be applied.

Figure 14, Figure 15, Figure 16, Figure 17, Figure 18, Figure 19, Figure 20, Figure 21, Figure 22, Figure 23, Figure 24, Figure 25, Figure 26 and Figure 27 show the magnitude and position of the von Mises stress (MPa) in each section of the blade (root, joint, body, and tip) and each fiberglass layer, both in the intrados (layers 1, 2, 3, 4, 5, 6, 7) and in the extrados (layer 1, 2, 3, 4, 5, 6, and 7). Considering the application of each of the seven load hypotheses in Table 1 (these values are obtained with the FEM software). The intention is to analyze and identify the critical structural positions and scenarios of the blade. The nomenclature indicated in the upper right corner of each graph details the part of the blade, whether intra for the intrados or extra for the extrados. The letter “L,” followed by a number, refers to the layer number. The syllable “UNI” or “BI” designates the type of layer: “UNI” if the layer is uniaxial and “BI” if it is biaxial. The grades described refer to the orientation of the threads of the fiberglass layers.

Figure 14. Von Mises stresses vs. blade section: Load Hypothesis A, $F_Z=4799.7 \mathrm{N}$ (intrados side).

Figure 14. Von Mises stresses vs. blade section: Load Hypothesis A, $F_Z=4799.7 \mathrm{N}$ (intrados side).

In Figure 14, Load Hypothesis A is applied, with force on the z-axis of $4799.7 \mathrm{N}$ in each of the layers in the intrados side. This figure shows that the stress values reach their maximum in the joint and body areas, while the rest of the layers reach their maximum in the area where they end. The inner layer (intra-L7) reaches its maximum value in the joint area. The intra-L4 layer in the body area presents the maximum stress value in the entire blade. Of the two layers, Intra L1 and Intra L2, that cover all sections of the blade, the latter, which is the outermost, presents the most significant stresses in all sections. Based on the above, it is concluded that with this hypothesis and in the intrados, the outer layers are subjected to the greatest stresses.

Figure 15. Von Mises stresses vs. blade section: Load Hypothesis A, $F_Z=4799.7 \mathrm{N}$ (extrados side).

Figure 15. Von Mises stresses vs. blade section: Load Hypothesis A, $F_Z=4799.7 \mathrm{N}$ (extrados side).

Figure 15 shows the maximum stress values in the joint area, with the inner layer (extra-L7) being the layer that presents the maximum stress value along the entire blade, applying the Load Hypothesis A, with a force on the z-axis of $4799.7 \mathrm{N}$, in each of the fiberglass layers that comprise the extrados side. Of the two layers covering all the blade sections, Extra L1 and Extra L2, the latter, which is the outermost, presents the most significant stresses in all the sections. It is worth noting that this layer presents greater stresses in the body area and is even greater than in the first four layers of the joint area. Based on the above, it is concluded that this hypothesis and the extrados subject the Extra L2 layer (internal to the joint and body areas) to more significant stresses.

Figure 16. Von Mises stresses vs. blade section: Load Hypothesis A, $M_X=7.22 \mathrm{N}·\mathrm{m}$ (intrados side).

Figure 16. Von Mises stresses vs. blade section: Load Hypothesis A, $M_X=7.22 \mathrm{N}·\mathrm{m}$ (intrados side).

As can be seen in Figure 16, when applying the Load Hypothesis A with a moment on the x-axis of $7.22 \mathrm{N}·\mathrm{m}$, the stress values in each layer of the intrados side reach their maximum in the joint and body areas, while the rest of the layers reach their maximum in the area where they end. The inner layer (intra-L4) reaches its maximum value in the body area, presenting the maximum stress value throughout the blade.

The outer layer, Intra L7, in the joint zone reaches the maximum stress of the section. The outer layer, Intra L4, in the body zone reaches the highest stress of the section and all the sections. Of the two layers covering all the blade sections, Intra L1 and Intra L2, the latter and outermost layer presents the highest stresses in all the sections. This layer presents higher stresses in the body zone and is even higher than in the first five layers of the joint zone. Based on the above, it is concluded that, according to this hypothesis and in the intrados, the Intra L2 layer (internal in the joint and body zones) is subjected to the highest stresses.

Figure 17. Von Mises stresses vs. blade section: Load Hypothesis A, $M_X=7.22 \mathrm{N}·\mathrm{m}$ (extrados side).

Figure 17. Von Mises stresses vs. blade section: Load Hypothesis A, $M_X=7.22 \mathrm{N}·\mathrm{m}$ (extrados side).

In Figure 17, with the Load Hypothesis A, applied with a moment on the x-axis of $7.22 \mathrm{N}·\mathrm{m}$, each of the fiberglass layers of the extrados side shows that the fiberglass layers that make up the blade have maximum stress values in the joint and body areas. In contrast, the rest of the layers reach their maximum stress in the area where they end. The inner layer (extra-L4) reaches its maximum value in the body area, presenting the maximum stress value throughout the blade. From the above, it is concluded that with this hypothesis and in the extrados, the Extra L2 layer (internal in the union zone and the body zone) is the one that is subjected to more significant stresses.

Figure 18. Von Mises stresses vs. blade section: Load Hypothesis A, $M_Y=32.52 \mathrm{N}·\mathrm{m}$ (intrados side).

Figure 18. Von Mises stresses vs. blade section: Load Hypothesis A, $M_Y=32.52 \mathrm{N}·\mathrm{m}$ (intrados side).

Figure 18 illustrates that the values reach their maximum in the joint and body areas, while the rest of the layers reach their maximum in the area where they end. The inner layer (intra-L4) reaches its maximum value in the body area. It presents the maximum stress value in the entire blade applying Load Hypothesis A, with a moment on the y-axis of $32.52 \mathrm{N}·\mathrm{m}$ in each of the fiberglass layers comprising the intrados. From the above, it is concluded that, with this hypothesis and in the intrados, the Intra L2 layer (internal in the union zone and the body zone) is subjected to more significant stresses.

Figure 19. Von Mises stresses vs. blade section: Load Hypothesis A, $M_Y=32.52 \mathrm{N}·\mathrm{m}$ (extrados side).

Figure 19. Von Mises stresses vs. blade section: Load Hypothesis A, $M_Y=32.52 \mathrm{N}·\mathrm{m}$ (extrados side).

As illustrated in Figure 19, the Load Hypothesis A is applied with a moment on the y-axis of $32.52 \mathrm{N}·\mathrm{m}$ in each fiberglass layer comprising the extrados side. The stress values reach their maximum in the joint and body areas, while the rest of the layers reach their maximum in the area where they end. The inner layer (extra-L4) reaches its maximum value in the body area, presenting the maximum stress value throughout the blade. From the above, it is concluded that with this hypothesis and in the extrados, the Extra L2 layer (internal in the union zone and the body zone) is the one that is subjected to more significant stresses.

Figure 20. Von Mises stresses vs. blade section: Load Hypothesis B, $M_Y=62.93 \mathrm{N}·\mathrm{m}$ (intrados side).

Figure 20. Von Mises stresses vs. blade section: Load Hypothesis B, $M_Y=62.93 \mathrm{N}·\mathrm{m}$ (intrados side).

In Figure 20, Load Hypothesis B is applied with a moment on the y-axis of $62.93 \mathrm{N}·\mathrm{m}$ in each fiberglass layer comprising the intrados side. The stress values reach their maximum in the joint and body areas, while the rest of the layers reach their maximum in the area where they end. The inner layer (intra-L4) reaches its maximum value in the body area, presenting the maximum stress value throughout the blade. From the above, it is concluded that with this hypothesis and in the intrados, the Intra L2 layer (internal in the union zone and the body zone) is the one that is subjected to more significant stresses.

Figure 21. Von Mises stresses vs. blade section: Load Hypothesis B, $M_Y=62.93 \mathrm{N}·\mathrm{m}$ (extrados side).

Figure 21. Von Mises stresses vs. blade section: Load Hypothesis B, $M_Y=62.93 \mathrm{N}·\mathrm{m}$ (extrados side).

Figure 21 illustrates the Von Mises stress (MPa) value vs. blade section by applying the Load Hypothesis B with a moment on the y-axis of $62.93 \mathrm{N}·\mathrm{m}$ in each of the fiberglass layers comprising the extrados side. It can be observed that the fiberglass layers that make up the blade from the root to the tip reach their maximum stresses in the joint and body areas, while the rest of the layers reach their maximum stresses in the area where they end. The inner layer (extra-L4) reaches its maximum value in the body area, presenting the maximum stress value throughout the blade. From the above, it is concluded that with this hypothesis and in the intrados, the Extra L2 layer (internal in the union zone and in the body zone) is the one that is subjected to more significant stresses.

Figure 22. Von Mises stresses vs. blade section: Load Hypothesis C, $M_Y=4894.36 \mathrm{N}·\mathrm{m}$ (intrados side).

Figure 22. Von Mises stresses vs. blade section: Load Hypothesis C, $M_Y=4894.36 \mathrm{N}·\mathrm{m}$ (intrados side).

Figure 22 illustrates the value of the Von Mises stress (MPa) vs. blade section, applying the C load hypothesis with a moment on the y-axis of $4894.36 \mathrm{N}·\mathrm{m}$ in each of the fiberglass layers that comprise the intrados side. It can be observed that the fiberglass layers that make up the blade from the root to the tip reach their maximum stresses in the joint and body areas, while the rest of the layers reach their maximum stresses in the area where they end. The inner layer (intra-L4) reaches its maximum value in the body area, presenting the maximum stress value throughout the blade. From the above, it is concluded that, with this hypothesis and in the intrados, the Intra L2 layer (internal in the union zone and in the body zone) is subjected to more significant stresses.

Figure 23. Von Mises stresses vs. blade section: Load Hypothesis C, $M_Y=4894.36 \mathrm{N}·\mathrm{m}$ (extrados side).

Figure 23. Von Mises stresses vs. blade section: Load Hypothesis C, $M_Y=4894.36 \mathrm{N}·\mathrm{m}$ (extrados side).

Figure 23 illustrates the Von Mises stress (MPa) value vs. blade section applying the Load Hypothesis C, with a moment on the y-axis of $4894.36 \mathrm{N}·\mathrm{m}$, in each of the fiberglass layers comprising the extrados side. It can be observed that the fiberglass layers that make up the blade from the root to the tip reach their maximum stresses in the joint and body areas, while the rest of the layers reach their maximum stresses in the area where they end. The inner layer (extra-L4) reaches its maximum value in the body area, presenting the maximum stress value throughout the blade. From the above, it is concluded that with this hypothesis and in the intrados, the Extra L2 layer (internal in the union zone and in the body zone) is the one that is subjected to greater stresses.

Figure 24. Von Mises stresses vs. blade section: Load Hypothesis E, $F_Z=3931.93 \mathrm{N}$ (intrados side).

Figure 24. Von Mises stresses vs. blade section: Load Hypothesis E, $F_Z=3931.93 \mathrm{N}$ (intrados side).

Figure 24 illustrates the Von Mises stress (MPa) value vs. blade section by applying the E load hypothesis with a force in the z-axis of $3931.93 \mathrm{N}$ in each of the fiberglass layers comprising the intrados. It can be observed that the fiberglass layers that make up the blade from the root to the tip reach their maximum stresses in the joint and body areas, while the rest of the layers reach their maximum stresses in the area where they end. The inner layer (intra-L4) reaches its maximum value in the body area, presenting the maximum stress value throughout the blade. From the above, it is concluded that, according to this hypothesis, the Intra L3 layer (internal in the union zone) is subjected to greater stresses in the intrados.

Figure 25. Von Mises stresses vs. blade section: Load Hypothesis E, $F_Z=3931.93 \mathrm{N}$ (extrados side).

Figure 25. Von Mises stresses vs. blade section: Load Hypothesis E, $F_Z=3931.93 \mathrm{N}$ (extrados side).

As illustrated in Figure 25, the value of the Von Mises Stress (MPa) vs. blade section when applying the Load Hypothesis E with a force in the z-axis of $3931.93 \mathrm{N}$ are shown for each of the fiberglass layers that comprise the extrados side. It can be observed that the fiberglass layers that make up the blade from root to tip reach their maximum stresses in the joint and body areas, while the rest of the layers reach their maximum stresses in the area where they conclude. The inner layer (extra-L4) reaches its maximum value in the body area, presenting the maximum stress throughout the blade. From the above, it is concluded that the Extra L2 layer (internal in the union zone and the body zone) is subjected to greater stresses with this hypothesis and in the intrados.

Figure 26. Von Mises stresses vs. blade section: Load Hypothesis H, $M_Y=3042.69 \mathrm{N}·\mathrm{m}$ (intrados side).

Figure 26. Von Mises stresses vs. blade section: Load Hypothesis H, $M_Y=3042.69 \mathrm{N}·\mathrm{m}$ (intrados side).

Figure 26 illustrates the Von Mises Stress (MPa) value vs. blade section applying the H load hypothesis with a moment on the y-axis of $3042.69 \mathrm{N}·\mathrm{m}$ in each fiberglass layer comprising the intrados side. It can be observed that the fiberglass layers that make up the blade from root to tip reach their maximum stresses in the junction and body areas, while the rest of the layers reach their maximum stresses in the area where they end. The inner layer (intra-L4) reaches its maximum value in the body area, presenting the maximum stress value throughout the blade. From the above, it is concluded that with this hypothesis and in the intrados, the Intra L2 layer is the one that is subjected to greater stresses.

Figure 27. Von Mises stresses vs. blade section: Load Hypothesis H, $M_Y=3042.69 \mathrm{N}·\mathrm{m}$ (extrados side).

Figure 27. Von Mises stresses vs. blade section: Load Hypothesis H, $M_Y=3042.69 \mathrm{N}·\mathrm{m}$ (extrados side).

Figure 27 illustrates the Von Mises stress (MPa) value vs. blade section by applying the y-axis moment load hypothesis H of $3042.69 \mathrm{N}·\mathrm{m}$ to each of the fiberglass layers comprising the extrados side. It can be observed that the fiberglass layers that make up the blade from the root to the tip reach their maximum stresses in the joint and body areas, while the rest of the layers reach their maximum stresses in the area where they end. The inner layer (extra-L4) reaches its maximum value in the body area, presenting the maximum stress value throughout the blade. From the above, it is concluded that, according to this hypothesis, the Extra L2 layer is subjected to greater stresses in the intrados.

Table 5. Summary of von Mises stresses for each Hypothesis, layer, and blade section.

			Von Mises Stress (MPa)
	Layer		Intrados				Extrados
Hypothesis	No	Type	Root	Union	Body	Tip	Root	Union	Body	Tip
AFz	1	Uniaxial	0	39.67	39.72	3.03	0	32.15	30.22	2.52
	2	Biaxial	0	61.98	77.72	5.50	0	57.35	61.27	3.92
	3	Biaxial	0	64.49	84.15		0	48.98	52.94
	4	Biaxial	0	50.23	99.88		0	36.25	57.41
	5	Biaxial	0	50.21			0	43.01
	6	Biaxial	0	59.99			0	62.62
	7	Biaxial	0	86.86			0	65.91
AMx	1	Uniaxial	0	2.84	3.39	0.10	0	1.88	2.10	0.10
	2	Biaxial	0	3.99	4.83	0.19	0	2.74	3.30	0.20
	3	Biaxial	0	3.62	3.71		0	2.24	3.25
	4	Biaxial	0	2.10	5.58		0	1.90	4.46
	5	Biaxial	0	2.69			0	1.86
	6	Biaxial	0	2.93			0	3.00
	7	Biaxial	0	4.32			0	2.64
AMy	1	Uniaxial	0	12.81	0.15	0.46	0	8.47	9.45	0.43
	2	Biaxial	0	17.95	21.78	0.86	0	12.34	14.86	0.88
	3	Biaxial	0	16.30	16.73		0	10.09	14.63
	4	Biaxial	0	9.45	25.15		0	8.54	20.11
	5	Biaxial	0	12.11			0	8.37
	6	Biaxial	0	13.20			0	13.52
	7	Biaxial	0	19.47			0	11.90
BMy	1	Uniaxial	0	22.10	26.09	0.77	0	15.01	16.70	0.72
	2	Biaxial	0	30.85	37.66	1.52	0	21.87	26.22	1.46
	3	Biaxial	0	28.37	20.03		0	17.79	26.60
	4	Biaxial	0	16.47	45.75		0	15.86	36.59
	5	Biaxial	0	22.44			0	15.61
	6	Biaxial	0	23.97			0	25.20
	7	Biaxial	0	36.24			0	22.24
CMy	1	Uniaxial	0	142.88	160.25	2.88	0	110.75	122.86	2.63
	2	Biaxial	0	249.18	242.91	6.05	0	163.80	216.50	5.33
	3	Biaxial	0	189.01	234.59		0	127.63	223.09
	4	Biaxial	0	139.75	373.47		0	145.93	306.16
	5	Biaxial	0	206.72			0	146.34
	6	Biaxial	0	215.19			0	236.03
	7	Biaxial	0	339.89			0	211.18
EFz	1	Uniaxial	0	29.01	29.05	2.21	0	23.53	22.11	1.84
	2	Biaxial	0	45.30	56.81	4.01	0	41.96	44.79	2.86
	3	Biaxial	0	47.14	61.52		0	35.78	38.67
	4	Biaxial	0	36.72	73.03		0	26.48	41.97
	5	Biaxial	0	36.72			0	31.43
	6	Biaxial	0	43.86			0	45.80
	7	Biaxial	0	63.55			0	48.22
HMy	1	Uniaxial	0	1068.50	1261.60	37.33	0	725.72	807.32	34.65
	2	Biaxial	0	1491.90	1821.00	73.40	0	1057.60	1267.70	70.79
	3	Biaxial	0	1371.60	1355.50		0	860.03	1286.10
	4	Biaxial	0	796.47	2212.10		0	766.77	1769.31
	5	Biaxial	0	1084.80			0	754.52
	6	Biaxial	0	1159.10			0	1218.30
	7	Biaxial	0	1752.10			0	1075.30
				2212.10	191.41	0.10
				Max	Mid	Min

summarizes the von Mises stresses by load hypothesis, layer, and section or zone of the blade. The table reveals that the load hypotheses that generate the most significant stresses in the blade are hypothesis C (orientation error) and hypothesis H (extreme wind load). In load hypothesis C, the highest stresses are located in the fourth layer of the intrados in the body zone (373.47 MPa), followed in order of magnitude by the stress of the seventh layer of the intrados in the joint zone (339.89 MPa) and the stress of the fourth layer of the extrados in the body zone (306.16 MPa). In hypothesis H, the highest stresses in the blade are recorded in the fourth layer of the intrados in the body area (2212.10 MPa), followed in order of magnitude by the stress in the second layer of the intrados in the body area and the stress in the fourth layer of the extrados in the body area (1769.31 MPa). A very close value of 1752.10 MPa is observed in the seventh layer of the intrados in the root area. The average stress value was 191.41 MPa, and the minimum value was 0.1 MPa, found in the blade tip area.

4. Discussion

Table 5 shows the relationship between the participation factors and the load hypotheses of the IEC 61400-2 Standard. The load hypotheses are listed in the rows, and the vibration modes are listed in the columns. The purpose of the table is to establish critical, acceptable, and permissible structural scenarios. A critical scenario occurs when the magnitude of the participation factor is maximum in a specific coordinate axis that is aligned with the axis of the maximum deformation, applying a load hypothesis on the blade.

For example, when load hypothesis A is applied, with load F along the z-axis (first row of Table 5), and the maximum deformation is found to be on the x-axis, and the participation factor reaches its maximum on the x-axis, then there will be a critical scenario. The acceptable scenario occurs when the magnitude of the participation factor is the average value of the magnitudes in the three coordinate axes, and it is aligned with the coordinate axis of the maximum deformation, applying a load hypothesis. Finally, a permissible scenario occurs when the magnitude of the participation factor is the minimum value in the three coordinate axes and is aligned with the coordinate axis of the maximum deformation by applying a load hypothesis. Thus, the orange color corresponds to a critical scenario, the yellow color corresponds to an acceptable scenario, and finally, the green color corresponds to a permissible scenario.

Since the maximum deformation occurs on the x-axis in all the load hypotheses of the IEC-61400-2 Standard, the scenarios are constant in each vibration mode. As can be seen in

Table 6. Comparison of the participation factors Scenarios for each load hypothesis applied to a wind turbine blade. —Permissible scenario; —Acceptable scenario; —Critical scenario.

Load Hypotheses	Vibration Mode	1	2	3	4	5	6	7	8	9	10	11	12	13	14	15
	Natural Frequencies (Hz)	13.4	48.3	78.3	127.3	209.9	280.0	339.3	360.2	470.2	587.3	604.6	706.6	780.3	834.1	933.3
A Fz
A Mx
A My
B My
C My
E Fz
H My

, the critical scenarios are found in vibration modes 2, 3, 5, 6, 10, 12, and 14, applying all the load hypotheses; the acceptable scenarios occur in vibration modes 1, 8, and 13. Finally, the permissible scenarios occur in vibration modes 4, 7, 9, 11, and 15. It is important to mention that according to Table 5, it can be concluded that in the first six vibration modes at low natural frequencies (<280 Hz), there are more critical scenarios (four of six), one acceptable scenario, and one permissible scenario. In contrast to the following vibration modes with high natural frequencies (>300 Hz), where fewer critical scenarios occur (three out of nine), two acceptable scenarios, and four permissible scenarios predominate.

5. Conclusions

The importance of this research is that structural load scenarios are proposed and analyzed by relating the load hypotheses established by the IEC 61400-2 standard and the blade participation factors obtained from the modal simulation in FEM.

The results obtained show that at low vibration frequencies more critical load scenarios can occur, so they must be considered in these operating conditions. The configuration of the fiberglass layers, in terms of their direction and length, plays a very important role in the design of the blade.

For the particular blade studied, the most critical values of the maximum principal stresses occur in the body section. The maximum stress values for each section appear at the end of the length of the layers, so leaving the first layer a little longer, exceeding the size of its corresponding section, should be considered in order to avoid a concentration of stresses at the end of each section of the blade.

According to the standard, the critical load scenarios are extreme wind loads and orientation errors. From the point of view of stresses, the critical fiberglass layer was the second internal layer for both the extrados and the intrados, which indicates that the internal stresses are very relevant throughout the blade and in all hypotheses. On the other hand, the stresses in the fourth layer, both on the intrados and extrados, are the most important throughout the blade, reaching their maximum when it becomes an external layer in the body area. The stresses in the blade are the result of a combination of internal stresses throughout the blade that are more or less uniform and of significant extreme external stresses on the surface.

To complement this research, the analysis and fatigue tests on the blade will be carried out as future work following the parameters of the standard, comparing the life cycles resulting from said analysis and tests, with the main stresses and stiffness of the fiberglass.