Simulation-Based Assessment of Vibration Effects on IGBT Module Lifetime in Wind Turbines Through Modal and Random Vibration Analysis

Abstract

This study explores the effect of vibrations generated by wind turbines on the lifespan of the IGBT module. Since wind turbines operate under varying dynamic loads, they produce vibrations that might influence the performance and longevity of electronic components like IGBTs. To investigate this concern, a modal analysis was carried out using the finite element analysis (FEA) in ANSYS to identify the natural frequencies of the module. These frequencies were then compared with typical load frequencies encountered in wind turbine operations. Furthermore, random vibration analysis, incorporating power spectral density (PSD), was conducted to assess the module’s deformation under stochastic vibration conditions. The simulation results demonstrated that the IGBT module located inside the wind turbine nacelle has an exceptionally long operational lifetime under random vibration conditions. This indicates that the impact of vibrations on the module’s durability is minimal. As a result, this study concludes that vibrations induced by wind turbine operations pose no significant threat to the lifespan of the IGBT module, reinforcing its reliability in power electronic systems, even in vibration-prone environments.

1. Introduction

Power electronic systems are essential in fields like renewable energy, aerospace, and electric vehicles because they offer high efficiency and precise control [1,2]. Despite their advantages, these systems often face reliability challenges in harsh environments. Among their critical components are power semiconductor devices, particularly insulated gate bipolar transistors (IGBTs), which are highly effective but also vulnerable to failure [3]. To enhance system reliability, it is crucial to understand how real-world stresses affect these components and to develop models that predict their lifespan.

According to industry-focused surveys [4,5], semiconductor switches and capacitors are the components in power converters most prone to failure. Random failures are primarily attributed to unexpected overloads and system transients. In contrast, long-term wear-out failures are predominantly caused by thermal stresses, mechanical vibrations, and humidity. In recent years several research works have been conducted to investigate the impact of thermal stresses on the lifespan of IGBTs. Reference [6] highlights the differences in power cycling test results between DC and switching modes, focusing on thermal stresses in IGBT power modules, particularly bond-wire contacts and interconnections. It was found that, under identical $\Delta T_j$ conditions, the higher load current in DC mode induces greater thermal stress on bond wires compared to switching mode, resulting in slightly higher local $\Delta T$ and reduced lifetime. A thermal fatigue feedback loop method has been suggested in [7] to assess the lifetime of an IGBT module, considering the cumulative impact of solder-layer fatigue. A three-dimensional (3D) finite element method (FEM) model is developed for the IGBT module, and, combined with accelerated aging experiments, it highlights the significance of the accumulated thermal resistance increase in thermal network modeling and lifetime evaluation. The Cauer thermal network is then enhanced to create the fatigue feedback loop model, incorporating the effects of solder-layer fatigue to better estimate the power module’s lifetime.

As mentioned, power cycling and thermal stress failure mechanisms have been thoroughly researched, while the impact of vibrational stress on IGBT modules is still not well-understood and warrants further exploration. Bridging this knowledge gap is essential for enhancing the design and performance of IGBT modules in practical applications. Vibrations, which can originate from diverse sources, may manifest as either random or harmonic. In addition, in real-world environments, vibrations typically exhibit a random nature [8].

In the aviation, wind turbines, and automotive industries, numerous products are subjected to vibrational conditions during operation. Among these environments, simple harmonic vibrations represent the most basic form, while random vibrations are the most prevalent [9]. Simple harmonic vibration represents the most fundamental type of vibration, as any periodic vibration can be constructed by combining multiple simple harmonic vibrations. In contrast, random vibration is the most intricate form, requiring probabilistic methods for analysis. Random vibration analysis, often referred to as power spectral density (PSD) analysis, is a spectral analysis technique grounded in probability and statistics. It converts time-history statistical samples into a power spectral density representation [8].

The main contributions of this paper are as follows:

• Modal analysis was performed on the IGBT module to determine its natural frequencies. These identified frequencies were then compared with the vibration frequencies present within the wind turbine nacelle to evaluate potential resonance effects. By assessing this, the risk of vibration-induced damage to the IGBT module and its components can be effectively monitored and mitigated;
• Random vibration analysis was conducted to assess the module’s response to unpredictable and fluctuating vibration environments, providing a more comprehensive understanding of its dynamic behavior. To carry out this analysis, finite element analysis (FEA) using ANSYS 2023 R1 was utilized to simulate the vibrational forces acting on the IGBT module, allowing for a detailed examination of its structural response under varying conditions. This approach ensures a more accurate prediction of the module’s performance and potential vulnerabilities to dynamic forces;
• The deformation pattern, lifetime, and damage distribution of the IGBT module were analyzed using ANSYS simulation tools to assess the impact of vibration on the module’s lifespan. This analysis provided insights into how the vibrational forces within the wind turbine nacelle affect the IGBT module, helping to predict potential failure points and optimize its design for enhanced durability and performance in such dynamic environments.

The structure of this paper is organized as follows. Section 2 covers our changes to the modal analysis, while Section 3 focuses on the random vibration analysis. In Section 4, the load frequencies in a wind turbine are discussed. Section 5 provides details on how to model the IGBT module in ANSYS. The simulation results are presented in Section 6, and, finally, Section 7 concludes the paper by summarizing key findings.

2. Modal Analysis and Natural Frequencies

The definition and formulation of modal analysis are described as follows.

2.1. Definition

Modal analysis is a common technique for characterizing the dynamic behavior of a structure through its modal parameters, including natural frequency, damping factor, modal mass, and mode shape. This analysis can be conducted either experimentally or mathematically [10]. In mathematical modal analysis, the goal is to decouple the structural equations of motion, allowing each equation to be solved independently. When exact solutions are not feasible, numerical methods like finite-element or boundary-element approaches are employed to approximate the results. In experimental modal testing, the structure is excited by applying a measured force at one or more points, and the resulting responses are recorded at specific locations. These measurements are used to develop frequency response functions.

Natural frequencies and mode shapes are two key aspects of modal analysis. Natural frequencies are the precise frequencies at which an item vibrates spontaneously when it is disturbed. For example, when a guitar string is plucked, the sound is caused by the natural frequency at which the string vibrates. Mode shapes depict how an item moves or changes shape while vibrating at a natural frequency. For example, consider a drumhead. It swings up and down in a rhythmic way and vibrates when contacted. The drumhead’s mode shape at a specific natural frequency is represented by this motion.

2.2. Formulation

A vibrating system’s motion is governed by the following basic equation [11]:

$$M·\ddot{x}\left(t\right)+C·\dot{x}\left(t\right)+K·x\left(t\right)=F\left(t\right)$$

(1)

where M is the mass matrix, C is the damping matrix, K is the stiffness matrix, and x(t), $\dot{x}$, and $\ddot{x}$ are the displacement, velocity, and acceleration vectors, respectively. Finally F(t) is the external force.

In modal analysis, in which no external force is applied, Equation (1) is reduced to

$$M·\ddot{x}\left(t\right)+K·x\left(t\right)=0$$

(2)

To solve for the natural frequencies and mode shapes, a harmonic solution of the form below is considered:

$$x\left(t\right)=\varphi ·e^{i\omega t}$$

(3)

where $\omega$ describes the natural frequencies and $\varphi$ represents the mode shape. When this answer is entered into the simplified Equation (2) of motion, the following happens:

$$(M·{\omega }^2-K)·\varphi =0$$

(4)

Therefore, by solving Equation (4), natural frequencies and corresponding mode shapes are obtained, which serve as the foundation for evaluating the system’s vibrational characteristics and identifying potential resonance issues.

3. Random Vibration Analysis

Random vibrations simultaneously engage all frequencies within a structure, unlike sinusoidal vibrations that occur at specific frequencies [12]. They exhibit unpredictable fluctuations in both amplitude and phase over time. These vibrations are common in applications such as vehicle dynamics, aerospace turbulence, seismic activity, machinery operation and wind turbines [13]. Engineers typically analyze them using statistical measures like power spectral density (PSD) and root mean square (RMS) acceleration. Understanding random vibrations is essential for designing robust and reliable structures, predicting fatigue life, and ensuring safe operation in dynamic environments [14].

The PSD function is commonly used in engineering to describe vibration test loads by analyzing how power is distributed across different frequencies. When a product is tested against a specific PSD profile, acceleration time signals can be measured at various points on the structure. These signals are often random, but, for stationary processes, their statistical properties remain constant, allowing meaningful frequency-based analysis [15]. The PSD is typically derived using the fast Fourier transform (FFT), which converts time-domain signals into frequency components. By squaring these frequency amplitudes, the PSD function is obtained, providing valuable information for evaluating how structures respond to dynamic loads. This approach is essential for applications such as vibration testing, structural health monitoring, and optimizing system designs to ensure resilience against vibration-induced failures [16].

As mentioned earlier, vibrations in real-world environments are seldom purely sinusoidal. In random vibration fatigue analysis, the Steinberg method is widely applied to estimate component lifespan by integrating S–N curves and stress levels [17]. Steinberg’s three-band method evaluates the Von Mises stress output from random vibration simulations. Assuming that the stress follows a Gaussian distribution, the method categorizes stresses into three distinct bands based on the standard deviation ($\sigma$) values, as depicted in Figure 1.

• $1\sigma$ Band: Covers approximately 68.27% of the vibration cycles (red region);
• $2\sigma$ Band: Encompasses around 27.18% of the cycles (orange region);
• $3\sigma$ Band: Represents about 4.28% of the cycles (pink region).

Each band corresponds to a range of stress levels, enabling engineers to track completed cycles statistically and determine their contribution to fatigue damage. This approach offers a statistical framework to analyze fatigue life by accounting for the varying stress amplitudes experienced during vibration cycles. By integrating the number of completed cycles within each band, engineers can better predict potential failure points and optimize structural designs.

4. Load Frequencies of a Wind Turbine

Wind turbines are subject to various load frequencies during operation. These frequencies arise from different mechanical and aerodynamic processes within the turbine system. Some of the key frequencies include the following:

• Rotational frequency: This is one of the most significant load frequencies and is directly related to the rotational speed of the turbine blades. These cyclic loads can cause fatigue in the turbine components over time. It occurs when each blade passes a fixed point, generating a load corresponding to the number of blades and the rotor speed. Rotational frequency is calculated based on $f_{rot}={\displaystyle \frac{RPM}{60}}$, where RPM is the revolutions per minute of the rotor. For a turbine with three blades, the passing frequency is three times the rotor speed. For example, if a turbine operates at a rotor speed of 15 RPM with 3 blades, the frequency can be calculated using $f_{rot}={\displaystyle \frac{15\times 3}{60}}=0.75$ Hz. This indicates that the frequency at which each blade passes a fixed point is 0.75 Hz [18];
• Gear frequency: The gear frequencies in a wind turbine are related to the rotational speeds of the gear system, which are influenced by the rotation speed of the turbine’s components. In a wind turbine, the gear system transfers power from the low-speed shaft, connected to the rotor blades, to the high-speed shaft that drives the generator, typically through a gearbox. The key gearbox frequencies in a wind turbine include the low-speed shaft (rotor frequency) at 0.25 Hz, the high-speed shaft frequency at 25 Hz, the meshing frequency of the input gear at 7.5 Hz, and the meshing frequency of the output gear at 1000 Hz [19]. Notice that these numbers are approximate and not exact, as they depend on specific design parameters such as rotor speed, gear ratio, and the number of teeth on the gears, which can vary across different wind turbine models;
• Yawing frequency: The yawing frequency of a wind turbine refers to the rate at which the nacelle rotates to keep the rotor aligned with the wind direction. This frequency depends on several factors, including the turbine’s design, the control system, and the wind conditions. Typically, the yawing frequency for wind turbines is low, generally in the range of 0.05 to 0.1 Hz [20]. However, the exact yaw frequency can vary based on the wind turbine’s specifications, the wind conditions, and the operational strategy of the turbine;
• Generator frequency: The generator in a wind turbine operates at a frequency that matches the electrical grid, either 50 Hz or 60 Hz. When the turbine operates at low speeds or under varying load conditions, the mechanical loads generated by the generator can cause vibrations. This can put stress on parts like the generator, bearings, and shafts, potentially leading to damage or failure. Designers account for these risks by optimizing the turbine’s mechanical system and using vibration-damping techniques to ensure stable operation [21];
• Wind turbine blade natural frequency: The natural frequencies of wind turbine blades typically range between 1 to 3 Hz, depending on factors such as the blade’s design, material properties, and length. The blades are subject to aerodynamic forces, including wind gusts and changes in wind speed, which can cause vibrations at certain frequencies. A typical 1–3 MW wind turbine might experience blade frequencies around 1.5 to 2.5 Hz, but this can vary based on blade material, geometry, and overall design. Larger or offshore turbines, which often use longer blades, may have lower natural frequencies [22].

The key load frequencies of wind turbine components during operation are listed in

Table 1. Key load frequencies of wind turbine components during operation.

Frequency Type	Frequency Value
Rotational Frequency	0.75 Hz (Example: Rotor speed of 15 RPM with 3 blades)
Gear Frequency	Low-speed shaft: 0.25 Hz High-speed shaft: 25 Hz Input gear: 7.5 Hz Output gear: 1000 Hz
Yawing Frequency	0.05 to 0.1 Hz
Generator Frequency	50 Hz or 60 Hz
Blade Natural Frequency	1.5 to 2.5 Hz

.

5. Modeling and Analysis in Ansys

To perform modal analysis and obtain the natural frequencies, finite element analysis (FEA) is required. FEA is a computational technique used to find approximate solutions to a wide range of engineering problems [23]. A finite element model provides a piecewise approximation to the governing equations. The fundamental idea behind FEA is to replace a solution region with a collection of discrete elements (discretization), which can be combined in various configurations. This approach allows FEA to represent highly intricate shapes.

ANSYS is a comprehensive engineering simulation software used for FEA, computational fluid dynamics (CFD), and other simulation-driven design tasks. It helps engineers and designers to model, analyze, and optimize products and systems in various industries such as aerospace, automotive, and electronics. ANSYS offers advanced tools for structural, thermal, electromagnetic, and fluid simulations, providing insights into a product’s performance under real-world conditions. It aids in reducing physical testing, improving product efficiency, and accelerating the design process [24].

To perform modal analysis in ANSYS, the first step is to create the geometry of the structure in ANSYS or import an existing CAD model. Once the geometry is ready, the next step is to define the material properties, including density, Young’s modulus, and Poisson’s ratio, which are essential for accurate simulation. After assigning the material properties, the structure needs to be meshed, dividing it into smaller elements to accurately model the physical system. Next, boundary conditions such as fixed supports or applied loads are defined to simulate real-world constraints. Once the model setup is complete, the modal analysis can be performed by selecting the “Modal” analysis type. ANSYS will solve for the natural frequencies and mode shapes of the structure. After the modal analysis, a random vibration analysis was also conducted in ANSYS by defining PSD input and computing the structural response. Finally, the results can be visualized and interpreted to assess the system’s vibrational characteristics and identify potential resonance issues.

A detailed explanation of these steps is provided below.

5.1. Case Study

In this research, the FP50R12KT4 IGBT module was selected to investigate how vibration affects its lifespan. The module was chosen due to its widespread use in power electronic systems, where its reliability under various operational conditions is critical. This is a 1200 V, 50 A power integrated module (PIM) by Infineon Technologies. As illustrated in Figure 2, the system comprises a three-phase inverter highlighted in a blue box, a bridge rectifier in a red box, and a brake chopper in a green box. These integrated components contribute to reducing system costs.

5.2. Creating Geometry

The IGBT structure, illustrated in Figure 3, begins at the bottom with a base plate that provides both mechanical support and thermal conductivity. Above this, a baseplate solder alloy (solder 1) is used to securely attach the layers above. Next is the lower copper layer (copper 1), which serves as a conductor and distributes heat evenly, followed by a ceramic layer that offers electrical insulation while maintaining thermal conductivity. Above this lies the upper copper layer (copper 2), another conductive layer that helps in electrical and thermal management. The die-attach solder alloy (solder 2) then connects the upper copper layer to the IGBT chip, the core active element of the device. Finally, aluminum bond wires are used to establish electrical connections between the chip and external circuitry. All these elements are located within a silicon gel, which helps in providing additional thermal conductivity and protecting the components. This multilayer design ensures efficient electrical performance, thermal management, and durability.

It is important to note that there are two types of bond wires in the module. The first type, referred to as chip-level bond wires, connects the chips to the copper plates. The second type, known as terminal bond wires, links the chips or copper plates to the external connections. While both types have the same diameter of 400 $\mathsf{\mu }\mathrm{m}$, the primary difference between them lies in their shape, with terminal bond wires being longer [25].

The dimensions of the various components of the IGBT, including width, length, and thickness, are detailed in

Table 2. Physical specifications of FP50R12KT4 IGBT module.

Component	Material	l (mm)	w (mm)	t ($\mathsf{\mu }\mathbf{m}$)
Baseplate	Cu	107.5	38	3000
Solder 1	SAC305	23	27.8	250
Copper 1	Cu	23	27.8	300
Ceramic	Al2O3	24	29	380
Copper 2	Cu	23	27.8	300
Rectifier diodes	Si	4.8	4.8	302
	SAC305	4.8	4.8	85
Brake chopper diode	Si	3.3	2.98	106.8
	SAC305	3.3	2.98	85
Brake chopper IGBT	Si	5.45	4.99	111.8
	SAC305	5.45	4.99	85
Inverter IGBTs	Si	7.25	6.84	111.8
	SAC305	7.25	6.84	85
Inverter diodes	Si	6.3	4.5	106.8
	SAC305	6.3	4.5	85

. These measurements are essential for accurate 3D modeling, ensuring the precise replication of the physical structure during the design and simulation processes. Noticed that solder 1, copper 1, and copper 2 are based on the nomenclature provided in Figure 3. Additionally, in Table 2, the symbols are defined as follows: l (in mm) represents length, w (in mm) represents width, and t (in $\mathsf{\mu }\mathrm{m}$) represents thickness.

Using these dimensions, a 3D model of the IGBT was created in ANSYS SpaceClaim, as shown in Figure 4. The model is constructed with a layered configuration to represent the entire structure. Notice that silicone gel was excluded from the 3D model, as its damping ratio remains constant for frequencies above 100 Hz. Since the failure model focuses on identifying failure locations and causes at frequencies above 100 Hz, this constant damping has no impact on the results. While the gel may extend the module’s lifespan, it does not influence failure locations or causes [26].

5.3. Material Assignment

After specifying the dimensions of the IGBT components, it is important to consider the material characteristics. The materials used in the IGBT include aluminum (Al), ceramic (Al₂O₃), silicon (Si), copper (Cu), and solder (SAC305). The key material properties that are considered are density ($\rho$), Young’s modulus (elastic modulus), and Poisson’s ratio ($\nu$).

Young’s modulus measures the stiffness of a material and represents the relationship between stress and strain in the linear elastic region of a material’s deformation. It is crucial for determining how much a material will deform under a given load. Poisson’s ratio, on the other hand, describes the ratio of lateral strain to axial strain when a material is stretched. It provides insights into the material’s behavior when subjected to stress in different directions [27]. These properties are essential for ensuring the mechanical integrity and performance of IGBT components. These material properties are presented in

Table 3. Material properties of FP50R12KT4 IGBT module.

	$\mathit{\rho }$ (kg·${\mathbf{m}}^{-3}$)	E (GPa)	$\mathit{\nu }$
Cu [28]	8960	120	0.33
SAC305 [29]	7380	26.2	0.42
Al2O3 [30]	4000	400	0.23
Si [31]	2330	130	0.28
Al [32]	2710	70	0.33

.

Another important property to consider in the context of vibration analysis is the S–N curve. The S–N curve or Wohler curve illustrates the relationship between the stress amplitude (S) and the number of cycles to failure (N) for a material subjected to cyclic loading. It helps predict the fatigue life of materials by showing how much stress a material can withstand before failure under repeated loading. The curve typically has a downward slope, with high stress leading to failure in fewer cycles, and low stress allowing for more cycles. Data for S–N curves for various materials used in IGBT modules can be found in references [33,34,35,36,37].

5.4. Meshing Strategies

Meshing methods are crucial for generating a discretized representation of the geometry used for FEA. The choice of meshing method can significantly impact the accuracy and efficiency of simulations. The three most famous meshing methods in ANSYS are tetrahedral meshing, hexahedral meshing, and sweep meshing.

Tetrahedral meshing is widely used due to its ability to handle complex and irregular geometries, making it a go-to option for unstructured domains [38]. Hexahedral meshing, known for its high accuracy and better convergence, is preferred for structured geometries and simulations requiring precise results, such as CFD or stress analysis [39]. Sweep meshing is ideal for prismatic or axisymmetric geometries, creating structured, high-quality meshes by sweeping a 2D mesh along a path [40]. These methods are versatile and widely adopted across various engineering applications.

Automatic meshing in ANSYS simplifies the process by automatically selecting the best meshing method based on the geometry and analysis type. It is ideal for quick setups, offering efficient and reliable results without manual intervention, making it popular for general-purpose simulations. This method has been used in the simulation part. The meshing of the different parts was performed in ANSYS to ensure accurate division of the geometry for the simulation, as shown in Figure 5.

A finer mesh with a body sizing of 0.25 mm was applied to improve the accuracy of the analysis in ANSYS. This finer discretization ensures a more precise representation of the geometry, allowing for a better resolution of the solution gradients and capturing subtle variations in the simulation, which leads to more reliable results.

5.5. Boundary Conditions

A boundary condition is a set of constraints or conditions applied to a model or system that defines how it interacts with its environment during a simulation or analysis. In the context of structural analysis, boundary conditions include supports that restrict movement or rotation, such as fixed supports or displacement constraints, and loads like forces, pressures, or moments that are applied to the system. These conditions ensure that the model behaves realistically by mimicking real-world physical limitations and external influences, and their proper definition is critical for obtaining accurate and reliable results [41].

In a modal analysis, as mentioned earlier, the objective is to determine the natural frequencies and mode shapes of a structure, which are critical for understanding its vibrational behavior. To set up a modal analysis in ANSYS, the key boundary conditions typically include the following:

• Standard Earth gravity: This is used to account for the gravitational forces acting on the model. While gravity doesn’t directly affect the natural frequencies in a typical modal analysis, it is important for some structures, particularly large or complex ones, where gravity might influence the stiffness or mass distribution, potentially affecting the modal characteristics.
  In this research, gravity is applied in the negative z-direction to simulate the effect of Earth’s gravitational force. The value of gravitational acceleration is set to 9.8 m/s², which is the standard value used to represent gravity at the Earth’s surface.
• Fixed support: A fixed support is crucial in modal analysis as it restricts all translations and rotations at specific points or surfaces of the structure. It serves as the foundation or anchor for the model, preventing rigid body motion and ensuring that the structure is held in place during the analysis.

Both these boundary conditions help in defining a realistic scenario for the modal analysis, ensuring that the vibrational behavior of the structure is accurately captured and that the model is appropriately constrained for analysis.

Figure 6 illustrates the mounting platform where the IGBT is positioned on the fixed support section, represented in dark blue. The 3D axis in the figure indicates that gravity acts in the negative z-direction, aligning with the simulation setup.

6. Simulation

Simulations were conducted on the 3D model described earlier using ANSYS 2023 R1 within its mechanical environment. The aims of these simulations were to determine the natural frequencies of the IGBT module through a modal analysis and a random vibration analysis, as follows:

• Natural Frequency Analysis and Resonance Risk Assessment: The natural frequencies are critical in determining whether the module may be subjected to resonant vibrations that could lead to excessive stresses and potential failure. To minimize the risk of resonance, it is essential that the natural frequencies are sufficiently separated from the load frequencies. In this part, the natural frequencies of the IGBT module are calculated to assess the potential for resonance under operational loading conditions. The first 15 natural frequencies of the IGBT module are listed in

  Table 4. First 15 natural frequencies of the IGBT module (in Hz).

  Mode	Frequency (Hz)
  1	18,972
  2	19,053
  3	19,398
  4	19,424
  5	19,496
  6	19,523
  7	19,702
  8	19,713
  9	19,769
  10	20,814
  11	20,845
  12	20,853
  13	20,856
  14	20,881
  15	21,826

  , with the lowest frequency being 18,972 Hz.

After comparing the natural frequencies obtained from the ANSYS simulations with the expected load frequencies mentioned in Section 4 during the operation of the IGBT module, it was found that the load frequencies are significantly different from the module’s natural frequencies, which are around 19 kHz. The operating load frequencies, typically caused by mechanical vibrations, fall far outside the range of the natural frequencies. As a result, there is no risk of resonance, which is a condition that can amplify vibrations and lead to potential performance issues or damage. Since the load frequencies do not overlap with the natural frequencies, the IGBT module is unlikely to experience resonance effects, ensuring stable operation without concerns related to vibrational amplification.

• Random Vibration Analysis and Fatigue Evaluation: In this part, random vibration loading is applied to the IGBT module to simulate the operational vibrational environment experienced within the wind turbine nacelle. The primary objective of this analysis is to assess how these vibrations affect the fatigue life of the IGBT module. This approach is crucial for understanding the long-term reliability of the module under dynamic loading conditions.

In this way, PSD data from [8] have been employed and implemented in ANSYS to study the effects of random vibration on the IGBT module’s lifetime. The goal was to understand which parts of the module are most affected by deformation under different vibration conditions. Both $1\sigma$ and $3\sigma$ analyses were performed to assess how deformation varied across the module.

In this study, the IGBT module was analyzed as a whole, assuming that the spatial placement of individual IGBTs within the module (including the six inverter IGBTs and the brake chopper IGBT) does not significantly influence the overall results. This assumption is based on the structural uniformity of the module, which ensures that all IGBTs experience similar vibrational characteristics. Since the primary focus of this research is on the vibration effects on IGBT lifetime, minor variations in placement are considered negligible in comparison to the overall vibrational response of the module.

The results highlighted that the bond wires are particularly sensitive to the effects of random vibration, as seen in Figure 7.

Table 5. Minimum, maximum, and average deformation values for $1\sigma$ and $3\sigma$ studies.

Deformation	$1\mathit{\sigma }$ (68.27%)	$3\mathit{\sigma }$ (99.73%)
Minimum (mm)	0	0
Maximum (mm)	9.74 $\times {10}^{-7}$	2.92 $\times {10}^{-6}$
Average (mm)	3.02 $\times {10}^{-7}$	9.07 $\times {10}^{-8}$

provides the minimum, maximum, and average deformation values for both the $1\sigma$ and $3\sigma$ studies.

To further assess the potential impact, ANSYS’s fatigue analysis tool has been used to estimate the expected lifetime and damage factor of the module components. The fatigue tool uses Miner’s rule to calculate the cumulative damage from vibration-induced stresses, factoring in both the amplitude of the stresses and the number of cycles that the component undergoes.

The following are what these values represent:

–

Expected life indicates how many cycles the component is expected to endure before failure, given the applied vibration conditions;

–

Damage factor shows how much cumulative damage has occurred on the component. A value of 1 means that the component is expected to fail, while values below 1 suggest that it is still within safe operating limits.

Figure 8 illustrates that bond wires experience higher stress levels than other parts of the module, particularly at the knee points of the bond wires. A closer view in Figure 9 highlights that the minimum lifetime under these conditions is around $2.14\times {10}^{12}$ cycles. To convert the number of cycles to failure into real lifetime, the frequency of vibrations to which the IGBT module is subjected needs to be specified. The operational lifetime in seconds is then calculated using the following equation:

$$TimetoFailure={\displaystyle \frac{Cyclestofailure}{Vibrationfrequency\left(\mathrm{H}\mathrm{z}\right)}}$$

(5)

As outlined in Section 4, the maximum vibration frequency is due to the gearbox mesh at 1000 Hz. As a result, the calculated time to failure based on Equation (5) is $2.14\times {10}^9$ s, which is equivalent to 67.4 years. This suggests that the effect of vibration on the IGBT module lifetime is relatively minimal. However, it is important to note that, in real-world conditions, vibration is not the only stressor affecting the IGBT module lifetime. Factors such as thermal stress, electrical load cycling, and the 3aging of the IGBT’s internal components—like the semiconductor material and bonding—are likely to contribute much more significantly to its failure than vibration alone. In addition, environmental influences, including temperature fluctuations, humidity, and electrical current spikes, often play a more substantial role in the degradation of the IGBT module.

Figure 10 and Figure 11 present the damage distribution. These outputs show how the damage varies spatially within the IGBT module. This helps to identify which areas of the module are more prone to failure based on the applied cyclic loads. These figures indicate that the highest concentrations are observed at the knee points of the bond wires. The maximum damage factor is $4.67\times {10}^{-13}$ ≃ 0, much lower than 1, indicating that vibration has an almost negligible effect on the IGBT module’s overall lifetime. This suggests that the module is highly reliable under the simulated vibration conditions.

7. Conclusions

To sum up, this study assessed the effect of vibrations from wind turbines on the lifespan of the FP50R12KT4 IGBT module. Modal analysis showed that the minimum natural frequency of the module is around 19 kHz, which is much higher than the maximum load frequency typically encountered in wind turbine operations. This large difference suggests that resonance is unlikely. Furthermore, the random vibration analysis revealed that the maximum deformation at the knee points of the bond wires was only 2.92 $\times {10}^{-6}$ mm, a very small value that has little to no effect on the module’s performance. With a minimum calculated lifetime of 2.14 $\times {10}^{12}$ cycles (67.4 years) and a maximum damage rate of just 4.67 $\times {10}^{-13}$, the impact of vibration on the IGBT’s lifespan is negligible. Overall, the findings confirm that vibrations in wind turbine nacelles do not pose a significant risk to the IGBT module’s longevity, supporting the continued reliability of IGBT-based power electronics in these environments. While this study is focused on the impact of vibration on IGBT lifetime, it is acknowledged that other environmental stressors, such as thermal cycling and humidity, also play a crucial role in IGBT reliability. Solder fatigue and bond wire degradation can be caused by thermal cycling, whereas insulation breakdown and corrosion may be induced by humidity exposure. In future work, the effects of all these stressors will be considered to provide a more comprehensive understanding of their combined impact on IGBT lifetime in wind turbine applications.