Research on assembly stress and deformation of thin-walled composite material power cabin fairings

Yushuang Dong; Bianhong Li; Houjiang Zhang; Hanjun Gao

doi:10.1515/rams-2025-0117

Article Open Access

Research on assembly stress and deformation of thin-walled composite material power cabin fairings

Yushuang Dong , Bianhong Li , Houjiang Zhang and Hanjun Gao

Published/Copyright: July 8, 2025

Published by

Become an author with De Gruyter Brill

Submit Manuscript Author Information

From the journal REVIEWS ON ADVANCED MATERIALS SCIENCE Volume 64 Issue 1

Abstract

As a critical component of a helicopter, the issue of assembly continuity deviation between the fairing and adjacent components during the assembly process can significantly impact flight stability and safety. The traditional fairing assembly process typically emphasizes basic alignment and fixation, often neglecting an analysis of the factors that influence its shape and performance characteristics. This study simulates the fairing assembly model under various working conditions to investigate stress distribution and deformation characteristics. The goal is to identify the primary factors that lead to changes in the shape and performance of the fairing and to summarize the overall stiffness distribution of the fairing. To ensure the accuracy of the constructed finite-element model of the fairing, experiments were initially designed to determine the intrinsic parameters of the fairing composites. This process aimed to obtain key data, such as the elastic modulus and Poisson’s ratio. Following this, a mechanical plate loading test simulating equivalent cutting of the fairing was conducted, and a corresponding simulation model was developed using ABAQUS software. By comparing the results from the tests and simulations of the mechanical plate, the feasibility of applying the determined intrinsic parameters to the fairing finite-element model was effectively validated. Subsequently, a three-dimensional model of the fairing was created in CATIA software and imported into ABAQUS for analytical modeling, allowing for the simulation and analysis of the fairing’s force conditions under various constraints. The results indicate that the overall stiffness of the fairing is influenced by fixed-boundary constraints and external forces. Additionally, the stress experienced by the fairing is negatively correlated with the width of the fixed-boundary constraints; as the width increases, the stress decreases continuously. This decrease is more pronounced in the initial stages and gradually slows down in later stages. Specifically, the stress decreases by as much as 79.25% within the constraint width range of 10–20 mm, while the reduction slows to 46.2% in the 60–80 mm range. The shape and performance of the fairing are influenced by various factors, with displacement load and clamping distance being the primary determinants. The effects of these two factors on fairing stress vary dynamically with changing working conditions. Notably, under different clamping distances, a significant linear relationship exists between displacement load and deformation. For instance, at a clamping distance of 200 mm, the difference between adjacent deformations stabilizes at 0.516 mm, with a relative deviation strictly controlled within ±3%. When the clamping distances are increased to 600 and 1,000 mm, the dispersion of the deformation increments relative to their mean values remains low, with the ratio of the standard deviation to the mean value being 2.5 and 2%, respectively.

Keywords: composite material; helicopter fairing; thin-walled structure; finite-element simulation

1 Introduction

In aerospace engineering, the fairing is a critical external component of a helicopter, serving essential functions in drag reduction, optimization of aerodynamic performance, and protection of payloads. As aerospace technology continues to evolve, lightweight and high-strength composite materials have increasingly emerged as the preferred choice for fairing manufacturing [1,2,3].

In recent decades, the technology for controlling deformation in thin-walled components, such as fairings, has garnered significant attention both domestically and internationally. This technology is recognized as a crucial aspect of the national defense industry and remains a focal point in research endeavors [4,5,6]. Liu et al. [7] proposed the virtual functional element method to simplify parallel dimensional chains, addressing the challenging issues of assembly accuracy and deformation prediction in industrial product components. The Jacobi–Toso model was developed to resolve integrated deviations, while the locking effect and lever activation effect were introduced to characterize the influence of invariance. Ding et al. [8] addressed the problem of intense vibration deformation during milling by proposing a first resonance approach to achieve local stiffness supplementation and a targeted vibration-damping mechanism. This semi-active electromagnetic vibration damping device was designed for non-magnetic thin-walled workpieces, effectively controlling the vibration deformation during the milling of thin-walled parts. Li et al. [9] explored the effect of equivalent bending stiffness using a semi-analytical model of bi-directional blank residual stresses, enabling the prediction of machining deformation in thin-walled parts with various reinforcement arrangements. Ge et al. [10] investigated the impact mechanism of coupling effects in iterative compensation, specifically focusing on thin-walled components used in aerospace applications and the associated challenges in machining accuracy, proposing a non-iterative compensation method to address the limitations of existing techniques, milling experiments demonstrated the potential for real-time deformation compensation in thin-walled parts. Yue et al. [11] introduced a digital double-drive deformation monitoring method utilizing digital twin technology, addressing the challenges associated with processing thin-walled parts that are prone to deformation and difficult to monitor. Gao et al. [12] developed a semi-analytical prediction model for machining deformation of thin-walled parts, employing the equivalent bending stiffness derived from finite-element simulation and plate-shell theory. This model successfully predicts deformation in seven typical cases and investigates the effects of initial residual stress and other factors to validate its accuracy. Xue et al. [13] introduced a robust optimization design method that incorporates an agent model to address the challenges of tolerance optimization in aerospace thin-walled components and successfully achieves tolerance control optimization for these components through a series of model constructions and algorithm enhancements. Saadat et al. [14,15] and Saadat and Cretin [16] further investigated the deformation mechanisms occurring during the assembly of parts by employing various methods, including finite-element analysis, to facilitate advanced predictions of thin-walled components. Li et al. [17] proposed a machining deformation prediction model based on residual stress, which utilizes equivalent stiffness numerical calculations and elastic mechanics theory and effectively predicts the deflection of six thin-walled components, significantly enhancing the accuracy of part predictions. Ge et al. [18] reduced the solution time by dynamically modifying the stiffness matrix of thin-walled components. Building on this approach, a compensation strategy that does not require iteration is proposed and validated through an example involving thin-walled components made of aluminum alloys. Gao et al. [19] employed a biaxial residual stress analysis model to establish a quantitative relationship between deformation and stress across three machining strategies and further summarized the impact of workpiece positioning on machining deformation. Zhou et al. [20] developed a distortion analysis method for thin-walled box girders considering the effects of inhomogeneous shear deformation in each wall plate based on the principles of micro-elementary stress equilibrium and the torsional self-equilibrium condition of the box girder cross-section. Deepak Kumar and Panigrahi [21] conducted a nonlinear vibration characterization of pre-twisted thin-walled anisotropic box girders by developing a mathematical model that accounts for shear deformation and the coupling of the Green’s strain tensor with large displacements.

According to the findings, research on the deformation control of thin-walled components has produced significant results. The study comprehensively examines various influencing factors and proposes effective strategies, such as high-speed machining, to minimize deformation and enhance process optimization. Innovative approaches, including gap reduction techniques, component optimization, and flexible positioning systems, are introduced to tackle assembly deformation issues and improve the quality of parts assembly. A variety of models have been developed for error analysis and prediction, integrated with advanced technologies, to achieve precise control over deformation errors in both machining and assembly processes. Anticipating the direction of deformation in advance provides essential data for formulating control strategies, thereby contributing to enhanced machining accuracy and stability in quality. Furthermore, the application of low-temperature tests to evaluate the molding quality of components, along with the dynamic adjustment of the stiffness matrix for an iterative compensation strategy, has significantly advanced the technology for controlling part deformation.

In terms of fixtures and clamping force, the deformation of thin-walled components can be controlled by employing various positioning and clamping methods, including clamping positions, clamping sequences, and loading forms. Li et al. [22] analyzed the critical impact of aerospace thin-walled components on aircraft performance and systematically described several techniques, including advanced fixtures, while targeting corresponding prediction and control methods. Ju et al. [23] achieved rapid control of clamping deformation based on the accuracy requirements of vacuum fixtures for thin-walled flat plate components by integrating an improved algorithm with a correlation function to address specific conditions. Wang et al. [24] proposed an optimized layout method based on the clamping position of the fixture to reduce stress concentration in the contact area, thereby mitigating the effects of fixture distribution on part machining deformation. Kaya [25] enhanced the distribution of fixtures by integrating finite-element analysis with genetic algorithms to minimize errors caused by part deformation. Li et al. [26] introduced a deep spatio-temporal learning network to simulate the complex geometric load–deformation relationship, addressing challenges such as the unpredictability of machining deformation and low accuracy by leveraging the spatio-temporal correlation characteristics of geometry and cutting load, thereby enabling accurate predictions of machining deformation in components. Wang et al. [27] developed a control method for digital dual-drive clamping force by combining finite-element simulation with a deep neural network algorithm, resulting in improved machining accuracy for thin-walled components. Tian et al. [28], addressing the challenges of end milling deformation and vibration in large thin-walled workpieces, proposed a novel method to mitigate vibration and deformation during mirror milling by employing a magnetic follower support fixture, which effectively reduces both vibration and deformation in thin-walled parts. Raghu and Melkote [29] examined the impact of fixture assembly sequences on part positioning errors through model simulations and experiments, and the results indicated that the clamping sequence of the part significantly influences the workpiece error. Deng and Melkote [30] addressed the clamping force optimization problem using a particle swarm optimization technique to minimize the deformation of parts caused by clamping. Bhatnagar et al. [31] developed a biaxial tensile testing mechanism and designed a new fixture that is highly adaptable to any orthotropic or fiber-reinforced material system. Ratchev et al. [32] proposed a machining error compensation method for low-stiffness thin-walled parts, utilizing finite-element simulation software to design the error compensation and presenting a relevant program to ensure the precise planning of tool trajectories for thin-walled components. Varadarajan and Culpepper [33] introduced a fixture-based statistical analysis method for errors in the assembly process of flexible parts, where the assembly process of thin-walled components was staged with reasonable linear assumptions to achieve effective deformation control.

Significant advances and results have been achieved in the field of deformation control and clamping force management for fixtures used with thin-walled components. Some researchers have proposed variable clamping force fixtures to optimize both the positioning of the clamping points and the clamping force itself, successfully reducing cutting deformation. The integration of fixture design with finite-element analysis (FEA) software allows for accurate predictions of the clamping state and dynamic behavior. By conducting finite-element analyses of various influencing factors and validating the results through testing, a robust foundation for related research has been established. Additionally, optimizing the layout of fixture distribution effectively reduces stress concentration in the contact zone. The study delves deeply into the impact of fixture assembly sequences on positioning errors, clearly elucidating their internal correlations. These research findings provide a solid theoretical and practical support system for controlling deformation in thin-walled parts, significantly advancing the ongoing development of this technology.

Although significant research efforts have been dedicated to the deformation machining of thin-walled parts both domestically and internationally, encompassing a range of topics from the proposal of variable clamping force fixture schemes to the integration and application of various advanced technologies and fixture designs, there remains a notable deficiency in fundamental formability research specifically related to fairings, which are a type of thin-walled component. In the aircraft assembly process, the geometric characteristics of the fairing are crucial for ensuring assembly accuracy. However, the lack of research in this area severely limits the enhancement of calculation accuracy in the aircraft assembly prediction deviation model, which subsequently impacts the optimization of the overall quality and performance of the aircraft assembly.

In light of this, this article uses the helicopter fairing model as a foundation and employs the finite-element method to conduct a comprehensive investigation. By simulating various working conditions, the deformation data of the fairing under different scenarios are accurately obtained. Additionally, the key factors influencing shape changes – such as clamping distance, force distribution, structural design, and other mechanisms – are analyzed in detail. Building on this analysis, the deformation behavior of the overall stiffness distribution of the composite fairing is further summarized. This research aims to provide more precise parameter support for the aircraft assembly prediction model, thereby advancing the aircraft assembly process toward greater precision and enhanced performance and contributing to technological progress in the aerospace sector.

2 Materials and methods

2.1 Objects of the study

The fuselage shell fairings of modern helicopters are primarily constructed from large, rigid carbon composite sandwich panels. The outer skin is relatively thick, while the inner stabilizing skin is thinner, featuring a honeycomb core layer that extends throughout the nacelle’s interior and is situated between the major internal frame members [34,35,36]. The fairing examined in this article is the side opening and closing fairing of the helicopter. In terms of spatial distribution, the helicopter’s side opening fairing is typically positioned in a specific area on both sides of the fuselage, conforming to the overall aerodynamic shape of the helicopter and closely integrated with the key systems housed within the fuselage, as illustrated in Figure 1.

Figure 1

Position of the side-opening and closing fairing of the helicopter.

The location of the side-opening fairing varies among different helicopter models and is often situated near the power, fuel, or electronic equipment compartments. This design facilitates quick access to critical areas during maintenance and overhaul while also protecting these areas during flight to ensure safety. When selecting materials for helicopter side-opening and closing fairings, it is essential to consider a variety of performance requirements. Composite materials, such as carbon-fiber-reinforced composites, are increasingly being utilized in the aerospace sector. These materials possess a very high strength-to-weight ratio, which can significantly reduce the weight of the fairing itself, thereby decreasing the overall fuel consumption of the helicopter and enhancing flight performance [37,38,39]. Their excellent corrosion and fatigue resistance allows them to maintain stable long-term performance in complex and variable flight environments, effectively resisting erosion from rain, sand, dust, ultraviolet rays, and other external factors. This ensures the structural integrity and longevity of the fairing [40,41,42].

The helicopter fairing examined in this article (Figure 2) measures 1,200 mm in length, 1,200 mm in width, and 2.3 mm in thickness. It comprises three main components: a skin and two reinforcing structures constructed from four materials: carbon fiber, high-temperature fire-resistant cloth, glass fiber, and interlayer aramid paper, in that order. The properties of the glass fiber and interstitial aramid paper honeycomb materials are presented in Table 1. The carbon fiber and high-temperature fireproof cloth materials will be characterized through intrinsic parameter determination experiments involving composite materials.

Figure 2

The helicopter fairing structure.

Table 1

Basic material parameters

Material	Glass fiber	Aramid paper honeycomb
Density (kg·m⁻³)	1.952 × 10²	6.05 × 10²
E1 (MPa)	17,000	2,780
E2 (MPa)	17,000	1,600
Nu12	0.34	0.34
G12 (MPa)	23,000	43,400
G13 (MPa)	23,000	23,200
G23 (MPa)	23,000	5,540

2.2 Experimental determination of intrinsic parameters of composite materials

Based on GB/T 1447-2005, Methods for Tensile Properties of Fiber Reinforced Plastics, the tensile modulus of elasticity and Poisson’s ratio of the processed standard specimens are determined. The tensile modulus of elasticity ( E ) , also known as Young’s modulus, can be calculated from the stress-strain curves obtained from the specimens after they have been uniformly loaded until failure. Additionally, Poisson’s ratio ( ν ) can be calculated using the axial and transverse strains measured by the strain measuring equipment. The specific shape of the specimen is illustrated in Figure 3.

Figure 3

Basic mechanical specimen model: (a) specimen size parameters, (b) carbon fiber specimen, and (c) high-temperature fireproof cloth specimen.

The tensile modulus of elasticity and Poisson’s ratio of the specimen were determined using a universal mechanical testing machine (LE3504 50 kN, Force Test [Shanghai] Scientific Instruments Co., Ltd.). The mechanical tensile test process is illustrated in Figure 4, and the test steps are as follows:

Apply axial loading by positioning the specimen centrally between the two supports. Measure the specific dimensions of the specimen with an accuracy of 0.2 mm, as illustrated in Table 2.
The specimen was loaded at a rate of 5 mm·min⁻¹ and was stretched until it sustained damage.
The data obtained from the testing machine software are utilized to construct the load–deformation diagram and the stress–strain curve of the specimen during the destructive testing process. The engineering stress–strain is directly calculated from the test data, as shown in Eqs. (1) and (2). Based on the engineering stress–strain, the true stress–strain can be calculated using Eq. (3). In the formulas, the subscript t is true stress and strain, while the subscript e is engineering stress and strain

(1) σ e = F i A i ,

(2) ε e = Δ l i L i ,

(3) σ t = ( 1 + ε e ) σ e ε t = ln ( 1 + ε e ) ,

where σ denotes the stress, ε denotes the strain, F represents the tensile force, A is the cross-sectional area of the specimen, L indicates the original length of the specimen, Δl signifies the change in length of the specimen after being subjected to the force F, and i refers to the ith specimen.

Figure 4

Mechanical tensile test process.

Table 2

Carbon fiber specimen tensile and high-temperature fireproof cloth experimental specimen size

Material	Specimen number	Marker size (L × W × H, mm)
Carbon fiber	①	180 × 20.1 × 5
Carbon fiber	②	180 × 19.8 × 5
High-temperature fireproof cloth	③	180 × 20.2 × 5
High-temperature fireproof cloth	④	180 × 19.8 × 5

Determine the stress σ and the corresponding strain values ε of the specimen within the linear range. Calculate the tensile modulus of elasticity (E) of the specimen. Additionally, determine the axial strain ε x and the transverse strain ε y values recorded by the strain measuring equipment at the time of the specimen’s failure. Finally, calculate Poisson’s ratio ν of the specimen using the following formula:

(4) σ = E ε ,

(5) ν = − ε y ε x .

The stress–strain curve (Figure 5(a)) and the tension–displacement curve (Figure 5(c)) for carbon fiber specimens ① and ② are presented. The entire tensile process can be categorized into three stages: the nonlinear onset stage, the linear elasticity stage, and the failure stage. As illustrated in Figure 5(c), the tensile force–displacement curves for both experiments exhibit a similar trend; however, the tensile stiffness of the specimens differs. The tensile strength of specimen ① was measured at 622.08 MPa, with a strain at a break of 1.35%. The elastic modulus of the carbon fiber specimen was calculated to be 510 GPa.

Figure 5

(a) Carbon fiber tensile stress–strain curve, (b) high-temperature fireproof cloth tensile stress–strain curve, (c) carbon fiber tensile force and displacement change curve, (d) high-temperature fireproof cloth force and displacement change curve, (e) carbon fiber specimen tensile breakage picture, and (f) high-temperature fireproof cloth specimen tensile breakage picture.

As illustrated in Figure 5(b) and (d), the high-temperature fireproof cloth exhibits a greater stress concentration and lower stiffness compared to the carbon fiber specimen. Both specimens fracture more rapidly. The stress–strain curve for specimen ③ of the high-temperature fireproof cloth, as shown in Figure 5(b), indicates that fracture occurs abruptly at the maximum load, with a predominantly linear stress–strain relationship observed prior to fracture. The results indicate that the tensile strength of specimen ③ is 222.36 MPa, the strain at break is 2.29%, and the modulus of elasticity is 13.18 GPa.

The fitting of the intrinsic parameters was conducted using Origin software, and the goodness-of-fit value was employed to assess the quality of the fit. A value closer to 1 indicates a better match between the fit curve and the experimental data. Generally, a value greater than 0.9 is considered indicative of a good fit. As illustrated in Figure 6(a) and (b), both the carbon fiber and the high-temperature fireproof cloth satisfy these criteria.

Figure 6

(a) Carbon fiber intrinsic parameter curves and (b) fitted curves of the intrinsic parameter of high-temperature fireproof fabrics.

Integrating the experimental data, the final resulting intrinsic parameters of the two materials are shown in Table 3.

Table 3

Intrinsic parameters of the two materials

Material	Density (kg·m⁻³)	Young’s modulus (MPa)	Poisson’s ratio
Carbon fiber	1.6 × 103	510,000	0.307
High-temperature fireproof cloth	1.952 × 102	13,180	0.316

2.3 Loading test of composite mechanical plates

To validate the accuracy of the material constitutive model determined for the fairing, a comparison was conducted between the loading tests of composite mechanical plates cut from the fairing and the simulation processes based on the measured constitutive parameters (as described in Section 2.1). The validity of the material parameters was assessed through the magnitude of deformation. The tests in this study adhered to the general test standard GJB 67.1-85, which outlines the strength and stiffness specifications for military aircraft. In conjunction with the characteristics of the composite mechanical plates, appropriate loading test methods were developed. The raw materials used for testing included carbon fiber prepreg cloth plates and high-temperature fire-resistant cloth plates, both manufactured by Harbin Aircraft Industry Group. Each layer of these materials had a thickness of 2.3 mm. The resin matrix of the high-temperature fire-resistant cloth plate was composed of epoxy resin. The specific geometric parameters are detailed in Table 4.

Table 4

Composite mechanical plate dimensions

Material	Length (mm)	Width (mm)	Height (mm)
Carbon fiber prepreg board	490	390	2.3
High-temperature fireproof cloth board	490	390	2.3

To accurately measure the stress, strain, and deformation values of the specimens, the test setup platform illustrated in Figure 7 is utilized. To comprehensively gather performance data of the specimens under various placement configurations, this experiment specifically establishes two placement modes: the horizontal arrangement and the vertical arrangement. Given the brittle nature of the composite mechanical plates, the test employs a loading operation method designed to prevent unexpected damage to the specimens or uneven force distribution during the testing process. In this method, one end of the specimen is securely clamped and fixed, while the other end is gradually loaded by placing thin iron sheets. The loading test procedures for the two types of composite mechanical plates, made from different materials, are identical. To clearly elucidate the test process, only the scenario in which the carbon fiber prepreg cloth plate is placed horizontally will be used as an example for illustration. The specific test steps are as follows:

The specimen is secured in a 5-in. tiltable clamping fixture and is loaded by placing thin pieces of iron.
Starting from 0 kg, place a loading iron on the prepreg plate and observe the surface condition for each additional loading iron applied.
Collect the values of stress, strain, and deformation using a micrometer and a strain gauge.

Figure 7

Loading test setup: (a) strain collector, (b) strain collection process curve, and (c) test building stand.

The strain collector (Figure 7(a)) can directly display the strain data processing map (Figure 7(b)) using the Sigma integrated testing software.

3 Finite-element simulation (FEM)

3.1 Composite mechanical plate simulation

3.1.1 FEA of composite mechanical plates

3.1.1.1 Design of composite mechanical plates

As described in Section 1.3, a numerical simulation model of the carbon fiber prepreg cloth plate and the high-temperature fire-resistant cloth plate was established using ABAQUS software to compare the deformations and investigate the rationality of the constitutive parameters. The basic material constitutive parameters are presented in Table 3, while the dimensional parameters are detailed in Table 4.

3.1.1.2 Finite-element modeling and calculation of composite mechanical plates

The finite-element model of the composite mechanical plate is constructed using shell elements. In this model, the fiber length direction of the prepreg plate corresponds to the X-axis, the width direction corresponds to the Y-axis, and the thickness corresponds to the Z-axis. The material’s elasticity is set to isotropic. One end of the prepreg board is fixed, while a load is applied to the opposite end. ABAQUS finite-element software was utilized to mesh the geometric model, resulting in an optimized finite-element calculation model. The carbon fiber prepreg panel structure was discretized using S4R elements, and the model was divided into 7,742 S4R elements.

Simulate the actual restrained load conditions of the composite mechanical plate during the loading test, as illustrated in Figure 8. Designate the midpoint of the left end of the composite mechanical plate as the solid support boundary, with a boundary length of 125 mm and a width of 15 mm. Position the reference point RP1 at the right end of the mechanical plate, coupling RP1 with the loading area of the iron sheet. Simultaneously, apply concentrated forces of 0.9, 1.8, 2.7, and 3.6 N in the positive Z-direction at this point, respectively.

Figure 8

Real constraint loads: (a) lateral arrangement and (b) vertical arrangement.

3.1.2 Comparison of composite mechanical plate simulation and test results

By solving the finite-element equations, the simulation results for the composite mechanical plate are presented in Figures 9 and 10. Here, U represents the total displacement, U1 indicates the displacement of the node in the X direction, U2 denotes the displacement of the node in the Y direction, and U3 signifies the displacement of the node in the Z direction. S represents the total stress, with S11 indicating the normal stress in the X direction, S12 representing the shear stress between the X and Y directions, and S22 denoting the normal stress in the Y direction. The stress and displacement distributions of the carbon fiber prepreg board under a force of 0.9 N reveal that the maximum displacement (U) is 0.2739 mm, while the maximum stress (S) is 2.708 MPa.

Figure 9

Displacement cloud results of 0.9 N vertical arrangement of carbon fiber prepreg panels: (a) U, (b) U1, (c) U2, and (d) U3.

Figure 10

Stress cloud results of 0.9 N vertical arrangement of carbon fiber prepreg panels: (a) S, (b) S11, (c) S22, and (d) S12.

To facilitate a comparison with the results of the composite mechanical plate loading tests, the numerical results from the mechanical plate simulation model are extracted at the location of the node cell RP-1. Based on the obtained numerical results and the test data, a line graph is plotted for isotropic comparison to verify the reliability of the fairing model. Since this article focuses solely on the shape study of the fairing, only the displacement results of the composite mechanical plate are compared.

Figure 11 illustrates the trend of deformation with pressure for carbon fiber and high-temperature fireproof cloth panels in both tests and simulations. From Figure 11(a) and (b), it is evident that the deformation data for the composite mechanical plates in the transverse arrangement are significantly greater than those in the vertical arrangement. For instance, in the case of the carbon fiber plate, the deformation value in the transverse arrangement exceeds that in the vertical arrangement under the same applied force, primarily due to the anisotropic nature of composite materials. In the horizontal arrangement of the carbon fiber plate, the maximum error in deformation is 0.34 mm when the pressure is 2.7 N. In contrast, the error in the test and simulation results for the vertical arrangement is relatively smaller, with the largest error being only 0.18 mm. Among all the groups in the vertical arrangement of the carbon fiber plate, the smallest error recorded is 0.03 mm at a loading of 2.7 N, resulting in a relative error ratio of 9.68%. Furthermore, the deformation data for the carbon fiber boards indicate that most of the test group data are higher than those of the simulation group. This discrepancy may be attributed to various errors during the testing process, such as measurement inaccuracies and operational mistakes, which could lead to inflated test results. In the case of the high-temperature fireproof cloth panels, the maximum error occurred in the transverse arrangement at a force of 2.7 N, with a relative error proportion of 15.51%.

Figure 11

(a) Variation of deformation of carbon fiber prepreg board with load and (b) variation of deformation of high-temperature fireproof cloth board with the load.

The test results indicate that, under a load of 3.6 N, the maximum absolute error in the transverse deformation of the high-temperature fireproof cloth test material is 0.90 mm, with a maximum stress of 19.35 MPa. In comparison, the maximum absolute error in the transverse deformation of the carbon fiber board test material is 0.201 mm, and the maximum stress reaches 12.74 MPa.

The theoretical data indicate that the deformation of the composite mechanical plate should increase linearly with the applied force. However, slight deviations may occur during testing due to constraints and artificial arrangements. Overall, the deformation trends of carbon fiber prepreg and high-temperature fireproof cloth panels in both the tests and simulations are comparable, with relative errors remaining within 20%. Therefore, it can be concluded that the fairing specimen model meets the necessary requirements and is suitable for conducting studies on the formability of aerospace composites-based fairings.

3.2 Finite-element simulation of fairing structure

3.2.1 Aircraft thin-walled parts assembly process analysis

There is a significant number of thin-walled components in aircraft structures, including skins and long trusses in wings and fuselage panels. Currently, the assembly process for thin-walled aircraft parts encompasses four key stages: positioning, clamping, connecting, and releasing spring back. The assembly deviation of thin-walled aircraft components can arise during the assembly process due to the combined influence of various factors, such as deviations generated during manufacturing, the effects of clamping force, and the application of connection force. Furthermore, these assembly deviations can propagate and accumulate as the assembly process progresses, ultimately adversely affecting the assembly accuracy of the aircraft.

3.2.1.1 Positioning phase

Deterministic positioning of thin-walled aircraft components is achieved by applying the 3–2–1 principle, along with the use of specialized tooling during the assembly process [43]. In this context, the thin-walled component is treated as a rigid body, meaning that it is assumed to be non-deformable under elastic conditions. The deterministic positioning method adheres to the 3–2–1 positioning principle, which fully constraints the six degrees of freedom of the component to prevent any translational or rotational movement. This approach establishes the positional relationship of the component in space, as illustrated in Figure 12.

Figure 12

Part deterministic model.

Based on the deterministic localization method, the constraint equation for the part at the localization point is established as follows:

(6) ϕ ( r , P ) = 0 ,

where r = ( x , y , z , α , β , r ) T represents the position vector of a part and P = ( p 1 T , p 2 T , p 3 T , p 4 T , p 5 T , p 6 T ) T is the set of localization vectors.

The relationship between part deviation and positioning deviation is established using the linear variational method

(7) δ r j = − J j − 1 ϕ P j δ P i ,

where J j = [ J j 1 , J j 2 , J j 3 , J j 4 , J j 5 , J j 6 , ] T represents the Jacobi matrix and ϕ p j denotes the constraint variable of the component.

In the assembly stage of thin-walled components, there are initial errors and fixture errors, namely:

(8) δ P j = V j K + V j C ,

where δ P j represents the positioning point deviation, V j K denotes the initial error established for part assembly, and V j C indicates the fixture error set.

The formula for continuous deviation accumulation can be expressed as follows:

(9) V j K ′ = δ r j + V j K .

3.2.1.2 Clamping stage

During the clamping process, the clamping force induces elastic deformation in the thin-walled component. Based on the equation provided (9), it can be determined that the error at the clamping point of the component during the clamping stage is

(10) V j K B ′ = δ r j + V j K B .

Assuming that the fixture error corresponding to the clamping point is V j C B , the equation for the displacement of the part controlled by the clamping force during movement can be expressed as follows:

(11) V j K B ″ = V j K B + V j C B ′ .

According to the theory of super-element stiffness matrices, it is known that

(12) I j L ⋅ [ V j K B ″ , δ V j K B ] T = [ F j B , 0 ] ,

where I j L represents the stiffness matrix under deterministic positioning, δ V j K B denotes the part deviation caused by the clamping force, and F j B refers to the over-positioning clamping force.

The formula for clamping force deviation is as follows:

(13) δ V j K B = V j K B S j L ,

where S j L represents the sensitivity between part deviation and over-positioning point deviation, reflecting the degree of correlation and the regularity of the influence that part deviation has on over-positioning point deviation.

3.2.1.3 Connection phase

The joining process (e.g., riveting, bolting) is characterized by joining forces that induce stresses and deformations in the components. In the case of riveting, for instance, the stress state of the component is further modified when the rivet is subjected to the connection force. A correlation exists between the deviation of the riveting point and the riveting force in thin-walled components

(14) C j P = V j K P ″ K j B ,

(15) C ( j + 1 ) P = V ( j + 1 ) K P ″ K ( j + 1 ) B ,

where C j P and C ( j + 1 ) P represent the riveting forces acting on two thin-walled components that are connected to one another, and K j B and K ( j + 1 ) B denote the stiffness matrices associated with these two thin-walled parts in the over-positioning scenario.

3.2.1.4 Rebound release phase

During the assembly operation, whether the parts are nested, fastened, or pressed against each other, assembly stresses will be generated within the thin-walled components, leading to elastic deformation. These elastic deformations accumulate throughout the assembly process. Once the entire assembly is completed and the external forces stabilize, the thin-walled parts, having undergone a series of prior elastic deformations, will experience a redistribution and release of internal stress. This process inevitably results in a rebound phenomenon.

Assuming that the assembly spring back is denoted as W and the assembly spring back force is represented by C U

(16) C U = C j P + C j + 1 P .

From the sensitivity matrices S j P ″ and S ( j + 1 ) P ″ , we have

(17) S j P ″ = [ I U ] − 1 I j B ,

(18) S ( j + 1 ) P ″ = [ I U ] − 1 I ( j + 1 ) B .

According to the influence coefficient method, the relationship can be established as follows:

(19) W = S j P ″ V j K P ″ + S ( j + 1 ) P ″ V ( j + 1 ) K P ″ .

Under the assumption of linear elasticity, let I U represent the super-element stiffness matrix and δ V j K U denote the assembly rebound error following the riveting of the components. It can be demonstrated that

(20) I U ⋅ [ W , δ V j K U ] T = [ C U , 0 ] T .

From Eq. (20)

(21) δ V j K U I = S u W ,

where S u is the sensitivity matrix of the part assembly spring back error.

After the release of the over-locating fixture, the assembly will also experience a certain amount of rebound deformation. Furthermore, it is assumed that the deviation V j K P ‴ following the release of the riveted joint is

(22) V j K P ‴ = V j K P ″ − W .

I A represents the super-element stiffness matrix associated with the two thin-walled components in the deterministic localization scenario, while δ V j K A I denotes the deviation at the over-localization clamping point. Under the assumption of linear elasticity, the relationship between the support force and the deformation at the over-localization clamping point can be derived as follows:

(23) I A ⋅ [ V j K P ‴ , δ V j K A I ] T = [ C j A , 0 ] T .

From this, we can observe

(24) δ V j K A I = S A V j K P ‴ .

The sensitivity matrix of the error at the riveted joint of the part is denoted as S A .

Accurate prediction of spring back is critical for compensating for the resulting deviations and ensuring the accuracy of the final assembly. Throughout the assembly process of thin-walled aircraft components, factors such as manufacturing deviations, clamping forces, and connection forces are interrelated, leading to the continuous transmission and accumulation of assembly deviations. Based on the analysis above, the continuous assembly deviation model can be expressed as follows:

(25) V j K U I = V j K I + ∑ j j + 1 ( S j K L V j K L + S j K B V j K B + S j K P V j C P + S j C L V j C L + S j C B V j C B ) .

3.2.2 Design of fairing structure

The assembly deviation model for aircraft thin-walled components is closely linked to the actual working conditions of these parts and assemblies. Stress and displacement deformation data for the components and assemblies, under real working conditions, are obtained through FEA. This data serves as a foundation for constructing the assembly deviation model. The specific simulation process is illustrated in Figure 13.

Figure 13

Simulation flowchart.

A finite-element simulation model of the fairing is created using shell elements, with the material’s elasticity defined as isotropic. The ABAQUS finite-element software is utilized to mesh the geometric model, resulting in an optimized finite-element calculation model. The fairing structure is primarily discretized using S4R elements, and the model is divided into 38,700 elements (Figure 14).

Figure 14

The helicopter fairing grid diagram.

3.2.3 Constraint settings for the fairing

To investigate the deformation behavior, shape, and overall stiffness distribution of the aerospace composite fairing, it is essential to simulate the planar stresses experienced by the fairing under rigidly supported boundaries across various operating conditions. By applying concentrated forces at different locations and orientations, identify critical points and determine the maximum stress, displacement, and deformation for each operating condition. Based on the research objectives, the changes in shape and performance of the fairing are examined in two distinct ways, as illustrated in Figures 15 and 16.

Figure 15

Schematic diagram of fairing case 1 constraints.

Figure 16

Schematic diagram of fairing case 2 constraints: (a) L = 200 mm, (b) L = 600 mm, and (c) L = 1,000 mm.

The first type of constraint, known as overall boundary loading, is fixed at one end while being loaded at the opposite end. In this context, X i represents the distance from the fixed boundary, and F denotes the magnitude of the applied external force. The specific implementation of the X _i–F relationship is illustrated in Figure 15 and detailed in Table 5. The left end of the fairing is designated as the fixed boundary, with the boundary width varying according to the working conditions. The reference point, RP-2, is located at the right end of the fairing and is coupled with the entire area of the fairing. Different values of the concentrated force are applied in the Z-positive direction at this point, with a total of five working conditions established in this study.

Table 5

Helicopter fairing case 1 setting

Serial no.	Binding settings
Serial no.	X i (boundary width of consolidation, mm) – F (external force, N)
1	X10–F1,000	X10–F2,000	X10–F3,000	X10–F4,000	X10–F5,000
2	X20–F1,000	X20–F2,000	X20–F3,000	X20–F4,000	X20–F5,000
3	X40–F1,000	X40–F2,000	X40–F3,000	X40–F4,000	X40–F5,000
4	X60–F1,000	X60–F2,000	X60–F3,000	X60–F6,000	X60–F5,000
5	X80–F1,000	X80–F2,000	X80–F3,000	X80–F8,000	X80–F5,000

Note: Xx1–Fx2 denotes the working condition number of the fairing edge loading, where x1 represents the width of the fairing’s solid support boundary, and x2 indicates the magnitude of the applied external force. For example, X10–F1,000 signifies the working condition in which X10 corresponds to a fairing solid support boundary width of 10 mm, with an external force of 1,000 N applied at the RP-2 point.

To further investigate the shape and performance of the fairing, this thesis simulates the working conditions encountered during the actual assembly process, specifically the second (four-point fixation) constraint method, as illustrated in Figure 16. This method involves altering the clamping position of the fixture to sequentially secure the fairing, allowing for the observation of how the applied displacement load force and the clamping fixation position affect the shape and performance of the fairing. In this context, L represents the interval distance of the fixture’s clamping and fixing area, F1 denotes the bottom displacement load force, and F2 indicates the top displacement load force. The specific settings for the working conditions, including L, F1, and F2, are detailed in Table 6.

Table 6

Helicopter fairing case 2 setting

Serial no.	Binding settings
Serial no.	Retention interval width (L) (mm) – top (F1) (mm) – bottom (F2) (mm)
1	L200–0.0–0.0	L600–0.0–0.0	L1,000–0.0–0.0
	L200–0.0–0.5	L600–0.0–0.5	L1,000–0.0–0.5
	L200–0.0–1.0	L600–0.0–1.0	L1,000–0.0–1.0
	L200–0.0–1.5	L600–0.0–1.5	L1,000–0.0–1.5
	L200–0.0–2.0	L600–0.0–2.0	L1,000–0.0–2.0
2	L200–0.5–0.0	L600–0.5–0.0	L1,000–0.5–0.0
	L200–0.5–0.5	L600–0.5–0.5	L1,000–0.5–0.5
	L200–0.5–1.0	L600–0.5–1.0	L1,000–0.5–1.0
	L200–0.5–1.5	L600–0.5–1.5	L1,000–0.5–1.5
	L200–0.5–2.0	L600–0.5–2.0	L1,000–0.5–2.0
3	L200–1.0–0.0	L600–1.0–0.0	L1,000–1.0–0.0
	L200–1.0–0.5	L600–1.0–0.5	L1,000–1.0–0.5
	L200–1.0–1.0	L600–1.0–1.0	L1,000–1.0–1.0
	L200–1.0–1.5	L600–1.0–1.5	L1,000–1.0–1.5
	L200–1.0–2.0	L600–1.0–2.0	L1,000–1.0–2.0
4	L200–1.5–0.0	L600–1.5–0.0	L1,000–1.5–0.0
	L200–1.5–0.5	L600–1.5–0.5	L1,000–1.5–0.5
	L200–1.5–1.0	L600–1.5–1.0	L1,000–1.5–1.0
	L200–1.5–1.5	L600–1.5–1.5	L1,000–1.5–1.5
	L200–1.5–2.0	L600–1.5–2.0	L1,000–1.5–2.0
5	L200–2.0–0.0	L600–2.0–0.0	L1,000–2.0–0.0
	L200–2.0–0.5	L600–2.0–0.5	L1,000–2.0–0.5
	L200–2.0–1.0	L600–2.0–1.0	L1,000–2.0–1.0
	L200–2.0–1.5	L600–2.0–1.5	L1,000–2.0–1.5
	L200–2.0–2.0	L600–2.0–2.0	L1,000–2.0–2.0

Note: The working condition number for the four-point positioning of the fairing is designated as Lx1–x2–x3. In this notation, x1 represents the width of the fixed support interval of the fairing, x2 indicates the magnitude of the displacement load applied at the top, and x3 denotes the magnitude of the displacement load applied at the bottom. For example, L200–0.0–0.0 signifies a working condition in which the width of the fairing’s fixed support interval is 200 mm, the displacement load at the top is 0.0 mm, and the displacement load at the bottom is also 0.0 mm.

4 Results and discussions

4.1 Simulation results of the overall boundary loading of the fairing

Based on Case 1 (overall boundary loading), the constraint force of the fairing was established, and the stress and displacement results for the fairing were obtained. Due to the similar shape of the resultant data cloud, the displacement cloud results for the fairing were only illustrated for Case No. X20, where the width of the solidly supported boundary was 20 mm. As shown in Figure 17, the maximum displacement of the fairing in this case was 8.884 mm.

Figure 17

Displacement cloud of X20 under different applied forces: (a) 1,000 N, (b) 2,000 N, (c) 3,000 N, (d) 4,000 N, and (e) 5,000 N.

The displacement and stress results obtained from the fairing under various constraint settings in Case I are organized and plotted in line graphs to examine the overall stiffness distribution and deformation behavior of the fairing. The stress trend of the fixed boundary variation of the fairing under different gradient forces is illustrated in Figure 18. The stress experienced by the fairing exhibits a decreasing trend as the constraint width increases. Specifically, as the constraint width increases from 10 to 80 mm, the stress decreases gradually. For instance, when a force of 1,000 N is applied, the stress at a 10 mm confinement width is 429.6 MPa, whereas the stress at an 80 mm confinement width drops to only 13.31 MPa. Notably, the reduction in stress becomes less pronounced with increasing confinement width. When comparing the 10 and 20 mm constraint widths, the stress decreases by 79.25%. In contrast, when comparing the 60 and 80 mm constraint widths, the stress decreases by 46.2%. This indicates that as the constraint width increases, the stress reduction effect gradually diminishes. This occurs because a wider constraint width allows the structure to be more stably supported, thereby weakening the effect of the stress–strain limit. In cases of narrower constraint widths, the phenomenon of material stress concentration is pronounced, as the stress is still significantly below its stress–strain limit. At this point, a slight increase in constraint width can substantially disperse the stress, resulting in a notable reduction in stress. However, once the constraint width reaches a certain threshold, the distribution of stress becomes relatively uniform, approaching the material’s allowable stability under the stress–strain limit. Consequently, any further increase in width yields only marginal improvements in stress dispersion, leading to a smaller reduction in stress.

Figure 18

(a) Variation of maximum stress with load for different fixed boundaries and (b) schematic diagram of maximum displacement with load for different fixed boundaries.

The deformation characteristics indicate that the amount of displacement deformation of the fairing exhibits a gradually decreasing trend as the constraint width increases. This trend parallels the relationship between stress deformation and load. Consequently, we can draw the same conclusion: a wider constraint width provides a larger support area, thereby reducing the impact of external forces on the fairing and decreasing the amount of displacement deformation. In contrast, a narrower constraint width fails to offer adequate support, leading to an increase in displacement deformation. Furthermore, the data reveal that, at certain constraint widths, the amount of displacement deformation experiences abrupt changes. For instance, with a constraint width of 10 mm, the displacement deformation resulting from an external force ranging from 1,000 to 6,000 N increases sharply from 6.754 to 13.44 mm, nearly doubling. This phenomenon occurs because the constraint width limits the fairing’s ability to deform freely, causing a significant increase in deformation when the external force surpasses a specific threshold value.

4.2 Simulation results of fairing four-point localization loading

The stress data for the fairing under various combinations of top and bottom displacement loads, at clamping distances of 200, 600, and 1,000 mm, were obtained using ABAQUS finite-element software. The data clearly indicate that the stress values increase with the bottom displacement load, and the rate of stress growth varies depending on the clamping distance.

4.2.1 Effect of clamping distance

When the displacement load remains constant, the stress value increases significantly as the clamping distance increases from 200 to 600 mm and then to 1,000 mm. Specifically, when a top displacement load of 0 mm and a bottom displacement load of 1 mm are applied, the stresses recorded are 5.403 MPa at a clamping distance of 200 mm, 21.81 MPa at 600 mm, and 204.3 MPa at 1,000 mm. These values represent increases of 3.96 times and 37.8 times, respectively. Assuming that the stress at a clamping distance of 200 mm is considered the baseline value (1) under the same displacement load, the influence percentage can be estimated by calculating the relative growth ratio of the stress at different clamping distances. In this example, the increase ratio from 200 to 600 mm is 3.04, while the increase ratio from 600 to 1,000 mm is 8.37. Consequently, at this displacement load, the influence share from 200 to 600 mm is approximately 26.7%, and the influence share from 600 to 1,000 mm is approximately 73.3%.

When comparing the same displacement load across different clamping distances, the deformation does not follow a straightforward pattern as the clamping distance increases. For a lower displacement load of 1 mm, the deformation at a clamping distance of 200 mm is 1.032 mm; at 600 mm, it is 1.036 mm; and at 1,000 mm, it is 1.027 mm. This indicates that variations in clamping distance do not lead to a monotonically increasing or decreasing deformation; rather, the relationship is relatively complex.

Analyzing the three aspects of how clamping distance affects the deformation, stiffness, and stability of the fairing. When the clamping distance is small, structural deformation primarily concentrates near the clamping position, exhibiting a localized nature. As the clamping distance increases, the range of force conduction expands, making large-scale deformations, such as overall bending and twisting, more likely to occur. When the clamping distance is small, the local stiffness near the fixture increases; however, the overall stiffness remains uneven. As the clamping distance increases, the distribution of overall stiffness becomes more uniform, although the overall stiffness value may decrease relatively. With a small clamping distance, the local area remains relatively stable. However, when the entire structure is subjected to complex external forces, local damage is likely to occur due to uneven stiffness, which can compromise stability. Conversely, with a larger clamping distance, the entire structure becomes susceptible to instability phenomena, such as shaking and tilting, due to dispersed constraints and insufficient support. In conclusion, the clamping distance significantly influences the deformation, stiffness, and stability of the fairing. A smaller clamping distance results in the structure exhibiting characteristics such as localized deformation and uneven stiffness, while certain local parts may remain relatively stable. However, the entire structure becomes more susceptible to complex external forces. Conversely, increasing the clamping distance is likely to result in overall deformation and more uniform stiffness, but it may also lead to a decrease in overall stability.

4.2.2 Effect of displacement load

For a fixed clamping distance, the stress value increases nearly linearly with the increase in the bottom displacement load. As illustrated in Figure 19(a), taking a clamping distance of 200 mm as an example, when the bottom displacement load is increased from 0 to 0.5, 1, 1.5, and 2 mm, the stress rises from 0 to 2.701, 5.403, 8.104, and 10.81 MPa, respectively, demonstrating a clear linear increasing trend. Similarly, for a clamping distance of 600 mm, the contribution of each 0.5 mm increment in the bottom displacement load to the stress growth is calculated. When the bottom displacement load increases from 0 to 0.5 mm, the stress increases by 2.701 MPa, resulting in a contribution rate of 25%. When the load increases from 0.5 to 1 mm, the stress again increases by 2.702 MPa, maintaining a contribution rate of 25%. This pattern continues, with each 0.5 mm increment in displacement load contributing equally to the stress increase, which remains at 25%. However, the overall stress change trend of the fairing at 200 mm is relatively flat compared to that at 600 and 1,000 mm.

Figure 19

(a) Variation of maximum stress with bottom displacement load at clamping distance L = 200 mm; (b) maximum stress variation with bottom displacement load at clamping distance L = 600 mm; and (c) maximum stress with bottom displacement load at clamping distance L = 1,000 mm.

Under the condition of maintaining a constant clamping distance, the relationship between displacement load and deformation is analyzed. Using a clamping distance of 200 mm as an example, the bottom displacement load begins at 0 mm and gradually increases to 2 mm in increments of 0.5 mm. The corresponding deformation values are 0, 0.516, 1.032, 1.548, and 2.064 mm, respectively. The relative deviation is minimal, remaining within ±3%, which sufficiently demonstrates that the growth pattern exhibits a high degree of homogeneity.

Expanding the scope of the study, the aforementioned experimental procedure was repeated with clamping distances set at 600 and 1,000 mm, respectively. The data obtained demonstrated a trend consistent with linear behavior. At a clamping distance of 600 mm, the standard deviation of each corresponding deformation increment relative to the mean value is approximately 2.5% on average, while at a clamping distance of 1,000 mm, this proportion is about 2%. The slight degree of dispersion indicates a relatively strong linear correlation between displacement loads and deformations. In other words, under the specified clamping boundary conditions, the displacement load, acting as an external excitation, establishes a nearly ideal proportional relationship with the amount of deformation. This implies that each unit of applied displacement load contributes to an equal and stable increase in deformation.

A comprehensive analysis indicates that the displacement load is the primary factor influencing fairing deformation, accounting for a significant portion of the changes observed. In contrast, the clamping distance is the critical factor affecting fairing stress, which primarily determines the variations in stress magnitude.

Displacement load plays a critical role in deformation, and a large displacement load can cause significant geometric alterations to the fairing, compromising its originally designed contour. This directly impacts its aerodynamic shape, thereby disrupting the airflow during flight and diminishing the fairing’s functionality. The clamping distance is a key factor influencing stress; an inappropriate clamping distance can trigger high-stress concentrations, which may lead to localized material damage. Over time, this accumulation of stress can result in structural fatigue or even failure, jeopardizing the overall stability and reliability of the fairing and compromising the safety of the internal equipment.

5 Conclusions

In this article, by constructing a numerical simulation model of the assembly process of the composite fairing, the stress and displacement deformation of this model under various working conditions, with the aim of identifying the primary factors that influence changes in the shape and performance of the fairing, summarizing the deformation patterns related to the overall stiffness distribution of the fairing and present the following conclusions:

Overall stiffness distribution deformation law: The overall stiffness of the fairing is influenced by the synergistic effects of fixed boundary constraints and external forces. The stress demonstrates a negative correlation with the width of the fixed boundary constraints. As the constraint width increases, the stress consistently decreases, with the rate of decline transitioning from rapid to gradual. Specifically, the stress reduction rate is 79.25% when the constraint width ranges from 10 to 20 mm, and it slows to 46.2% for the 60–80 mm constraint range. Displacement deformation increases in tandem with the growth of external forces. For instance, with a 10 mm constraint width, when the external force rises from 1,000 to 6,000 N, the displacement increases from 6.754 to 13.44 mm, representing a 99.0% increase. This indicates that under narrower constraints, even a slight increase in external force can lead to a significant rise in deformation. The underlying reason is that narrow constraints limit the fairing’s ability to deform freely; thus, once the external force exceeds a certain threshold, the deformation will escalate dramatically.
Both the clamping distance and the displacement load are critical factors influencing the deformation (characterized by stress) of the fairing, and their effects on deformation are quite significant. When the displacement load is low, the stress variation resulting from changes in clamping distance is relatively minor. However, as the displacement load gradually increases, the impact of clamping distance changes on the stress of the fairing becomes more pronounced. Regarding the displacement load, regardless of how the clamping distance is altered, its effect on stress consistently exhibits a relatively stable linear increasing trend. Furthermore, the contribution to stress growth corresponding to each unit increment in displacement load remains relatively constant.
The shape and performance of the fairing are influenced by multiple factors, among which displacement load and clamping distance are the principal ones. Displacement load contributes substantially to the variation in fairing deformation, making it a crucial determinant of deformation. In contrast, the clamping distance dominates the change in fairing stress, acting as the core factor dictating stress levels. When the displacement load remains constant, the stress exhibits a marked upward trend as the clamping distance gradually widens.

There are discrepancies in the influence weights across different spacing intervals. For instance, the stress rises from 5.403 MPa at a 200 mm clamping distance to 21.81 MPa at 600 mm and 204.3 MPa at 1,000 mm, representing increases of 3.96 times and 37.8 times, respectively. The influence proportion of the clamping distance from 200 to 600 mm is 26.7%, and from 600 to 1,000 mm, it is 73.3%. With a fixed clamping distance, the stress grows almost linearly with the increment of the bottom displacement load, and the contribution of each equal displacement load increment to stress growth is more consistent. At different clamping distances, displacement load and deformation are highly linearly correlated. For example, at a 200-mm clamping distance, the difference between adjacent deformations is 0.516 mm, with a relative deviation within ±3%. At 600 and 1,000 mm, the standard deviation of the deformation increment as a proportion of the mean value is 2.5 and 2%, respectively. In low-displacement load scenarios, the effect of clamping distance on stress is relatively minor. However, as the displacement load increases, the influence of clamping distance becomes more significant. These two factors interact to shape the stress state and deformation of the fairing, ultimately determining its shape and performance.

Funding information: This work was financially supported by the Fundamental Research Funds for the Central Universities (No. BLX202230) and the National Natural Science Foundation of China (Grant No. 52375140).
Author contributions: All authors have accepted responsibility for the entire content of this manuscript and approved its submission.
Conflict of interest: The authors state no conflict of interest.
Data availability statement: The datasets generated and/or analyzed during the current study are available from the corresponding author on reasonable request.

References

[1] Gao, H., X. Li, B. Li, Q. Wu, Y. Ma, X. Jian, et al. Residual stress and microstructure of Ti6Al4V treated by thermal-vibratory stress relief process. Journal of Materials Research and Technology, Vol. 18, 2022, pp. 5161–5181.10.1016/j.jmrt.2022.04.137Search in Google Scholar

[2] Song, H., H. Gao, Q. Wu, and Y. Zhang. Residual stress relief mechanisms of 2219 Al–Cu alloy by thermal stress relief method. Reviews on Advanced Materials Science, Vol. 61, No. 1, 2022, pp. 102–116.10.1515/rams-2022-0019Search in Google Scholar

[3] Jiang, S., H. Liu, Y. Zuo, D. Sun, Y. Yang, D. Zhao, et al. Cutting vibration characteristics and mechanisms in the end milling of superalloy honeycomb core with ice fixation clamping. Mechanical Systems and Signal Processing, Vol. 215, 2024, id. 111422.10.1016/j.ymssp.2024.111422Search in Google Scholar

[4] Yao, G. and Z. Liu. Analytical modelling for residual stress prediction in multi-step side milling of GH4169 thin-wall parts based on deformation. Journal of Materials Research and Technology, Vol. 32, 2024, pp. 1984–1995.10.1016/j.jmrt.2024.08.042Search in Google Scholar

[5] Li, Y., A. Yang, Y. Liu, Y. Gao, J. Zhou, Y. Dong, et al. Analysis of warping defect formation mechanisms in hot molding of CF/PEEK thin-wall structures and their influence on mechanical properties. Thin-Walled Structures, Vol. 207, 2025, id. 112740.10.1016/j.tws.2024.112740Search in Google Scholar

[6] Guo, F., Q. Xiao, S. Xiao, and Z. Wang. Analysis on quantifiable and controllable assembly technology for aeronautical thin-walled structures. Robotics and Computer-Integrated Manufacturing, Vol. 80, 2023, id. 102473.10.1016/j.rcim.2022.102473Search in Google Scholar

[7] Liu, S., H. Yu, Z. Xia, and K. Chen. A new virtual functional element method for deviation prediction of assembled structures with parallel connection chain. CIRP Journal of Manufacturing Science and Technology, Vol. 48, 2024, pp. 42–54.10.1016/j.cirpj.2023.11.006Search in Google Scholar

[8] Ding, B., J. Kong, W. Wang, Z. Wang, J. Xiao, and Q. Zhang. Investigation on a semi-active vibration attenuation device with follow-up support technology for mirror milling of thin-walled workpieces. Mechanical Systems and Signal Processing, Vol. 224, 2025, id. 12053.10.1016/j.ymssp.2024.112053Search in Google Scholar

[9] Li, B., H. Gao, H. Deng, H. Pan, and B. Wang. Investigation on the influence of the equivalent bending stiffness of the thin-walled parts on the machining deformation. The International Journal of Advanced Manufacturing Technology, Vol. 101, No. 5–8, 2018, pp. 1171–1182.10.1007/s00170-018-2987-5Search in Google Scholar

[10] Ge, G., Y. Xiao, J. Lv, and Z. Du. A non-iterative compensation method for machining errors of thin-walled parts considering coupling effect of tool-workpiece deformation. Manufacturing Letters, Vol. 41, 2024, pp. 287–295.10.1016/j.mfglet.2024.09.034Search in Google Scholar

[11] Yue, C., R. Jia, X. Zhu, B. Geng, and J. Zhang. Research on online deformation monitoring of thin-walled parts driven by digital twin. Digital Engineering, Vol. 3, 2024, id. 100023.10.1016/j.dte.2024.100023Search in Google Scholar

[12] Gao, H., Y. Zhang, Q. Wu, and B. Li. Investigation on influences of initial residual stress on thin-walled part machining deformation based on a semi-analytical model. Journal of Materials Processing Technology, Vol. 262, 2018, pp. 437–448.10.1016/j.jmatprotec.2018.04.009Search in Google Scholar

[13] Xue, D., Y. Li, H. Zhang, X. Tong, B. Gao, and J. Yu. Reliability-based robust optimization design for tolerance of aerospace thin-walled components based on surrogate model. Advanced Engineering Informatics, Vol. 62, 2024, id. 102754.10.1016/j.aei.2024.102754Search in Google Scholar

[14] Saadat, M., L. Cretin, R. Sim, and F. Najafi. Deformation analysis of large aerospace components during assembly. The International Journal of Advanced Manufacturing Technology, Vol. 41, No. 1–2, 2008, pp. 145–155.10.1007/s00170-008-1464-ySearch in Google Scholar

[15] Saadat, M., R. Sim, and F. Najafi. Modelling and analysis of Airbus wingbox assembly. Proceedings of the Institution of Mechanical Engineers, Part B: Journal of Engineering Manufacture, Vol. 222, No. 6, 2008, pp. 701–709.10.1243/09544054JEM898Search in Google Scholar

[16] Saadat, M. and C. Cretin. Dimensional variations during Airbus wing assembly. Assembly Automation, Vol. 22, No. 3, 2002, pp. 270–276.10.1108/01445150210436482Search in Google Scholar

[17] Li, B., H. Deng, D. Hui, Z. Hu, and W. Zhang. A semi-analytical model for predicting the machining deformation of thin-walled parts considering machining-induced and blank initial residual stress. The International Journal of Advanced Manufacturing Technology, Vol. 110, No. 1–2, 2020, pp. 139–161.10.1007/s00170-020-05862-1Search in Google Scholar

[18] Ge, G., Y. Xiao, X. Feng, and Z. Du. An efficient prediction method for the dynamic deformation of thin-walled parts in flank milling. Computer-Aided Design, Vol. 152, 2022, id. 103401.10.1016/j.cad.2022.103401Search in Google Scholar

[19] Gao, H., Y. Zhang, Q. Wu, and J. Song. An analytical model for predicting the machining deformation of a plate blank considers biaxial initial residual stresses. The International Journal of Advanced Manufacturing Technology, Vol. 93, No. 1–4, 2017, pp. 1473–1486.10.1007/s00170-017-0528-2Search in Google Scholar

[20] Zhou, M., Y. Zhang, and K. Luo. Distortion warping displacement pattern of thin-walled box girders under the influence of non-uniform shear deformation and its corresponding beam-type finite element model. Thin-Walled Structures, Vol. 211, 2025, id. 113108.10.1016/j.tws.2025.113108Search in Google Scholar

[21] Deepak Kumar, G. and B. Panigrahi. Nonlinear free vibrations of a structurally tailored anisotropic pre-twisted thin-walled beam subjected to large deformations. Journal of Sound and Vibration, Vol. 596, 2025, id. 118766.10.1016/j.jsv.2024.118766Search in Google Scholar

[22] Li, Z., Z. Zeng, Y. Yang, Z. Ouyang, P. Ding, J. Sun, et al. Research progress in machining technology of aerospace thin-walled components. Journal of Manufacturing Processes, Vol. 119, 2024, pp. 463–482.10.1016/j.jmapro.2024.03.111Search in Google Scholar

[23] Ju, K., C. Duan, J. Kong, Y. Chen, and Y. Sun. Clamping deformation of thin circular workpiece with complex boundary in vacuum fixture system. Thin-Walled Structures, Vol. 171, 2022, id. 108777.10.1016/j.tws.2021.108777Search in Google Scholar

[24] Wang, Y., X. Chen, Q. Liu, and N. Gindy. Optimisation of machining fixture layout under multi-constraints. International Journal of Machine Tools and Manufacture, Vol. 46, No. 12–13, 2006, pp. 1291–1300.10.1016/j.ijmachtools.2005.10.014Search in Google Scholar

[25] Kaya, N. Machining fixture locating and clamping position optimization using genetic algorithms. Computers in Industry, Vol. 57, No. 2, 2006, pp. 112–120.10.1016/j.compind.2005.05.001Search in Google Scholar

[26] Li, E., J. Zhou, C. Yang, J. Zhao, Z. Li, S. Zhang, et al. Part machining deformation prediction based on spatial-temporal correlation learning of geometry and cutting loads. Journal of Manufacturing Processes, Vol. 92, 2023, pp. 397–411.10.1016/j.jmapro.2023.02.042Search in Google Scholar

[27] Wang, G., Y. Cao, and Y. Zhang. Digital twin-driven clamping force control for thin-walled parts. Advanced Engineering Informatics, Vol. 51, 2022, id. 101468.10.1016/j.aei.2021.101468Search in Google Scholar

[28] Tian, Y., J. Xiao, S. Liu, S. Ma, H. Liu, and T. Huang. Vibration and deformation suppression in mirror milling of thin-walled workpiece through a magnetic follow-up support fixture. Journal of Manufacturing Processes, Vol. 99, 2023, pp. 168–183.10.1016/j.jmapro.2023.04.074Search in Google Scholar

[29] Raghu, A. and S. N. Melkote. Analysis of the effects of fixture clamping sequence on part location errors. International Journal of Machine Tools and Manufacture, Vol. 44, No. 4, 2004, pp. 373–382.10.1016/j.ijmachtools.2003.10.015Search in Google Scholar

[30] Deng, H. and S. N. Melkote. Determination of minimum clamping forces for dynamically stable fixturing. International Journal of Machine Tools and Manufacture, Vol. 46, No. 7–8, 2006, pp. 847–857.10.1016/j.ijmachtools.2005.07.040Search in Google Scholar

[31] Bhatnagar, N., R. Bhardwaj, P. Selvakumar, and M. Brieu. Development of a biaxial tensile test fixture for reinforced thermoplastic composites. Polymer Testing, Vol. 26, No. 2, 2007, pp. 154–161.10.1016/j.polymertesting.2006.09.007Search in Google Scholar

[32] Ratchev, S., S. Liu, W. Huang, and A. A. Becker. An advanced FEA based force induced error compensation strategy in milling. International Journal of Machine Tools and Manufacture, Vol. 46, No. 5, 2006, pp. 542–551.10.1016/j.ijmachtools.2005.06.003Search in Google Scholar

[33] Varadarajan, K. M. and M. L. Culpepper. A dual-purpose positioner-fixture for precision six-axis positioning and precision fixturing. Precision Engineering, Vol. 31, No. 3, 2007, pp. 276–286.10.1016/j.precisioneng.2006.11.002Search in Google Scholar

[34] Vijayalakshmi, S., A. V. Sekar, A. M. Hassan, B. S. Arputharaj, S. S. Jayakumar, H. A. Z. Al-bonsrulah, et al. Multi-perspective structural integrity-based computational investigations on airframe of Gyrodyne-configured multi-rotor UAV through coupled CFD and FEA approaches for various lightweight sandwich composites and alloys. Reviews on Advanced Materials Science, Vol. 62, No. 1, 2023, id. 20230147.10.1515/rams-2023-0147Search in Google Scholar

[35] Fink, A. and C. Einzmann. Discrete tailored asymmetric sandwich structures. Composite Structures, Vol. 238, 2020, id. 111990.10.1016/j.compstruct.2020.111990Search in Google Scholar

[36] Naufal, A. M., A. R. Prabowo, T. Muttaqie, A. Hidayat, J. Purwono, R. Adiputra, et al. Characterization of sandwich materials – Nomex-Aramid carbon fiber performances under mechanical loadings: Nonlinear FE and convergence studies. Reviews on Advanced Materials Science, Vol. 63, No. 1, 2024, id. 20230177.10.1515/rams-2023-0177Search in Google Scholar

[37] Zhang, J., G. Lin, U. Vaidya, and H. Wang. Past, present and future prospective of global carbon fibre composite developments and applications. Composites Part B: Engineering, Vol. 250, 2023, id. 110463.10.1016/j.compositesb.2022.110463Search in Google Scholar

[38] Khatkar, S. K. Hybrid magnesium matrix composites: A review of reinforcement philosophies, mechanical and tribological characteristics. Reviews on Advanced Materials Science, Vol. 62, No. 1, 2023, id. 20220294.10.1515/rams-2022-0294Search in Google Scholar

[39] Wei, X., W. Chen, L. Chen, Q. Wu, and Y. Xin. Investigation of temperature effect on thermo-mechanical property of carbon fiber/PEEK composites. Reviews on Advanced Materials Science, Vol. 63, No. 1, 2024, id. 20240069.10.1515/rams-2024-0069Search in Google Scholar

[40] Sabet, M. Innovations in carbon nanotube polymer composites: Electrical, thermal, and mechanical advancements for aerospace and automotive applications. Synthetic Metals, Vol. 310, 2025, id. 117794.10.1016/j.synthmet.2024.117794Search in Google Scholar

[41] Quan, D., X. Wang, J. Pan, Y. Ma, G. Scarselli, and G. Zhao. Enhancing the fracture toughness of aerospace-grade carbon fibre/epoxy composites by interlaying surface-activated low-melt polyaryletherketone (LMPAEK) meshes. Composites Part B: Engineering, Vol. 287, 2024, id. 111824.10.1016/j.compositesb.2024.111824Search in Google Scholar

[42] Karaboğa, F., F. Göleç, D. E. Yunus, S. Toros, and Y. Öz. Mechanical response of carbon fiber reinforced epoxy composite parts joined with varying bonding techniques for aerospace applications. Composite Structures, Vol. 331, 2024, id. 117920.10.1016/j.compstruct.2024.117920Search in Google Scholar

[43] Liu, Y., X. Tian, J. Geng, M. Zhang, and L. Ma. Modeling andsimu lation analysis of aircraft thin-walled parts assembly devi ation. Machine Tool & Hydraulics, Vol. 48, No. 2, 2020, pp. 138–143.Search in Google Scholar

Received: 2025-01-11

Revised: 2025-03-08

Accepted: 2025-05-16

Published Online: 2025-07-08

This work is licensed under the Creative Commons Attribution 4.0 International License.

Articles in the same Issue

https://doi.org/10.1515/rams-2025-0117

Keywords for this article

composite material; helicopter fairing; thin-walled structure; finite-element simulation

Creative Commons

BY 4.0