Optimizing Structural Integrity of Fighter Aircraft Wing Stations a Finite Element Analysis Approach.pdf

Scientific Paper / Artículo Científico
https://doi.org/10.17163/ings.n32.2024.09
pISSN: 1390-650X / eISSN: 1390-860X
Optimizing Structural Integrity of Fighter
Aircraft Wing Stations: a Finite Element
Analysis Approach
Optimización de la integridad estructural de
las estaciones de ala de aeronaves de combate:
un enfoque de análisis de elementos finitos
Aun Haider Bhutta1,∗ ID
Received: 02-05-2024, Received after review: 29-05-2024, Accepted: 13-06-2024, Published: 01-07-2024
1,∗
Instituto de Aeronáutica y Astronáutica, Universidad Aérea de Islamabad, Pakistán.
Corresponding author✉: aunbhutta@gmail.com.
Suggested citation: Haider Bhutta, Aun. “Optimizing Structural Integrity of Fighter Aircraft Wing Stations: a
Finite Element Analysis Approach,” Ingenius, Revista de Ciencia y Tecnología, N.◦
32, pp. 90-100, 2024, doi:
https://doi.org/10.17163/ings.n32.2024.09.
Abstract Resumen
Modern fighter aircraft are equipped with multiple
stations on the fuselage and under the wings to accom-
modate various external stores, both jettisonable and
non-jettisonable. Each configuration undergoes air-
worthiness certification, including structural analysis
of individual stations within the carriage flight enve-
lope. This study focuses on the structural analysis of
a fighter aircraft wing station within this specified
envelope. To perform this analysis, the wing station is
extracted from the comprehensive global wing model,
creating a sub-model with equivalent stiffness proper-
ties. Utilizing ANSYS Workbench®, Finite Element
Analysis (FEA) is conducted for critical load cases
to determine the Factor of Safety (FoS). The initial
analysis reveals that the wing station has an FoS
of 1.2 under the maximum design load. Prestressed
modal and buckling analyses indicate a 10% increase
in stiffness due to stress-stiffening effects. To further
enhance load-carrying capacity, parametric design
changes are introduced. Increasing the bolt diameter
from 8 mm to 10 mm raises the FoS to 1.33, result-
ing in an 8% increase in the maximum load-carrying
capacity of the wing station. This comprehensive ap-
proach, employing FEA, ensures the wing’s structural
integrity under static load conditions within the car-
riage envelope. The study’s findings support the wing
station’s enhanced performance and contribute to
safer and more efficient aircraft operations.
Los aviones de combate modernos están equipados
con múltiples estaciones en el fuselaje y debajo de
las alas para acomodar varios almacenes externos,
tanto descartables como no descartables. Cada con-
figuración se somete a una certificación de aeron-
avegabilidad, incluido un análisis estructural de las
estaciones individuales dentro de la envolvente de
vuelo del transporte. Este estudio se centra en el aná-
lisis estructural de una estación de ala de un avión de
combate dentro de esta envolvente especificada.Para
realizar este análisis, la estación del ala se extrae del
modelo global integral del ala, creando un submodelo
con propiedades de rigidez equivalentes. Utilizando
ANSYS Workbench®, se realiza un análisis de elemen-
tos finitos (FEA) para casos de carga críticos para
determinar el factor de seguridad (FoS). El análisis
inicial revela que la estación del ala tiene un FoS
de 1,2 bajo la carga máxima de diseño. Los análisis
modales y de pandeo pretensados indican un aumento
del 10 % en la rigidez debido a los efectos de rigidez
por tensión. Para mejorar aún más la capacidad de
carga, se introducen cambios de diseño paramétrico.
El cambio del diámetro del perno de 8 mm a 10 mm
incrementa el FoS a 1,33, lo que da como resultado
un aumento del 8 % en la capacidad máxima de carga
de la estación del ala. Este enfoque integral, que em-
plea FEA, garantiza la integridad estructural del ala
bajo condiciones de carga estática dentro de la envol-
vente del carro. Los hallazgos del estudio respaldan
el rendimiento mejorado de la estación del ala y con-
tribuyen a operaciones de aeronaves más seguras y
eficientes.
Keywords: External store; Weapon Carriage; Static
Structural Analysis; Sub-modelling; Modal Analysis;
Buckling Analysis; Design Optimization
Palabras clave: Tienda externa, transporte de ar-
mas, análisis estructural estático; submodelado, análi-
sis modal, análisis de pandeo, optimización del diseño
90

Haider Bhutta / Optimizing Structural Integrity of Fighter Aircraft Wing Stations: a Finite Element Analysis
Approach 91
1. Introduction
In the last two decades, there has been a notable up-
swing in the adoption of the finite element method
(FEM) for the analysis of complex structures [1]. This
numerical technique provides a highly accurate ap-
proximate solution for problems that lack closed-form
solutions.
In static structural finite element analysis (FEA),
constitutive laws describe how materials respond to ap-
plied loads and define the relationship between stress
and strain. Hooke’s Law, presented in Equation (1), is
the fundamental constitutive law employed for linear
elastic materials. This law provides a linear relation-
ship between the stress (σij) and strain tensors (ϵkl),
represented as follows:
σij = Cijklϵkl (1)
Cijkl is the elastic stiffness tensor, which depends
on material properties such as Young’s modulus E and
Poisson’s ratio (ν)
In a practical FEA scenario, several variables are
known, including material properties (Young’s modu-
lus, Poisson’s ratio and density), geometry (dimensions
and shape of the structure), and boundary conditions
(displacements such as fixed supports or prescribed
movements, and forces such as applied loads or pres-
sure).
In FEA, unknown quantities include nodal displace-
ments (ui) at each node in the mesh, as well as strains
(ϵij) and stresses (σij) at each integration point or
node. For a linear elastic material in 3D, the stiffness
matrix can be expressed using Lame’s constants, λ
and G , derived from Young’s modulus and Poisson’s
ratio.
λ =
Eν
(1 + ν)(1 − 2ν)
, G =
E
2(1 + ν)
(2)
Equation (3) presents stress-strain relationship in
matrix form.





σxx
σyy
σzz
σxy
σyz
σzx





=





λ + 2G λ λ 0 0 0
λ λ + 2G λ 0 0 0
λ λ λ + 2G 0 0 0
0 0 0 G 0 0
0 0 0 0 G 0
0 0 0 0 0 G










ϵxx
ϵyy
ϵzz
ϵxy
ϵyz
ϵzx





(3)
By inputting the known material properties and
boundary conditions into the FEA software, the un-
knowns (displacements, strains, and stresses) can be
determined. This process ensures accurate prediction
of structural behaviour under applied loads, facilitating
the design and assessment of structural integrity.
A review of published research reveals the prevalent
use of fixed boundary conditions (BC) in the static
structural analysis of members isolated from the global
structure [2]. While commonly employed, it is acknowl-
edged that this boundary condition represents a con-
servative approximation, which overestimates the max-
imum stress on the structural member, consequently
leading to an underestimation of the Factor of Safety
(FOS) [3].
The use of fixed support boundary conditions in
the analysis of statically indeterminate structures, such
as aircraft wings, presents notable limitations primar-
ily due to the assumptions that fixed supports in-
troduce, which may not accurately reflect real-world
conditions [4]. Fixed supports assume no movement or
rotation at the support points, which is often unrealis-
tic in practical scenarios. Aircraft wings experience var-
ious forces and moments that cause deformations, sig-
nificantly influencing overall structural behaviour [5].
Additionally, joints and connections in an aircraft are
not perfectly rigid; they possess some degree of flexi-
bility which must be considered for a more accurate
structural analysis.
Fixed supports can misrepresent actual load paths
and stress distributions within the structure. Aircraft
wings are engineered to distribute loads efficiently, but
fixed supports can alter these distributions, leading
to inaccurate analyses [6]. This can result in artificial
stress concentrations that do not exist in the struc-
ture, potentially leading to erroneous assessments of
structural integrity and fatigue life.
Moreover, fixed supports simplify the boundary
conditions to a degree that may not accurately capture
material non-linearities, such as plastic deformation
and creep [7]. Aircraft wings frequently operate under
conditions where these material non-linearities are sig-
nificant, necessitating boundary conditions that can
account for such effects. Additionally, large deforma-
tions and geometric non-linearities in aircraft wings
require boundary conditions that can adapt to chang-
ing configurations, a capability that fixed supports
cannot provide.
Lastly, results from analyses using fixed supports
may not correlate well with experimental data or in-
flight measurements. To ensure accurate and reliable
analysis, engineers often resort to more realistic bound-
ary conditions that simulate the interaction between
different parts of the structure, and flexible supports
that incorporate the elasticity of attachments and con-
nections. Hybrid models, combining various bound-
ary conditions, are also employed to better capture
the complex interactions within the structure. These
advanced boundary conditions facilitate more accu-
rate predictions of structural behaviour under diverse
loading conditions, leading to safer and more efficient
aircraft designs.
The wing of an aircraft is classified as a statically
indeterminate structure [8]. Such structures feature
kinematic redundancy, wherein the constraints exceed
the minimum necessary to prevent rigid body motion

92 INGENIUS N.◦
32, july-december of 2024
under applied loads. In statically indeterminate struc-
tures, the values of reaction forces and moments at
supports are influenced by the stiffness characteris-
tics of the structure [9]. Consequently, the stiffness of
the wing plays a crucial role in determining the load
distribution on the tulips of the wing station [10].
Rather than imposing a fixed boundary condition
on a local model isolated from the global model, an
alternative approach involves assigning nodal displace-
ments derived from the solution of the global Finite
Element (FE) model [11]. An FE analysis of the iso-
lated structural member, incorporating these nodal
displacements and the applied load, is conducted to
obtain accurate results. This method requires solu-
tions for both the global and local models for each
load case [12].
A third technique involves isolating the local model
from the global model using translational and rota-
tional springs. The stiffness of these springs depends
on the deformation field of the global model under the
applied load [13]. Subsequently, a refined local model
is analysed using these springs for each load case. Im-
plementing these springs in ANSYS is accomplished
by applying elastic support boundary conditions, with
stiffness derived from analysing the global wing model
under design load [14].
This examination focuses on a contemporary jet
fighter aircraft.
Figure 1 depicts the wing of an aircraft, including
four spars: the Front Wall Spar, Front Spar, Main Spar,
and Rear Spar [15]. These spars constitute a cohesive
framework intricately interconnected through a system
of 12 ribs.
Figure 1. Internal Structure of Aircraft Wing [15]
This study focuses on outboard wing station 2/6,
located on Wing Rib 7, specifically designated for carry-
ing external stores. This station comprises two integral
structural components: the Front Tulip (FT) and the
Rear Tulip (RT). Considering the limitations of fixed
boundary conditions, this study enhances the analysis
fidelity by incorporating wing stiffness. The primary
aim is to ascertain the maximum load-carrying capac-
ity of wing station 2/6, employing accurate boundary
conditions through the sub-modelling technique [16].
This method aims to provide a more accurate por-
trayal of structural behaviour, enabling precise evalua-
tion of stress levels and FOS for the wing station. In-
corporating wing stiffness enhances reliability of struc-
tural analysis and provides nuanced insights into wing
performance under diverse conditions. Sub-modelling
techniques account for the influence of wing stiffness,
resulting in improved accuracy and understanding of
structural behaviour. Ultimately, integrating wing stiff-
ness enhances structural analysis reliability, offering
valuable insights into wing performance across various
scenarios.
2. Materials and Methods
The methodology involves extracting the front and rear
tulips from the global wing model and introducing wing
stiffness via elastic boundary conditions derived from
FE analysis under the design load [17]. Critical loads
are applied to each wing tulip, and static structural
analysis is conducted in ANSYS Workbench version
14.5 to generate deformation and stress field. Utilizing
the Factor of Safety (FOS) based on yield strength,
the study determines the maximum load-carrying ca-
pacity of the wing station. Prestressed modal and
buckling analyses [18] are performed to assess the
stress-stiffening effect under the maximum design load.
The real potential of this study lies in the design op-
timization, which is implemented through parametric
alterations of the bolt holes of the wing tulip. This
process enhances the load-carrying capacity of the
wing station, facilitating a comprehensive evaluation
of structural performance and enhancing the overall
capabilities of the fighter aircraft [19]. While this study
provides a comprehensive understanding of the wing
station’s behaviour under static loads, it does not ac-
count for cyclic loading conditions. PSD analysis for
cyclic loading will be addressed in subsequent studies.
3. Results And Discussion
3.1. Boundary Conditions for Tulips
The FE model of the wing, constructed using line
and shell elements, is illustrated in Figure 2. Analy-
sis of this wing model under design load generates a
displacement field depicted in Figure 3. The result-
ing displacement field under applied loads provides

Approach 93
stiffness values for the elastic support imposed as a
boundary condition for the analysis of the Front and
Rear Tulips.
Figure 2. FE Model of the Wing [9]
Figure 3. Deformation Field of the Wing
The stiffness values for the respective elastic sup-
ports, obtained through ANSYS Workbench version
14.5, are presented. These stiffness values are utilized
in the analysis of isolated wing tulips.
Loads applied to the wing are transferred to the
fuselage, causing deformation and motion at the air-
craft’s center of gravity. To eliminate rigid body motion
in the analysis, it is necessary to constrain the air-
craft’s centreline. In the current study, the wing model
of the aircraft is constrained to six degrees of freedom
(6 DOF) at the aircraft’s centreline. This constraint
prevents undesired rigid body motions, ensuring an
accurate load transfer and structural behaviour sim-
ulation. By applying these constraints, the analysis
provides stable and realistic boundary conditions for
the Finite Element Analysis (FEA).
3.2. FE Models of Tulips
CAD models of the front and rear tulips for wing sta-
tion 2/6, which have been developed in the ANSYS
Design Module®, are illustrated in Figure 4 and Figure
5, respectively. These CAD models serve as templates
for developing FE models in ANSYS Workbench®.
Material properties assigned to the wing tulips are
detailed in the aerodynamic analysis of aircraft with
external stores within the carriage envelop of the air-
craft, providing provides critical load cases for wing
tulips [1]. Table 3 and Table 4 comprehensively outline
the load cases exerted on the Front Tulip (FT) and
Rear Tulip (RT) during the carriage envelop [1]. These
forces and bending moments are applied to both the
front and rear tulips of station 2/6.
Table 1. Elastic Boundary Condition for Tulips [9]
Tulip Linear Stiffness Rotational Stiffness
Front Tulip 242 kN/m 11173 Nm/rad
Rear Tulip 99 kN/m 50825 Nm/rad
Figure 4. Solid Model of the Front Tulip (FT) [9]
Figure 5. Solid Model of the Rear Tulip
Table 2. Material Properties of Tulips
Component Material
σ y E Poison Density
(MPa) (GPa) Ratio ν (g/cm3
)
Front Tulip (FT) 30CrMnSi 835 196 0.3 7.75
Rear Tulip (RT) 7050- 427 70 0.33 2.82

94 INGENIUS N.◦
Table 3. Loads Cases (LC) for the Front Tulip (FT) (force in kN and moments in kN.m) [1]
LC NZ FX FY FZ MX MY MZ
1 5 1.2 –11 –33 0 0 1
2 5 –20 –4 1 2 –78 –3
3 4.5 3.8 –12 –29 –1 40 2
4 4.5 28 4 –37 1 35 1
5 2 –14.8 –9 –11 2 –82 –2
6 2 16.8 –5 –20 –1 –49 1
7 4.5 2.96 –10 –30 0 21 1
8 4.5 30 10 –37 1 37 1
9 2.74 –10 –5 –17 2 –121 –3
10 2.74 14 3 –24 0 11 1
11 2 –16 –6 –10 2 –112 –3
12 2 11 –6 –5 0 –31 1
13 –1 1.4 2 6 0 31 1
Table 4. Load Cases (LC) for the Rear Tulip (RT) (force in kN and moments in kN.m) [1]
LC NZ FX FY FZ MX MY MZ
14 1 4 2 0 –1 –2 24
15 5 6 7 0 –2 –8 –9
16 5 2 6 2 –3 –7 13
17 2 1 3 1 –1 –4 –13
18 5 6 7 0 –2 –8 –10
19 1 –1 1 1 0 –1 2
20 4.5 –4 7 2 0 –6 –28
21 4.5 -3 3 11 0 0 24
22 2.17 15 6 -5 1 -5 6
23 2.17 -40 6 3 0 0 73
3.3. Analysis of the Front Tulip (FT)
The model has been free-meshed using Tet6 elements,
which are tetrahedral-shaped elements with three
nodes and a quadratic shape function. To ensure ac-
curacy, the mesh is refined at stress hot spots located
at bolt holes. As illustrated in Figure 6, a mesh inde-
pendence study establishes that the solution becomes
independent of mesh refinement at 70,000 elements.
Figure 7 displays the meshed model of the Front Tulip
(FT), while Figure 8 illustrates the applied boundary
conditions and loads on the FT.
Figure 6. Grid Independence of the FT
Figure 7. Free Mesh of the FT [9]
Figure 8. Loads and Boundary Conditions on the FT

Approach 95
For each load case, deformation and stress plots are
generated in ANSYS. The comparison of maximum
equivalent (von Mises) stress for each load case on the
Front Tulip (FT) is illustrated in Figure 9. Load Case
No. 4 is identified as the critical load case for the FT,
with a stress value of 674 MPa. The deformation field
of the Front Tulip under critical Load Case No 4 is
depicted in Figure 10. A maximum deformation of 0.13
mm is observed on the flange of the FT.
Figure 9. Max Stress for the FT under all LCs
Figure 10. Deformation of the FT under LC No 4
Further insight into the structural response, namely
the resultant stress field and Factor of Safety (FOS),
is provided in Figure 11 and Figure 12, respectively.
The FOS of the Front Tulip (FT) is 1.23 under crit-
ical Load Case No. 4, indicating that the FT is safe
within the carriage envelop. These analyses contribute
to a comprehensive understanding of the structural
behaviour, assessing safety margins and identifying
potential areas for design optimization.
Figure 11. Equivalent Stress of the FT under LC No 4
Figure 12. FOS of the FT under LC No 4
3.4. Analysis of the Rear Tulip (RT)
The free meshing of the rear tulip model has been
conducted using Tet6 elements, which are tetrahedral-
shaped elements with three nodes and a quadratic
shape function. Mesh refinement at bolt holes is im-
plemented to capture the large stress gradient at these
hot spots. A mesh independence study, as illustrated
Figure 13, demonstrated that the solution became
independent of mesh refinement at 130,000elements.
Figure 14 illustrates the meshed model of the Rear
Tulip (RT). Figure 15 illustrates the boundary con-
ditions and applied loads, represented as forces and
moments.
Figure 13. Mesh Independence for the RT
Figure 14. Free Mesh for the RT
Figure 15. Boundary Condition and Loads for the RT

96 INGENIUS N.◦
Through Finite Element (FE) analysis, deforma-
tion and stress for each load case were determined. The
comparison of maximum equivalent (von Mises) stress
for each load case on the Rear Tulip (RT) is presented
in Figure 16. The critical load case for RT is identified
as Load Case No 21, exhibiting a stress value of 323
MPa. Figure 17 illustrates the deformation field of
the Rear Tulip under Load Case No. 21. A maximum
deformation of 0.83 mm is observed under this critical
LC.
Figure 16. Max Stress for all LCs on the RT
Figure 17. Deformation of RT under LC No 21
Additional insights into resultant stress field and
Factor of Safety (FOS) under this specific load case is
provided in Figure 18 and Figure 19. FOS of RT is 1.3
under the critical LC NO 21 which indicates that RT is
safe within the carriage envelop. These comprehensive
analyses contribute to a detailed understanding of the
structural behaviour, aiding in assessment of safety
margins and potential areas for design optimization of
Rear Tulip.
Figure 18. Equivalent Stress of the RT under LC No 21
Figure 19. FOS of the RT for under LC No 21
3.5. Modal and Prestressed Modal Analysis
Modal analysis of the Front and Rear Tulips of the
wing station has been conducted to explore the dy-
namic characteristics of free vibrations without exter-
nal forces [20]. This analysis used free mesh models of
the Front and Rear Tulips within the ANSYS Modal
Module. The fundamental mode shapes for the Front
and Rear Tulips are depicted in Figure 20 and Figure
21, respectively. The fundamental mode frequencies
for the Front Tulip (FT) and Rear Tulip (RT) are 286
Hz and 282 Hz, respectively.
Figure 20. Fundamental Mode Shape for Free Mesh
Figure 21. Fundamental Mode Shape of the RT
Additionally, a prestressed modal analysis has been
conducted to assess stress-stiffening effects. A compar-
ison between free and prestressed modal frequencies
for the Front and Rear Tulips is presented in Figure
22 and Figure 23, respectively. The prestressed modal
analysis reveals a minimal decrease in modal frequen-
cies for the Front Tulip (FT). For the Rear Tulip (RT),
there is no decrease in modal frequency under applied

Approach 97
stress. Therefore, the stress-stiffening effect for the FT
and RT Tulips is insignificant.
Figure 22. Free and Prestressed Modal Analysis of the FT
Figure 23. Free and Prestressed Modal Analysis of RT
A comparative analysis offers insights into how
prestressed conditions affect the modal behaviour of
tulips, shedding light on the structural response under
the influence of pre-existing stresses. These findings
enhance the comprehensive understanding of the dy-
namic characteristics of the Front and Rear Tulips.
3.6. Buckling Analysis
Buckling analyses of the Front and Rear Tulips have
been conducted to ascertain buckling loads and cor-
responding buckling mode shapes [21]. The results of
these analyses are depicted in Figure 24 and Figure
25, showcasing the first buckling mode for the Front
and Rear Tulips, respectively, under their critical load
cases.
Figure 24. 1st Buckling Mode of the FT
Figure 25. 1st Buckling Mode of RT
The buckling load multipliers for the front and rear
tulips are determined to be 95 and 13, respectively,
under critical load cases. These high load multipliers
suggest buckling is not a likely failure mode for the
wing tulips. The mode shapes provide crucial insights
into the structural stability of the tulips under specific
loading conditions, enhancing the identification of po-
tential failure modes and the determination of safety
margins for the wing station components.
3.7. Optimization
The current radio for all bolt holes of the tulips are 4
mm. This study reveals that the maximum stress under
a critical load case occurs at the bolt holes. To conduct
a stress sensitivity analysis, the diameter of the bolt
holes varies from 6 to 10 mm using the ANSYS Opti-
mization Module [22]. Figure 26 and Figure 27 display
the stress response surfaces as a function of bolt-hole
radii for the Front Tulip and Rear Tulip, respectively.
These surfaces visually demonstrate how changes in
bolt-hole radii influence the tulips’ maximum stress.
Figure 26 indicates that the radii of bolts on the
inboard side (P2) have no discernible impact on the
maximum stress value of the Front tulip (P3). Con-
versely, the radii of bolts on the outboard side (P1)
significantly influence the maximum stress value of
the Front tulip. Initially, increasing the radii of bolt
holes on the outboard side from 3 mm results in an
increase in the maximum stress value (P3) up to 3.5
mm; beyond this point, further increases lead to a
decrease in the maximum stress value.
Figure 27 demonstrates that the radii of bolt holes
on both the front (P1) and rear (P2) sides of the Rear
Tulip significantly impact the maximum stress value
(P3). Initially, as the values of P1 and P2 increase from
3 mm, the maximum stress value decreases, reaching
a minimum of 4.5 mm. However, further increases in
the radii of the bolt holes increase the maximum stress
value.
This sensitivity analysis reveals that the minimum
stress for the Front Tulip occurs with a bolt-hole radius
of 5 mm, while for the Rear Tulip, a radius of 4.5 mm
is optimal. These design parameters reduce the max-
imum stress to 627 MPa and 286 MPa for the Front

98 INGENIUS N.◦
and Rear Tulips, respectively. The larger bolt holes
contribute to an increased Factor of Safety (FOS) of
1.33. Consequently, the maximum load-carrying capac-
ity of the wing station increases from 653 kg to 706 kg
with this optimized design. This sensitivity analysis is
crucial for optimizing the design of bolted connections
in tulips, helping to identify the most suitable diameter
that minimizes stress concentrations and enhances the
overall structural performance of the Front and Rear
Tulips.
Figure 26. Response Surface for Max Stress FT
Figure 27. Response Surface for Max Stress RT
4. Conclusions
This study addresses a significant gap in the state-
of-the-art application of similar research problems by
focusing on the influence of stiffness characteristics on
the maximum load-carrying capacity of a fighter air-
craft’s wing. Although previous studies have explored
various factors affecting the structural integrity of air-
craft components, few have delved into the role of wing
stiffness and its direct impact on load-carrying capac-
ity. This research integrates wing stiffness into the
Finite Element (FE) model of isolated tulips, provid-
ing an analysis that accurately predicts the structural
integrity of the weapon station. Additionally, using
sub-modelling as a versatile and computationally effi-
cient technique introduces an innovative methodology,
bridging a gap in the existing literature by showcas-
ing its applicability to intricate structural components
with minimal computational expense.
Validation of the initial hypothesis through ob-
tained data underscores the significance of wing stiff-
ness in assessing the wing station’s maximum load-
carrying capacity. Overall, this research enhances the
understanding of structural analysis in aerospace engi-
neering by providing novel insights and methodologies
to address a critical gap in the field. The key findings
of this research are outlined as follows:
Front Tulip:
• Optimal bolt-hole radius: 5 mm
• Reduced maximum stress: 627 MPa
Rear Tulip:
• Optimal bolt-hole radius: 4.5 mm
• Reduced maximum stress: 286 MPa
Factor of Safety (FOS):
• Increased to 1.33 with larger bolt holes
Maximum Load-Carrying Capacity:
• Increased from 653 kg to 706 kg with the opti-
mized design
Identifies critical design parameters for optimizing
bolted connections in tulips, helping to determine the
most suitable diameter that minimizes stress concentra-
tions and enhances the overall structural performance
of both the Front and Rear Tulips.
A notable limitation of this research is the exclu-
sion of fasteners from the analysis, predicated on the
assumption of perfect load transfer between the struc-
tural elements of the wing and the wing tulips. Conse-
quently, this study does not account for the potential
failure modes associated with fasteners.
Future research endeavours should explore the
following aspects to enhance the comprehensiveness of
structural analyses. Addressing these aspects would
significantly contribute to the structural assessments
of large assemblies.
Non-linear Effects:
• Implications of non-linear effects on structural
integrity.
Mesh Patterns:
• Effects of regular mesh patterns on simulation
results.
Cyclic Loading / Power Spectral Density
(PSD) Analysis:
• Cyclic loading and PSD analysis to evaluate long-
term structural performance.

Approach 99
Author Contributions
The entirety of this research, including literature re-
view, methodology, results and findings represents
work of Author.
Acknowledgments
The author acknowledges the support of his depart-
ment at Air University for providing all the necessary
resources for this publication.
Conflict of Interest
The author declared no potential conflicts of interest
concerning research, authorship, and publication of
this article.
Funding
The author received no financial support for research,
authorship, and publication of this article.
Data Availability Statements
The current study is available from the corresponding
author upon reasonable request.
References
[1] K. Sinha, T. Klimmek, M. Schulze, and V. Han-
dojo, “Loads analysis and structural optimization
of a high aspect ratio, composite wing aircraft,”
CEAS Aeronautical Journal, vol. 12, no. 2,
pp. 233–243, Apr 2021. [Online]. Available:
https://doi.org/10.1007/s13272-021-00494-x
[2] B. D. Upadhyay, S. S. Sonigra, and S. D.
Daxini, “Numerical analysis perspective in
structural shape optimization: A review post
2000,” Advances in Engineering Software, vol.
155, p. 102992, 2021. [Online]. Available: https:
//doi.org/10.1016/j.advengsoft.2021.102992
[3] N. Zimmermann and P. H. Wang, “A review of
failure modes and fracture analysis of aircraft com-
posite materials,” Engineering Failure Analysis,
vol. 115, p. 104692, 2020. [Online]. Available: https:
//doi.org/10.1016/j.engfailanal.2020.104692
[4] R. L. Muhanna and S. Shahi, Uncertainty in
Boundary Conditions—An Interval Finite Ele-
ment Approach. Cham: Springer International
Publishing, 2020, pp. 157–167. [Online]. Available:
https://doi.org/10.1007/978-3-030-40814-5_20
[5] T. Martins, V. Infante, L. Sousa, A. Fon-
seca, P. Antunes, A. Moura, and B. Serrano,
“Numerical and experimental study of aircraft
structural health,” International Journal of Fa-
tigue, vol. 132, p. 105348, 2020. [Online]. Available:
https://doi.org/10.1016/j.ijfatigue.2019.105348
[6] J. Lim, C. You, and I. Dayyani, “Multi-objective
topology optimization and structural analysis of
periodic spaceframe structures,” Materials & De-
sign, vol. 190, p. 108552, 2020. [Online]. Available:
https://doi.org/10.1016/j.matdes.2020.108552
[7] C. Touzé, A. Vizzaccaro, and O. Thomas,
“Model order reduction methods for geometrically
nonlinear structures: a review of nonlinear
techniques,” Nonlinear Dynamics, vol. 105, no. 2,
pp. 1141–1190, Jul 2021. [Online]. Available:
https://doi.org/10.1007/s11071-021-06693-9
[8] C. You, M. Yasaee, S. He, D. Yang, Y. Xu,
I. Dayyani, H. Ghasemnejad, S. Guo, P. Webb,
J. Jennings, and G. Federico, “Identification of the
key design inputs for the FEM-based preliminary
sizing and mass estimation of a civil aircraft wing
box structure,” Aerospace Science and Technology,
vol. 121, p. 107284, 2022. [Online]. Available:
https://doi.org/10.1016/j.ast.2021.107284
[9] A. Haider Bhutta, “Appropriate boundary con-
dition for finite element analysis of structural
members isolated from global model,” NED
University Journal of Research, vol. 18, no. 3, pp.
61–75, 2021. [Online]. Available: https://doi.org/
10.35453/NEDJR-STMECH-2021-0001
[10] E. Narvydas, N. Puodziuniene, and T. A. Khan,
“Application of finite element sub-modeling
techniques in structural mechanics,” Mechanika,
vol. 27, no. 6, pp. 459–464, 2021. [Online]. Avail-
able: https://doi.org/10.5755/j02.mech.25962
[11] J. Jang and S. Ahn, “Fe modeling method-
ology for load analysis and preliminary
sizing of aircraft wing structure,” Interna-
tional Journal of Aviation, Aeronautics, and
Aerospace, vol. 6, no. 2, 2019. [Online]. Available:
https://doi.org/10.15394/ijaaa.2019.1301
[12] A. Mishra, S. Pal, G. Singh Malhi, and P. Singh,
“Structural analysis of UAV airframe by us-
ing FEM techniques: A review,” International
Journal of Advanced Science and Technology,
vol. 29, pp. 195–204, 06 2020. [Online]. Available:
https://is.gd/4NRfx9
[13] S. Henclik and A. Maurin, “Determination of the
stiffness matrix of flat springs for modeling of
the boundary condition at a pipeline support,”
Mechanical Systems and Signal Processing, vol.

100 INGENIUS N.◦
123, pp. 102–116, 2019. [Online]. Available:
https://doi.org/10.1016/j.ymssp.2018.12.047
[14] M. d. C. Alves, F. N. Corrêa, J. R. M. de Sousa,
and B. P. Jacob, “A coupled, global/local finite
element methodology to evaluate the fatigue life
of flexible risers attached to floating platforms
for deepwater offshore oil production,” Mathe-
matics, vol. 12, no. 8, 2024. [Online]. Available:
https://doi.org/10.3390/math12081231
[15] V. Karnozov, “China’s fighter aircraft detailed,”
Defence Review Asia, vol. 13, no. 1, pp. 42–47,
2019. [Online]. Available: https://is.gd/dM2DHD
[16] A. G. Manca and C. M. Pappalardo, “Topology
optimization procedure of aircraft mechanical
components based on computer-aided design,
multibody dynamics, and finite element anal-
ysis,” in Advances in Design, Simulation and
Manufacturing III, V. Ivanov, I. Pavlenko,
O. Liaposhchenko, J. Machado, and M. Edl,
Eds. Cham: Springer International Publish-
ing, 2020, pp. 159–168. [Online]. Available:
[17] A. Aabid, M. A. M. B. M. Zakuan, S. A.
Khan, and Y. E. Ibrahim, “Structural anal-
ysis of three-dimensional wings using finite
element method,” Aerospace Systems, vol. 5,
no. 1, pp. 47–63, Mar 2022. [Online]. Available:
https://doi.org/10.1007/s42401-021-00114-w
[18] P. Wang, Y. Chen, R. Pei, C. Lian, K. Zhang,
and Y. Zhou, “Buckling and post-buckling
analysis of composite wing box under loads with
torsion-bending coupling,” Thin-Walled Struc-
tures, vol. 193, p. 111266, 2023. [Online]. Available:
https://doi.org/10.1016/j.tws.2023.111266
[19] N. Yang, “Methodology of aircraft structural de-
sign optimisation,” International Journal of Com-
puter Applications in Technology (IJCAT), vol. 70,
no. 3, pp. 145–154, 2022. [Online]. Available:
https://dx.doi.org/10.1504/IJCAT.2022.130874
[20] A. Basutkar, K. Baruah, and S. K. Kudari,
“Frequency analysis of aircraft wing using FEM,”
in Recent Trends in Mechanical Engineering, G. S.
V. L. Narasimham, A. V. Babu, S. S. Reddy,
and R. Dhanasekaran, Eds. Singapore: Springer
Singapore, 2020, pp. 527–533. [Online]. Available:
[21] B. Ravi Kumar, “Investigation on buck-
ling response of the aircraft’s wing us-
ing finite-element method,” Australian Jour-
nal of Mechanical Engineering, vol. 18, no.
sup1, pp. S122–S131, 2020. [Online]. Available:
https://doi.org/10.2514/1.C034818
[22] S. De, M. Jrad, and R. K. Kapania, “Structural
optimization of internal structure of aircraft
wings with curvilinear spars and ribs,” Journal of
Aircraft, vol. 56, no. 2, pp. 707–718, 2019. [Online].
Available: https://doi.org/10.2514/1.C034818

Optimizing Structural Integrity of Fighter Aircraft Wing Stations a Finite Element Analysis Approach.pdf

More Related Content

Similar to Optimizing Structural Integrity of Fighter Aircraft Wing Stations a Finite Element Analysis Approach.pdf (20)

More from Aun Haider (14)

Recently uploaded (20)

Optimizing Structural Integrity of Fighter Aircraft Wing Stations a Finite Element Analysis Approach.pdf