Structural statics analysis was a fundamental method in engineering mechanics used to analyze the stress, strain, and deformation of structures under static loads. The analysis results played a critical role in ensuring engineering structures’ safety, reliability, and stability (Zhang et al., 2021). When conducting statics analysis, the equilibrium equations for solving internal forces and external loads were: K u = F (1)

Where K denotes the structural stiffness matrix, u represents the displacement vector, and F signifies the nodal load vector.

After solving the equilibrium equations to obtain the nodal displacements of the structure, these displacements were substituted into the following equation to calculate the elemental nodal stresses within the structure: σ = D B δ e (2)

Where D was the structural stiffness matrix, B was the displacement vector, and δ e denotes the nodal displacement.

For the calculation of equivalent stress, the material of the frame component in this simulation was titanium alloy (Ti-6Al-4V), which was a standard material in the aerospace field. According to material mechanics, the failure mode of this material was yield failure. Therefore, the von Mises equivalent stress was calculated based on the fourth strength theory. Then, the von Mises equivalent stress was compared with the allowable stress of the material. It was required that the von Mises equivalent stress had to be less than the allowable stress of the material to prevent failure. The formula for calculating the von Mises equivalent stress was as follows: σ s = 1 2 σ 1 − σ 2 2 + σ 2 − σ 3 2 + σ 3 − σ 1 2 ≤ σ (3)

Where σ s denotes the equivalent stress; σ represents the allowable stress of the material; σ 1 , σ 2 , and σ 3 were the first, second, and third principal stresses, respectively.

This study used the Altair Inspire software to build a simulation model. As shown in Figure 1a, a lens frame was used to fix the lens of a spectacle. Overall, the model was a symmetric solid structure with a total mass of 0.062 Kg and an overall size of ∅ 154*2 mm. The fan-shaped lenses were clamped in the groove of the frame, and the thickness of the groove surface in contact with the lens was 0.5 mm. Small lenses (a total of 12 pieces) were installed on the outer layer of the frame, large lenses (a total of six pieces) were installed in the middle layer, and the innermost layer was a solid structure. The thickness of each lens was 1.5 mm, and they were distributed at equal intervals along the circumference. At each lens installation position on the lens frame, a fillet of ∅ 2 was designed at the corner to facilitate the lens installation and protect the lens corners.

This lens frame was installed in a sleeve device. There was an interference fit between the sleeve and the shaft hole of the lens frame, and other parts fixed both end-faces. Therefore, in the software, a fixed-constraint boundary condition was set for the outermost circumference of the part. Spacecraft need to withstand complex working conditions such as impact loads during the launch phase, dynamic loads generated by micrometeoroid impacts and attitude adjustments during in-orbit operation. During the simulation. Two significant types of load cases were set in the simulation. The first type of load case was to simulate the situation where an object hit the part, generating an impact force that could damage the part. In this case, there were three situations: (1) The load was applied at the center of the part (Position 1); (2) The load was applied on the large lens, and then transferred to the frame through the large lens (Position 2); (3) The load was applied on the small lens, and then transferred to the frame through the small lens (Position 3). The load magnitudes were 200 N, 400 N, 600 N, and 800 N, respectively, which covered the typical extreme values of mechanical loads that the spacecraft might encounter during takeoff and on-orbit operation. During the simulation, the lens was simplified as a rigid component, and the mechanical transmission relationship between the lens and the frame was simulated through the connector function in the software. When a load was applied to the lens, this setup could equivalently simulate the uniform pressure distribution generated by the lens on the groove of the frame, so as to simulate the extreme stress conditions borne by the frame. The other type of load case was to simulate the torque that might be generated during the installation process of the lens frame (Position T1). The torque magnitudes were 30 N m, 50 N m, and 100 N m, respectively, and they were applied to the solid disc at the center. The load application positions were shown in Figure 1b.

Regarding the definition of the material properties of the model, the titanium alloy (Ti-6Al-4V) material was selected from the material library of the Altair software. It was an α + β type titanium alloy, with titanium as the main component, containing about 6% aluminum, 4% vanadium, and a small amount of impurity elements. This material had high strength, good toughness, and fatigue-resistance performance. Its yield strength was as high as 823.371 MPa, and its elastic modulus was 116.522 GPa. Moreover, it had superior physical properties. Its density was about 4.5 g/cm³, which was much lower than that of traditional metal materials, and it was beneficial for reducing the weight of aerospace vehicles. It had a relatively high melting point (1,660°C–1,690°C). Its high-temperature resistance and low thermal conductivity could reduce the risk of heat transfer and thermal-stress deformation. The study used the yield strength of Ti-6Al-4V alloy as the failure criterion, focused on exploring the ultimate load-bearing behavior of the structure, and aimed to provide a reference structural specification and performance boundary for the safety design of similar lightweight telescope frames.

In this simulation, the average mesh size was set to 0.3 mm. The mesh was automatically generated by the Inspire software, and the total number of meshes was 2.927 million. The OptiStruct solver built into the software was used for the solution. It was a high-end solver integrating structural analysis and optimization design. Based on the Finite Element Method (FEM), it discretized the continuum into a finite number of elements to solve the mechanical behavior of complex engineering structures accurately. For this simulation, the static-simulation module of the OptiStruct solver was used. Taking the nodal displacements as the fundamental unknowns, by establishing the element stiffness matrix and the global stiffness matrix, the Newton-Raphson iterative algorithm was used to handle nonlinear problems. The stiffness matrix was continuously updated through iterations to approach the exact solution gradually.

The simulation results when the load was applied at the center of the part were shown in Figures 2, 3. As seen from the displacement nephogram (Figure 2), the maximum displacement occurred at the exact center of the part. Under an 800 N load, the displacement was approximately 1.796 mm, and the displacement magnitude decreased diffusely towards the periphery. Under 200 N, 400 N, and 600 N loads, the maximum displacement degrees were 0.4490 mm, 0.8981 mm, and 1.347 mm, respectively. Significant stress concentrations in the von Mises equivalent stress nephogram (Figure 3) were evident within the lens-protecting fillets at the connections with the middle disk beam and the outermost ring beam. The maximum von Mises equivalent stresses under each load were 228.6 MPa, 457.2 MPa, 685.8 MPa, and 914.4 MPa, respectively. As the load gradually increased, stress concentration first occurred at the connection of the middle disk beam, followed by the lens-protecting fillets at the connection of the outer ring beam. When the load reached approximately 700 N, the stress concentration level reached the critical failure load of the titanium alloy material. Therefore, during the design of this part, special attention should be paid to the stress state and deformation conditions at the corners of the beam connections. Increasing the radius of fillets appropriately can help mitigate this issue.

When the load was applied on the large lens, the deformation and stress conditions of the frame became severe (Figures 4, 5). Under an 800 N force, the maximum displacement reached 3.463 mm. Even under a low force of 200 N, the displacement was 0.8656 mm. This significant deformation may be caused by the thickness of the lens-fitting area of the part, which was only 0.5 mm, and it was simultaneously affected by the torque generated by the quasi-cantilever structure. The area with the maximum stress occurred at the connection of the outer ring beam, which was the connection end of the cantilever structure and had a relatively small cross-sectional area. The second highest stress area was at the connection of the central disk beam. However, as the load increased, obvious stress concentration gradually appeared at the middle ring’s connection, a phenomenon not observed in other load cases. Under a low load of 200 N, the maximum von Mises equivalent stress reached 640.3 MPa, and the yield strength of the material was reached at approximately 250 N. For every additional 200 N of load, the maximum von Mises equivalent stress caused by the structural deformation increased by about 640 MPa. However, when the load acted on the center of the small lens, this situation improved (Figures 6, 7). Both the displacement and von Mises equivalent stress were significantly reduced. From the displacement nephogram, it could be seen that the middle ring became the area with the maximum displacement. The displacements under each load were 0.2418 mm, 0.4837 mm, 0.7255 mm, and 0.9673 mm, respectively. As the load increased, the influence of the displacement change gradually affected the central position, while the impact on the outer ring changed little. This was because the fixed position of this part was the outer ring, and the central position was at the far end of the quasi-cantilever structure, making it more prone to displacement. Then, observing the von Mises equivalent stress nephogram (Figure 5), the stress concentration was located at the connection between the outer ring and the beam. Even under high loads, the connection between the middle ring and its connection beam was not significantly affected. The maximum von Mises equivalent stresses on the part were 375.2 MPa, 750.4 MPa, 1,126 MPa, and 1,501 MPa, respectively.

In summary, when this structure was subjected to vertical loads, the maximum load it could withstand was approximately 700 N. However, to ensure the structure’s safety, the load it endured during normal operation should not exceed 250 N. To improve the structure’s stability, it was necessary to further increase the fillet size at the beam connections and the cross-sectional area of the lens-protecting fillets.

The torsional load case was established to simulate the torque the part might experience during installation, aiming to evaluate the structural torsional resistance. As shown in Figure 8, under torsional loading, the overall displacement of the part remained extremely low. Although the central disk and rings were supported only by crossbeams, the maximum displacement reached just 0.2205 mm even under a high load of 100 N·m. Notably, the fillets designed at the crossbeam connections had a radius of only 1 mm, which inevitably caused significant stress concentration during torsion. As indicated by the von Mises equivalent stress nephogram (Figure 9), stress concentration first occurred at both ends of the middle long crossbeam. As the torque increased, the stress-concentrated region gradually expanded toward the crossbeam center, affecting its structural strength. Simulation results showed that when a torsional load of approximately 50 N·m was applied, the von Mises equivalent stress from stress concentration reached the yield stress threshold of the titanium alloy material.