## 3 FEM Case Analysis  
The reduced size of the interstage structure of a certain type of rocket body is used to develop a fine finite-element analysis model in this paper (Figure 5). The genuine interstage connection structure is complex, with a typical thin-walled cylindrical shell structure with bolted connections as its major bearing structure. After maintaining the characteristics of the primary load-bearing structure, the structure is adequately simplified, and the influence of the thread is ignored to enable simulation analysis and laboratory tests. Two aviation aluminum alloy shell structures with the same size and material properties were selected, and connected by six bolts at the flange surface, with a length of 340 mm, a wall thickness of 4 mm, a diameter of 295 mm, according to the parameter background of the relevant rocket body's interstage section. The bolt hole diameter on the flange face is 8.4 mm, and continuous flange thickness is 10 mm. The elastic modulus of the shell structure is 70 GPa, with Poisson's ratio of 0.3 and a density of 2700 kg/m\({}^{3}\). High-strength steel bolts have a 210 GPa elastic modulus, a Poisson's ratio of 0.3, a density of 7850 kg/m\({}^{3}\), a head diameter of 12 mm, and a shaft diameter of 5.7 mm. ABAQUS software was used to create the finite-element model. The bolt and nut can be merged due to the thread simplicity, and the preload is applied in the form of bolt load. This simplified modeling method, which simplifies the bolt into an I-shaped model in Figure 5, has been applied in previous research [14], and its effectiveness has been proved. However, although the contact relationship is considered in [PERSON]'s research [14], the influence of the bolt preload is not considered. This paper further considers the preload in the model. In the ABAQUS Load Manager, the preload is applied as a bolt load, which simulates bolt preload using face pressure. The C3D8R hexahedral mesh, which is separated in the axial direction, is used to assure calculation efficiency and precision. The contact surfaces in the model include the contact between the flange surfaces and the contact between the bolt and the flange surface in Figure 6. All the contact is set to be surface contact with a contact friction coefficient of 0.2 and the friction formula's penalty function applied. All contact surfaces in the model are set to hard contact in ABAQUS, which means that the augmented Lagrangian method and the penalty approach are used to solve the normal and tangentialcontact problems according to the research by [PERSON] [27]. The bottom of the structure is fastened. The following text includes static and dynamic calculations (Load as Figure 7), in which the Static General calculation step in ABAQUS is used for the static calculation, and the Dynamic Implicit calculation step is used for the dynamic calculation. The acceleration response is obtained by applying a continuous impulse load to the top of the structure, performing dynamic computations, and obtaining the acceleration response. The sampling frequency is set to 5000 Hz. The impulse width is 0.2 ms, and the load amplitude is 1000 N. The number of impulses for the same equipment and bolt preload is 20. Figure 5: Bolted flange of the rocket connection structure. Figure 6: Contact surface of the connection structure. To verify the mesh sensitivity of the finite element model, the meshes of different sizes were applied to the modeling of bolts and flanges. In addition, the calculation was carried out under the same static and dynamic conditions. As shown in Figure 8, the mesh size of the bolt has little effect on the static calculation results, but the mesh size of the flange has a greater effect. When the mesh size of the flange is 10, the calculation result is obviously distorted, and the deviation is very large. When the flange mesh sizes are three, five, and six, the static calculation results are very close, with almost no difference.