## 5 Frequency Response Analysis Using TLE
### TLE Modeling  
The NASTRAN/FREQUENCY RESPONSE software was used to simulate the penetration response of the projectile-fuse system. The projectile body and fuse body are connected by threads. The vibration response of the fuse cannot be accurately predicted because of the uncertain factors at the threaded contact. The primary uncertainty in threaded connections arises from the contact stiffness and friction damping [30]. Because the commonly used dynamic analysis software cannot correctly deal with nonlinear factors, the TLE was used to characterize the contact stiffness between threaded contacts. In addition, the thread friction damping was described by setting a reasonable damping coefficient for the TLE. According to the height of the thread tooth, the thickness of the TLE was determined to be 2 mm. The length of the TLE was 33 mm, i.e., the threaded length. Figure 15 shows the FE model of the projectile-fuse system. The FE model was composed of three parts: the projectile body, fuse body, and TLE. All of the entities were modeled using eight-node hexahedral elements (CHEXA), and each node had six degrees of freedom. For the convenience of constraint treatment at the contact interface, the element sizes of the projectile body, fuse body, and TLE should be consistent at the thread contact interface. The projectile and fuse were characterized using a linear elastic model. The material parameters are listed in Table 8. The TLE was also characterized by a linear elastic material model, and Table 9 lists the material parameters. The contacts between the two pairs (TLE and projectile, TLE and fuse) were defined as 'tied' constraints. At the projectile nose, the numbers of circumferential and axial nodes were 120 and 44, respectively. To satisfy the quality requirements of the hexahedral mesh, the number of circumferential nodes at the tip of the projectile nose was generally reduced during mesh generation. Thus, we allocated the penetration excitation forces by combining the node position with the number of circumferential nodes. In the present simulation, \(F\) in Equation (12) refers to the experimental rigid-body deceleration. The magnitudes of each nodal force were obtained using Equation (12). The projectile had a free state without any boundary constraints. In addition, the damping was incorporated by the complex stiffness matrix \(K*\) domain with dissipation multipliers \(\alpha_{i}\) and \(\beta_{i}\) for the material and joint damping, respectively, and the associated element stiffness matrices. \[K*=K+j\sum_{i=1}^{n}\alpha_{i}K_{i}^{(Material)}+j\sum_{i=1}^{n}\beta_{i}K_{i}^{( Joint)}\,, \tag{13}\]  
where \(K\) is a real-value stiffness matrix, and \(n\) and \(m\) are the number of different materials and joints with different properties used in the model, respectively. Material damping is applied to the elements belonging to the components of the projectile-fuse system, and joint damping is realized by applying damping to the TLEs [13]. In the present calculation, the material damping \(\alpha\) is \(5\times 10^{-4}\), and the joint damping \(\beta\) is 0.03, determined through a trial-and-error method. The Lanczos algorithm for the modal superposition method was applied for analysis and solution. The number of desired roots was set to 100. To meet the 40 kHz output frequency range, the length and number of output frequency steps were 100 Hz and 400 respectively. One node at the middle partition (accelerometer position) of the fuse was selected as the frequency response point (Figure 15). Figure 16 shows a comparison of the nodal force distribution methods, including an equal distribution and the distribution according to Equation (12). The frequency response resonance peaks of the nodal force distribution using Equation (12) are concentrated in the frequency band of 30-40 kHz, while the resonance peaks of the equal distribution method are concentrated around the first-order frequency.