## 4 Finite Element Analysis  
### Accuracy of Formulas  
The verification of Equation (29) was mainly conducted through finite element simulations using software such as HyperWorks 2019, ANSA v24.0.0, ANSYS APDL, and ANSYS Workbench 2023R1. Numerical simulations in statics and harmonic response were performed to verify the calculated negative stiffness values and transmissibility derived from Equation (29). In the previous section on the derivation of the \(U_{a}\) term we showed that the superposition method produces errors for large deflection behavior and that there is no better solution for the time being because of the boundary condition problem, so finite element simulations will be used as a reference point here as a way to correct the \(U_{a}\) term. Figure 12: Finite element simulation of negative stiffness values at different displacements, with a LS \(E\) of 193 GPa, \(b\) of 80 mm, \(l_{0}\) of 80 mm, \(h\) of 0.1 mm, \(u_{x}\) of 0.1 mm, and \(N\) of 6. The finite element model is shown in Figure 13. The structure mainly consists of a crystal assembly, a basic frame, a peripheral frame, and LSs. The number of LSs is 6. One end of the LS is connected to the peripheral frame and the other end is connected to the basic frame through a slider. The key parameters of the LS are shown in Table 1. The compression of the compliant LSs is achieved by applying a displacement boundary to the slider, while the force transfer between the LSs and the slider contact pair is measured using a force response probe. The force transfer between the plate spring and the slider is equal to the \(F\) illustrated in Figure 7, and these data are measured in order to solve for the value of the \(U_{a}\) term in the finite element simulation in the next calculation. A total of two springs with a stiffness of 25 N/mm were used for the connection of the basic frame to the peripheral frame, with a total positive stiffness of 50 N/mm and a mass of 58.5 kg for the peripheral frame. The calculation method for negative stiffness values is as follows: In the Static Structural module, firstly, compression buckling of the LS is achieved through slider displacement. Secondly, the peripheral frame is driven to move along the y-axis using displacement boundary conditions, and the force reaction probe measures the force required for this displacement boundary condition. Finally, the actual stiffness value is obtained by dividing the force reaction of the peripheral frame by the displacement distance. The negative stiffness value is then derived by subtracting the positive stiffness value from the actual stiffness value. The role of the force reaction probe here is to measure the driving force \begin{table}
\begin{tabular}{c c c c} \hline \hline
**Parameter** & \multicolumn{2}{c}{**Value**} \\ \hline Length (mm) & 60 & 70 & 80 \\ Width (mm) & 60 & 70 & 80 \\ Thickness (mm) & 0.1 & 0.2 & 0.3 \\ Compression (mm) & 0.1 & 0.2 & 0.3 \\ Elastic Modulus (GPa) & & 193 & \\ Poisson’s Ratio & & 0.28 & \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Dimensions and material properties of LSs. Figure 13: Finite element model: **(a,b)** boundary conditions and layout; **(c)** distribution of positive stiffness helical springs; **(d)** force reaction measurement locations. required for the peripheral frame to move a specified distance along the y-axis. Using force to drive peripheral frame displacement can also calculate stiffness values, but it is less effective in terms of solution speed and convergence compared to using displacement boundary conditions. The simulation of transmissibility involves three modules: Static Structural, Modal, and Harmonic Response. The analysis process is as follows: First, compression buckling of the LS is completed in the Static Structural module. Second, the first six modal frequencies of the entire structure after buckled are computed. Third, 1 g acceleration excitation is applied to the base of the basic frame in the harmonic response.