## 3 Finite Element Simulation  
### Finite Element Model  
A finite element model of a simple VBI system has been constructed to validate the proposed method. The VBI system adheres to the configuration established in a prior study [42]. The bridge is a simply supported beam with a span of 25 m, and its physical parameters are illustrated in Table 1. A simplified quarter-car model is employed to simulate the vehicle, encompassing a sprung mass, a suspension spring, and a wheel interface in contact with the beam's surface. The comprehensive parameters of the vehicle are enumerated in Table 2.  
\begin{table}
\begin{tabular}{c c} \hline \hline Sprung mass (kg) & 600 \\ \hline Spring stiffness (N/m) & 500,000 \\ \hline Bouncing frequency (Hz) & 4.60 \\ \hline \hline \end{tabular}
\end{table}
Table 1: Physical parameters of the simply supported beam [42].  
A finite element model, depicted in Figure 4a, was constructed utilizing the commercial software ABAQUS 2020 [47]. Solid elements of type C3 DRR were utilized to model both the beam and the sprung mass, with each element measuring 0.1 m \(\times\) 0.1 m \(\times\) 0.1 m. Our preliminary analysis confirmed that the mesh density exerts a negligible impact on the simulation's accuracy. The boundary conditions (Figure 4b) for the simply supported beam were implemented by restraining the appropriate degrees of freedom at the beam's edge nodes. For the left edge nodes, which are part of a simply supported beam, movements along the X, Y, and Z axes, as well as rotations about the Y and Z axes, were constrained. Similarly, for the right edge nodes, constraints were applied to motions along the X and Y axes and rotations about the Y and Z axes. The spring element was used to model the connection between the sprung mass and the wheel. The wheel, depicted as a cylindrical solid element, engaged with the beam surface using the penalty method. It is important to note that during the simulation, the wheel's rotation was restricted. The friction coefficient between the wheel and the bridge surface was set to zero to simplify the interaction. Consistent with the theoretical derivation and considering its minimal impact on bridge dynamics, road roughness was excluded from the analysis. The vehicle's movement across the bridge was assumed to be at uniform speeds. The simulation was divided into two computational stages: a static analysis to account for gravitational forces on the entire VBI system, followed by a dynamic analysis to assess the system's responses to the moving vehicle. The dynamic analysis was conducted using the Hilber-Hughes-Taylor (HHT) algorithm with a time step of 0.01 s. The simulation approach we utilized is grounded in the method initially proposed and substantiated in the existing body of research [48]. For an exhaustive examination of the simulation methodology, one can refer to the detailed account provided in the aforementioned study [48].  
\begin{table}
\begin{tabular}{c c} \hline Mass per meter (kg/m) & 4800 \\ \hline EI (N/m\({}^{2}\)) & \(3.33\times 10^{9}\) \\ \hline First bending frequency (Hz) & 2.08 \\ \hline Second bending frequency (Hz) & 8.33 \\ \hline Length (m) & 25 \\ \hline \end{tabular}
\end{table}
Table 2: Parameters of the vehicle model [42].  
Figure 4: Finite element model of the VBI system [41].