## 1 Introduction
### Implementation Process of the Contact Constraint Method in ANSYS  
Vehicle-bridge coupling analysis falls within the scope of multi-degree-of-freedom dynamic analysis. The finite element method has been applied to the structural analysis of full-scale bridge engineering [39]. Some scholars have even employed a hybrid simulation method that combines the finite element method with experiments [40; 41]. In this study, the vehicle-bridge coupling vibration analysis method based on the contact constraint approach is implemented on the ANSYS R18.0, as shown in Figure 5. The steps are as follows:  
Step 1. Establish the bridge model based on the model data.  
Step 2. Determine the lane information, including lane positions, number, and direction, and create lanes at a certain distance from both ends of the bridge to ensure vehicles enter the bridge with stable vibration states.  
Step 3. Determine the vehicle information, including the number of vehicles, types, initial positions, and vehicle speeds. Establish a multi-rigid-body vehicle model at the initial position.  
Step 4. Input the three-dimensional pavement roughness sample into ANSYS, and couple the wheel bottom nodes with the wheel-bridge deck contact points using constraint equations, with the constant term of the constraint equation being the pavement roughness value.  
Step 5. Establish point-to-surface contact between the wheel-bridge contact points and the bridge deck, forming the vehicle-bridge coupling system.  
Step 6. Enter the static analysis module, apply gravitational acceleration, and bring the spring-damping system of the vehicle model into a balanced position.  
Step 7. Enter the transient dynamic analysis module and apply displacement in the driving direction to the vehicle model. The displacement within one time step is determined by the vehicle speed. The time step is automatically adjusted by ANSYS to optimize computational accuracy and efficiency. The displacement coordination condition between the wheel and the wheel-bridge deck contact points at any moment is established by changing the constant term of the constraint equation, thus considering the effect of pavement roughness.  
Step 8. After completing the solution, enter the time history post-processing to examine the system's dynamic response.  
With the gradual development of the finite element method, various finite element analysis software packages are available for researchers and engineers [42]. ANSYS provides extensive element and material libraries for numerical simulation [43]. Vehicle is a complex vibration system often simplified to consist of rigid components such as the body and wheels. Vehicle models have now evolved to allow simulation of various parameters,such as vehicle load and axle spacing [24]. Figure 1 shows a simplified model of a two-axle plane vehicle, considering the heave and pitch degrees of freedom for the vehicle body, as well as the heave degree of freedom for the wheelset. The mechanical model is illustrated in Figure 2, taking the multi-body model of a two-axle plane vehicle as an example. In this study, the vehicle body and bogie are represented using MASS21 mass elements, the suspension system is modeled with COMBIN14 spring-damper elements, and the vehicle body and suspension elements are connected by MPC184 rigid beam elements. In this study, bridge damping is not considered. The Newmark-\(\beta\) method is used for vehicle-bridge coupling analysis, with the key parameters of \(\gamma\) and \(\beta\) set to 0.5 and 0.25, respectively.