## 2 Verification of Simulation Methods
### Numerical Method  
Figure 5 illustrates the computational model of the fast transient response process for the cavity-tube combined flow path under sudden boundary changes. This simplified model comprises the cavity-tube fluid domain and the atmospheric fluid domain, corresponding to the green and blue sections in Figure 5, respectively. In the experiment, the gas within the cavity-tube flow path directly enters the atmosphere. To simulate the influence of the atmospheric environment on the outlet boundary conditions of the flow path, a dual fluid domain modeling approach is employed, with both fluid domains lacking inlets or outlets. The entire fast transient response process occurs within these two fluid domains. The initial pressures of the cavity-tube fluid domain and the atmospheric fluid domain differ; at the beginning of the simulation, the two fluid domains are connected to facilitate the abrupt boundary change in the cavity-tube combined flow path. Additionally, to ensure that atmospheric pressure remains relatively constant during the simulation, the volumes of the two fluid domains meet condition \((V_{Vessel}+V_{Pipe})/V_{Air}\ll 1\). Relevant parameters for the atmospheric fluid domain are presented in Table 2, while other model parameters are consistent with those in Table 1.  
Figure 4: Schematic diagram of the sudden change boundary simulation device. Figure 5: Schematic diagram of the cavity-single tube model. The entire model is constructed using a hexahedral mesh. The O-Block partitioning technique is utilized to separately address the cavity-tube fluid domain and the atmospheric fluid domain, facilitating the creation of a regular hexahedral mesh structure on the curved surfaces. To capture flow details more accurately in critical areas, the mesh in the wall regions, the interface between the two fluid domains, and the junction between the cavity and the tube has been refined. The initial layer mesh height is set to 0.05 mm, with a normal growth rate of 1.2, allowing for a gradual transition between refined and non-refined meshes. The results of the mesh partitioning are presented in Figure 6.  
This study employs ANSYS CFX 2021 software for three-dimensional transient numerical simulations. The fluid is represented as an ideal gas, with the convective terms in the momentum, energy, and turbulence equations discretized using a second-order upwind scheme. The entire fast transient response occurs over a very short time frame, and wall heat transfer is not considered; all walls are defined as adiabatic no-slip boundaries. Due to the small diameter of the interaction interface between the fluid domains, the flow near the inlet and outlet of the cavity resembles a circular jet. According to the research by [PERSON] et al. [20], the SST turbulence model exhibits high simulation accuracy for circular jet modeling; therefore, this study prioritizes the SST turbulence model and performs grid independence and time step analyses prior to selecting the turbulence model. Throughout the simulation process, convergence is deemed achieved when the residuals reach approximately times \(10^{-4}\). The appropriate grid resolution is determined through grid independence verification, with the time step temporarily set to times \(10^{-5}\) s, aligning with the precision of the experimental data collection. The model is simulated using grid counts of 0.03 million, 0.06 million, 0.09 million, 0.14 million, 0.31 million, and 0.52 million. Static pressure monitoring points are established in the model based on the locations of pressure measurement points from the experiments. By comparing the variations in static pressure at these monitoring points, an appropriate grid resolution is identified; the locations of the measurement points and the comparison results are presented in Figure 7. Once the grid count reaches