## 3 Valve Opening Characteristics  
### Investigation Methods and Boundary Conditions  
The opening and closing of the valve is typically an almost instantaneous process. In actual operation, it is difficult to observe the change of the internal flow field during the opening of the high-pressure valve. With the development of information technology, various simulation tools based on numerical investigation methods are being widely used in various industries to overcome the deficiencies of experimental methods [26; 27; 28; 29; 30; 31]. For valve design problems, computational fluid dynamics (CFD)-based simulation methods are often used in the industry to study the dynamic changes in the flow field [32; 33; 34]. In this numerical investigation, the global unstructured tetrahedral mesh is used for the discretization of the high-pressure liquid basin, and the grid at the valve gap is locally refined. The Reynolds-averaged Navier-Stokes (RANS) equation governing the fluid flow is solved in the commercial CFD software Ansys Fluent using a workstation (Manufacturer: Lenovo, Seoul, Korea) with an Intel Xeon E5 2690 v4 processor operating at 2.6 GHz with 128 GB of RAM. In the simulation, the fluid is assumed to be incompressible and conforming to the RANS equation. Ansys fluent provides many RANS turbulence models to solve different fluid dynamics problems (e.g., Spalart-Allmaras, Standard k-epsilon, renormalization group (RNG) k-epsilon, Realizable k-epsilon, standard k-omega, Menter's shear stress transport (SST) k-omega, Reynolds stress etc.) [35]. In this study, the Standard k-epsilon model was adopted because it has been verified by numerous studies that, for calculations related to hydraulic power transmission systems, this model is more stable, economical and accurate than other turbulence models [32; 34]. The semi-Implicit method for pressure implicit method for pressure-linked equations (SIMPLE) solver is used to solve momentum and continuous equations. This method uses a second-order upwind style to discretize the equations in parallel grid nodes to ensure the accuracy of the simulation results. The boundary conditions are set as pressure inlet and pressure outlet for this calculation domain. The initial pressure value of the valve is set as 630 kPa, and the outlet pressure is set as 530 kPa. In this simulation, international organization for standardization (ISO) VG32 hydraulic oil with a density of 844.4 kg/m\({}^{3}\) and a dynamic viscosity of 0.0135 kg/m\(\cdot\)s is used as the transportation medium. In order to more intuitively observe the NFFCS' effects of instantaneous pressure relief and easy coupling, same-sized (ISO 16082 size 10) CFFCS and NFFCS were separately pre-processed for modeling and simulation. In this study, the entire valve opening process of the two hydraulic couplings was simulated using novel dynamic mesh technology. The dynamic mesh algorithms mainly include layering, smoothing and remeshing [22]. Considering the complexity of the internal geometric structure of the hydraulic coupling systems, it is difficult to use a layering method that is highly dependent on prismatic meshes. Therefore, in this study, smoothing and remeshing methods were adopted for dynamic meshing. The general conservation equation of a dynamic mesh [36; 37] for a general scalar (\(\Phi\)) on an arbitrary control volume (\(V\)), whose boundary is moving, can be written as:  
\[\frac{\partial}{\partial t}\int_{V}\rho\varpi dV+\int_{A}\rho\varnothing\left( \overset{\rightarrow}{v}-\overset{\rightarrow}{v}_{g}\right)\cdot d\overset{ \rightarrow}{A}=\int_{A}\left(\Gamma\
abla\varnothing\right)\cdot d\overset{ \rightarrow}{A}+\int_{V}S_{\varnothing}dV \tag{1}\]  
where \(\overset{\rightarrow}{v}\) is the speed vector; \(\overset{\rightarrow}{v}_{g}\) ts the grid velocity of the moving mesh, \(\rho\) is the liquid density, \(\Gamma\) is the diffusion coefficient, and \(S_{\varnothing}\) represents the source term of \(\varnothing\).