## 2 Numerical Simulation of Flow Forces in Slide Valves
### CFD Simulation of Flow Force  
The flow channel model of the pressure relief valve is created in the 3D modeling software ProE 5.0 and imported into ANSYS/Fluent 17.0 for fluid domain numerical simulation. ANSYS/Fluent 17.0 provides various turbulence models, including \(k\)-\(\varepsilon\), \(k\)-\(\omega\), and Reynolds models. Due to the throttling effect at the valve port, the velocity gradient of the fluid in the valve chamber is significant, with a high Reynolds number flow at the center of the valve chamber and low Reynolds number flow near the wall. According to [PERSON] et al. [28], the \(k\)-\(\varepsilon\) model performs well in hydraulic flow fields, and it has been successfully used in numerous studies of steady flow forces on valve spools, such as those by [PERSON] et al. [25; 26; 29], [PERSON] et al. [21; 22] and [PERSON] et al. [18; 19]. The governing equations of the \(k\)-\(\varepsilon\) turbulence model are as follows:  
\[\frac{\partial}{\partial t}(\rho k)+\frac{\partial}{\partial x_{i}}(\rho ku_{ i})=\frac{\partial}{\partial x_{i}}[\left(\mu+\frac{\mu_{t}}{\sigma_{k}} \right)\frac{\partial k}{\partial x_{j}}]+G_{k}+G_{b}-\rho\varepsilon-Y_{M}+S _{k} \tag{7}\]  
\[\frac{\partial}{\partial t}(\rho\varepsilon)+\frac{\partial}{\partial x_{i}} (\rho\varepsilon u_{i})=\frac{\partial}{\partial x_{j}}[\left(\mu+\frac{\mu_ {t}}{\sigma_{\varepsilon}}\right)\frac{\partial\varepsilon}{\partial x_{j}}] +C_{1\varepsilon}\frac{\varepsilon}{K}(G_{k}+C_{3\varepsilon}G_{b})-C_{2 \varepsilon}\rho\frac{\varepsilon^{2}}{k}+S_{\varepsilon} \tag{8}\]  
where \(G_{k}\) represents the turbulent kinetic energy generated by the mean velocity gradient; \(G_{b}\) denotes the turbulent kinetic energy generated by buoyancy; \(Y_{M}\) is the contribution of compressible turbulence expansion to the total dissipation rate; \(C_{1\varepsilon}\), \(C_{2\varepsilon}\), and \(C_{3\varepsilon}\) are model constants; \(\sigma_{k}\) and \(\sigma_{\varepsilon}\) are turbulent Prandtl numbers; \(S_{k}\) and \(S_{\varepsilon}\) are user-defined source terms; and \(\mu_{t}\) is the turbulent viscosity, which is related to \(k\) and \(\varepsilon\) as follows:  
\[\mu_{t}=\rho C_{\mu}\frac{k^{2}}{\varepsilon} \tag{9}\]  
where \(C_{\mu}\) is a model constant. The coefficients in the \(k\)-\(\varepsilon\) turbulence model adopt the following recommended values [30]: \(C_{1\varepsilon}=1.44\), \(C_{2\varepsilon}=1.92\), \(C_{3\varepsilon}=0.09\), \(\sigma_{k}=1.0\), and \(\sigma_{\varepsilon}=1.3\). In the low Reynolds number boundary layer region near the wall, viscous forces dominate momentum, mass, and heat transfer, and turbulence models cannot accurately resolve the flow field in the boundary layer. In this study, the enhanced wall treatment method in ANSYS/Fluent 17.0 is employed to handle boundary layers. This approach combines the two-layer zonal model with enhanced wall functions, making it independent of wall-law assumptions and well suited for complex flows, particularly low Reynolds number flows. When the near-wall mesh is sufficiently refined (the \(y+\) of the first node near the wall close to 1), it can resolve the entire turbulent boundary layer, including the viscous sublayer [8]. The working fluid is hydraulic oil with a density of 870 kg/m\({}^{3}\) and a dynamic viscosity of 0.04 Pa-s, while the mating clearance between the valve spool and sleeve is neglected. Pressure boundary conditions are applied at the inlet and outlet, with a typical pressure difference of 1 MPa, where the inlet pressure is 2.5 MPa and the outlet pressure is 1.5 MPa. Using the aforementioned CFD settings, the model is solved, and the obtained velocity, pressure, and other flow field information in the valve chamber are substituted into pressure Equation (1) and momentum Equation (3) to achieve a numerical solution for the steady flow force on the spool of the slide valve.