# Optimization Study on a Novel High-Speed Oil-Free Centrifugal Water Pump with Hydrodynamic Bearings
## 2 Numerical Model
### Control Equation and Solution  
The commercial CFD code CFX (Computational Fluid X) 18.0 was employed to simulate the 3D incompressible flow under a steady condition. It was assumed that physical properties of the fluid kept constant during the computation, as well as the effect of gravity, was neglected. The continuity and momentum equations are shown below [22]:  
Continuity equation:  
\[\frac{\partial u_{i}}{\partial x_{i}}=0 \tag{1}\]  
Momentum equation:  
\[\frac{\partial u_{i}}{\partial t}+u_{j}\frac{\partial u_{i}}{\partial x_{i}}=f _{i}-\frac{1}{\rho}\frac{\partial p^{*}}{\partial x_{i}}+v\frac{\partial^{2}u _{i}}{\partial x_{j}^{2}} \tag{2}\]  
where \(\rho\) is the liquid density, \(x_{i}\), \(x_{j}\) is the components along three directions, \(i,j=1,2,3\). \(u_{i}\), \(u_{j}\) is the velocity components, \(f_{i}\) is the components of body force, \(p^{*}\) is the reduced pressure including the turbulence kinetic energy and centrifugal force, and \(v\) is the coefficient of the kinematic viscosity. [PERSON] et al. [23] pointed out that the \(k-\varepsilon\) turbulence model is popular for numerical research of the centrifugal pump. They examined the applicability of the standard \(k-\varepsilon\) model, the renormalization group (RNG) \(k-\varepsilon\) model, and the Realizable \(k-\varepsilon\) model, concluding that these three models were suitable for the numerical simulation of the internal flow inside a centrifugal pump. Therefore, the standard \(k-\varepsilon\) model is chosen in this study and the transport equations are shown as follows. The detailed information is introduced in [23; 24]. The standard \(k-\varepsilon\) turbulence transport equations:  
\[\left\{ \begin{array}{ll}\frac{\partial}{\partial t}(\rho k)+\frac{\partial} {\partial x_{i}}(\rho u_{i}k)=\frac{\partial}{\partial x_{j}}\left[\left(u+ \frac{\mu_{i}}{\partial x_{i}}\right)\frac{\partial k}{\partial x_{j}}\right] +\rho(p_{k}-\varepsilon)\\ \frac{\partial}{\partial t}(\rho\varepsilon)+\frac{\partial}{\partial x_{i}}( \rho u_{i}\varepsilon)=\frac{\partial}{\partial x_{j}}\left[\left(\mu+\frac{ \mu_{i}}{\varepsilon_{j}}\right)\frac{\partial k}{\partial x_{j}}\right]+ \rho\frac{\varepsilon}{\left(C_{1}p_{k}-C_{2}\varepsilon\right)\end{array} \right. \tag{3}\] \begin{table}
\begin{tabular}{c c c c} \hline \hline
**Parameter** & Coarse (2,087,663) & Medium (4,569,430) & Fine (6,857,792) \\ \hline
**Head at BEP(m)** & 24.11 & 25.02 & 25.18 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Mesh independence study. BEP: Best efficiency point. Figure 4: Mesh of flow path in the thrust bearing and mesh independence study. The turbulent viscosity \(\mu_{t}\) is computed as follows:  
\[\mu_{t}=\rho C_{\mu}\frac{k^{2}}{\varepsilon} \tag{4}\]  
where \(C_{\mu}\), \(\sigma_{k}\), \(\sigma_{c}\), \(C_{1}\), and \(C_{2}\) are the coefficients of the turbulence model. \(p_{k}\) represents the generation of the turbulence kinetic energy induced by the mean velocity gradients. Pressure-velocity coupling is achieved by the SIMPLE algorithm, which can reformat the continuity equation and derive an additional condition for the pressure. The inlet and outlet boundary conditions greatly affect the accuracy and the convergence of calculation results. The pressure inlet and mass flow rate outlet conditions were specified at the inlet and outlet to obtain good convergence. The turbulence kinetic energy \(k_{in}\) and the turbulence dissipation rate \(\varepsilon_{in}\) of the inlet are computed by Equation (5). \[\left\{ \begin{array}{l}k_{in}=0.005u_{in}^{2}\\ \varepsilon_{in}=\frac{C_{0}^{3/4}k_{in}^{2/3}}{0.07D_{in}}\end{array} \right. \tag{5}\]  
where \(u_{in}\) is the inlet velocity and \(D_{in}\) is the inlet diameter. As for the wall boundary condition, the no slip condition was imposed on the wall surface. This assumes that there is no relative velocity between the liquid and the wall. Therefore, the flow adjacent the wall had a low Reynolds number and the standard wall function was adopted to compute the flow at the adjacent region.