# Numerical Calculation and Experimental Study of the Axial Force of Aero Fuel Centrifugal Pumps
## 2 Numerical Simulation of Axial Force
### Boundary Conditions and Solution Settings  
Inner flow simulations are carried out by using the CFD code ANSYS Fluent 19.2 and the SST \(k\)-\(\omega\) turbulence model is used to solve the turbulent flow field in the pump. The SST model can accurately predict the flow in a wider range, especially for the calculation of the starting point of flow separation and the size of the separation area under the condition of negative pressure gradient. When calculating the centrifugal pump model with high specific speed, it can obtain more ideal calculation results compared with other  
Figure 4: Hybrid mesh of the computational domain: (**a**) centrifugal impeller grid and (**b**) centrifugal pump integral grid.  
Figure 5: Y-plus of the inducer and impeller blades surface: (**a**) inducer and (**b**) impeller.  
Figure 3: Grid independence verification.  
models [27; 28]. The transport equations of turbulent kinetic energy \(k\) and turbulent kinetic energy dissipation rate \(\omega\) are as follows:  
\[\frac{\partial(\rho k)}{\partial t}+\frac{\partial(\rho ku_{i})}{\partial x_{i}} =\frac{\partial}{\partial x_{j}}\left(\Gamma_{k}\frac{\partial k}{ \partial x_{j}}\right)+G_{k}-Y_{k} \tag{1}\]  
\[\frac{\partial(\rho\omega)}{\partial t}+\frac{\partial(\rho\omega u_{i})}{ \partial x_{i}}=\frac{\partial}{\partial x_{j}}\left(\Gamma_{\omega}\frac{ \partial\omega}{\partial x_{j}}\right)+G_{\omega}-Y_{\omega}+D_{\omega} \tag{2}\]  
where \(Y_{k}\) and \(Y_{\omega}\), respectively, represent the dissipation term of turbulent kinetic energy caused by turbulence and the dissipation rate of turbulent kinetic energy; \(\Gamma_{k}\) and \(\Gamma_{\omega}\), respectively, represent the effective diffusion coefficient of \(k\) and \(\omega\); \(G_{k}\) and \(G_{\omega}\), respectively, represent \(k\) and \(\omega\) generate items; and \(D_{\omega}\) denotes the cross diffusion term.  
Grid interface is used to transfer data between computing domains. The wall conditions of the pump inlet and outlet wall, volute wall, front cavity wall, and back cavity wall are set as static walls. The wall boundary of the impeller blade surface and the front and rear cover plates of the pump were set as non-slip and adiabatic rotation boundaries and the standard wall function was used near the wall. The flow medium is aero fuel kerosene with a density of 780 kg/s and a dynamic viscosity of 0.003 Pa-s at room temperature. The inlet boundary is set as the pressure inlet in the static coordinate system and the pressure value is set according to the experimental measurement of the model pump. The outlet boundary is set to the outlet with different masses according to the flow condition.  
The SIMPLEC solver is used for the discrete format of the system of equations. The standard format is adopted for the pressure term and the first-order upwind format is adopted for other terms such as the velocity term, turbulent viscosity coefficient, and turbulent kinetic energy term.  
The multi-reference frame model (MRF) is used to simulate the coupling relationship between the rotating domain and the stationary domain. After the steady-state calculation converges, the transient slip grid (SMM) is used to solve the unsteady flow field. In the transient solution, the number of turns was set as nine and the average monitoring value of the last three turns was set as the unsteady solution value.  
In order to verify the reliability of the numerical simulation results, the simulated head values under multiple flow conditions at 9000 r/min were compared with the test values, as shown in Figure 6. As can be seen from the figure, the simulated head number is basically consistent with the test value. Under the condition of large flow, the error is slightly larger and the maximum error is 6.5%, which is still within the allowable error range, indicating that the numerical calculation model is credible.  
Figure 6: Comparison of performance curves between experiment and CFD.