# Analysis of the Guide Vane Jet-Vortex Flow and the Induced Noise in a Prototype Pump-Turbine
## 4 CFD Setup  
Based on the fluid domain shown in Figure 1, the computational fluid dynamics (CFD) simulation was conducted using the commercial code CFX in ANSYS (v18, Pittsburgh, PA, USA). The mesh used in the CFD simulation was done by using ICEMCFD with structural hexahedral elements and checked in size and in \(y^{+}\). The mesh size was checked by using the grid convergence index (GCI) method [37] at the condition C\({}_{1}\). The pressure difference between the solute outlet and draft tube inlet was selected as the index. Three mesh schemes with 1'062'882, 2'813'808, and 6'511'958 nodes were GCI-checked with the discretization uncertainty of 5.5%, which is smaller than the limit of acceptance limit of 10% [37]. Thus, the final mesh scheme had 6'511'958 nodes to balance the accuracy and the computational cost. The \(y^{+}\) value on all the walls was controlled between 0.27 and 9.13 for applying the automatic wall-function [38] by refining the near-wall first layer height. The detail of mesh node number is shown in Figure 3. To capture the complex undesirable flow regime, especially from the runner outlet to the stay vane outlet, the mesh node density in these regions were specifically refined.  
The multiple reference frame (MRF) model [39] was used where the draft tube, guide vane, stay vane, and volute were stationary, and the runner was rotational by \(n_{d}\) = 430 r/min. The fluid medium, which is mentioned above, was set as water at 20 \({}^{\circ}\)C, with a molar mass of 18.02 g/mol, density of 997 kg/m\({}^{3}\), dynamic viscosity of \(8.899\times 10^{-4}\) kg/m\(\cdot\)s. The environment pressure was set as 1 Atm. The boundary conditions are given as follows:  
* A velocity inlet boundary was given at the draft tube inflow with uniformly distributed value.
* A static pressure outlet boundary of 0 Pa was given at the volute outflow.
* No-slip wall boundaries were given on all the solid walls.
* Interfaces were set for connecting different domains based on the general grid interface method. The \"frozen rotor\" type was used for the rotor-stator interface in steady state simulations. The \"transient rotor stator\" type was used for transient simulations.  
Both the steady state and transient simulations were conducted. The steady state simulation was the initial simulation by 600 steps. It converged based on the criterion of root-mean-square (RMS) residuals of the continuity and momentum equations of less than \(1\times 10^{-5}\). The transient simulation was based on the steady state results. More than 5 runner revolutions were simulated. In one runner revolution, 720 time steps were conducted. At most, 10 iterations were allowed for the convergence of each time step based on the convergence criterion of RMS residuals of less than \(1\times 10^{-6}\). The discrete form of the advection term in both the momentum equation and the turbulent transport equation were set as high resolution. Based on the guide vane opening angle law shown in Figure 2, the mesh scheme and numerical setup above were verified by comparing them with the model-test. Because the internal flow regime is unable to capture in model-test, the efficiency \(\eta\) was chosen for verification. The numerical \(C_{\varphi}\)-\(\eta\) data was compared with experimental \(C_{\varphi}\)-\(\eta\) data, as shown in Figure 4. The 4 compared conditions include the objective condition C\({}_{1}\), the best efficiency condition, another partial-load condition, and another over-load condition. The same tendency can be observed. It proves that the mesh scheme and numerical setup is somehow reliable for flow mechanism analysis.