## 2 Methodology
### Numerical Method and Validation  
Vista Centrifugal Compressor Design (Vista CCD), available in ANSYS Workbench, was used to design the radial compressor. The design inputs of the compressor, shaft speed, mass flow rate, pressure ratio, air inlet temperature, and pressure were entered. In the continuation of the same module, geometric measurements, hub diameter, shroud diameter, the number of blades, and tip clearance values were entered. A compressor with 0.254 mm tip clearance and 18 blades without intermediate blades was designed as the number of blades. A mesh structure suitable for the design was created using the Turbogrid module. The normal distance option was selected by checking the override upstream geometry options. Automatic was selected for topology settings. The global size factor method was used for the mesh structure, and the method proportional to the mesh size was used for boundary layer improvement control. The absolute method was used for the element size near the wall. Figure 4 shows the mesh structure. In Turbogrid, mesh statistics are used to see the quality of the mesh. Thus, the quality parameters of the created mesh such as minimum surface angle, maximum surface angle, maximum element volume ratio, and minimum volume ratio were examined. Percentage distortions were checked for entry, exit, and passage, and all were achieved with zero percent error. The minimum surface angle was 22.23\({}^{\circ}\) and the maximum surface angle was 160.72\({}^{\circ}\). Figure 4: Mesh structure. Figure 3: The outline of the design methodology. Conservation equations for each element created were solved by the program. For a compressible, steady-state, homogeneous, and Newtonian fluid, the continuity, momentum, and energy equations can, respectively, be written as follows [32]:  
Continuity equation:  
\[\frac{\partial\rho}{\partial t}+\frac{\partial}{\partial xj}\left(\rho\text{U} _{j}\right)=0 \tag{1}\]  
Momentum equation:  
\[\frac{\partial(\rho\text{U}i)}{\partial t}+\frac{\partial}{\partial xj}\big{(} \rho U_{i}U_{j}\big{)}=-\frac{\partial p^{\prime}}{\partial xj}+\frac{ \partial}{\partial xj}\bigg{[}(\mu+\mu_{t})\bigg{(}\frac{\partial Ui}{ \partial xj}+\frac{\partial Uj}{\partial xj}\bigg{)}\bigg{]}+S_{M} \tag{2}\]  
where \(S_{M}\) is the sum of body forces, \(\mu_{t}\) is turbulent viscosity, and \(p^{\prime}\) is the modified pressure. Energy equation:  
\[\frac{\partial(\rho h_{e})}{\partial t}-\frac{\partial p}{\partial t}+\frac{ \partial}{\partial t}\big{(}\rho U_{j}h_{e}\big{)}=\frac{\partial}{\partial xj }\bigg{(}\lambda\frac{\partial T}{\partial xj}-\rho\ \overline{u_{i}h_{e}}\bigg{)}+\frac{ \partial}{\partial xj}[U_{i}(\tau_{ij}-\rho\ \overline{u_{i}u_{j}})] \tag{3}\]  
Which is suitable for flows and can be useful for liquids and gases in ANSYS CFX. The term \(\rho\ \overline{u_{j}h_{e}}\) is additional turbulence flux and the \(\frac{\partial}{\partial xj}[U_{i}(\tau_{ij}-\rho\ \overline{u_{i}u_{j}})]\) term in the equation is the viscous work term. Symbol \(h_{e}\) is the enthalpy, and \(\lambda\) is thermal conductivity. After the mesh structure was created, computational fluid dynamics analyses were performed using CFX-Pre. In order to analyze the experimental studies in the literature, the same inlet and outlet sections were designed and analyses were carried out as a vaneless diffuser, as in the literature. In the ANSYS CFX module, the radial compressor and coordinate system are defined as the machine type. Steady-state and compressible flow properties were preferred as analysis types. Rotation and speed as 17,473 rpm were entered as the component type. As for the wall structure, the tip clearance at the shroud was marked yes, and the tip clearance at the hub was marked no. Ideal air was chosen as physical definitions, reference pressure was chosen as 0 atm, heat transfer was chosen as total energy, and turbulence was chosen as shear-stress transport (SST).