# Design and Numerical Analysis of Recuperator for a Liquid Carbon Dioxide Energy Storage System
## 3 Numerical Calculation Method and Validation of Numerical Method
### Computational Meshes and Boundary Conditions  
The tetrahedral unstructured grid utilized in the validation model calculation was generated using ANSYS ICEM. To improve the grid quality, prism grids were employed near all wall surfaces. For low Reynolds number turbulence models based on the \(\omega\) equation, it is required that the value of \(y^{+}\) near the wall be less than 1. Therefore, the thickness from the first mesh layer of the cold-side fluid to the wall surface was set to 0.0001 mm, and 32 layers of prism grids were arranged in the vertical wall direction with a grid expansion ratio of 1.2. Similarly, for the hot side fluid, the distance from the initial mesh to the wall surface was defined as 0.0002 mm, and 28 layers of prism grids were placed in the vertical wall direction with a grid expansion ratio of 1.2. The thickness between the first mesh at the solid-fluid interface and the boundary was the same as that on the corresponding fluid side, and 8 layers of prism grids were arranged in the vertical boundary direction. The count of grid nodes was around 3.081 million, and the total number of elements was approximately 6.58 million. For high Reynolds number turbulence models based on the \(\varepsilon\) equation, the first layer grid adjacent to the wall needed to be placed in the area of intense turbulence. In this case, a two-layer prism grid was used, and the distance from the initial layer grid to the wall surface was defined as 0.1 mm and \(y^{+}\) was controlled between 12 and 80. On the solid-fluid interface, the initial layer grid was set at the same distance from the boundary as on the corresponding fluid side, and 1 layer of prism grid was arranged vertically along the boundary direction. The total number of grid nodes was approximately 398,000 and the count of elements was around 1.216 million.  
\begin{table}
\begin{tabular}{c c c c c c} \hline \hline  & **Channels** & **Diameter/mm** & **Angle/\({}^{\circ}\)** & **Segment Length/mm** & **Length/mm** \\ \hline Hot Side & 2 & 1.9 & 32.5 & 4.5 & 54 \\ Cold Side & 1 & 1.8 & 32.5 & 4.5 & 54 \\ \hline \hline \end{tabular}
\end{table}
Table 4: Geometry of the PCHE used for turbulence model validation.  
Figure 3: Geometry of the PCHE unit used in the validation calculation.  
ANSYS CFX was performed in the calculations process, and boundary conditions were consistent with those of [PERSON] et al. [22]. The inlet pressure was set to 3.2 MPa for the cold side and 10.5 MPa for the hot side. The inlet temperature on the hot side was 280 \({}^{\circ}\)C. Figure 4 displays the temperature distribution, with the computational range limited to 0 to 0.054 m. Therefore, according to Figure 4, the cold-side inlet temperature of CO\({}_{2}\) was set to 221.8 \({}^{\circ}\)C, which corresponds to the temperature at the location of 0.054 m. The inlet turbulence intensity was set to 5% for both channels. The mass flow rate boundary conditions were specified at the outlets of both channels, with the total flow rate being the same. A total of 13 operating conditions were calculated over the mass flow rate scope of 30-390 kg\(\cdot\)h\({}^{-1}\). The fluid-solid interface was defined as a coupled heat transfer boundary. Periodic boundaries were set to the left-right and top-bottom surfaces. The total energy model was adopted for the fluid domain in the calculations. The properties of CO\({}_{2}\) were obtained from the RGP property parameter table derived from NIST. The solid domain was modeled using a thermal energy model that neglects density variations during the solution process. \"Steel\" was set as the material from the material library, and \(\lambda\) is 16.2 W\(\cdot\)m\({}^{-2}\cdot\)K\({}^{-1}\).