## 3 Methodology
### Establishing Analysis Models  
In ANSYS Fluent 17, the pressure-based solver was selected due to its versatility across various applications and its numerical efficiency, despite requiring approximately 1.5 to 2 times more memory than the density-based method. During the initial simulation phase, the standard k-\(\omega\) turbulence model was employed [56], which involves solving transport equations for the turbulence kinetic energy (k) and the specific dissipation rate (\(\omega\)). This model is suitable for accurate boundary layer analysis and flows with low Reynolds numbers but necessitates fine mesh discretization near solid surfaces to yield reliable results. Due to inconclusive initial findings, the transient SST k-\(\omega\) model was subsequently implemented [57]. This model integrates the shear stress transport (SST) mechanism to combine the advantages of two distinct modeling approaches. The SST k-\(\omega\) model demonstrates superior capability in accurately capturing boundary layer phenomena, extending down to the viscous sublayer, and performs efficiently in low Reynolds number flows without requiring additional damping functions. Although the SST model significantly improves velocity profile predictions and flow separation under adverse pressure gradients [58], it demands increased mesh density near solid boundaries. For radiative heat transfer analysis, the surface-to-surface (S2S) model was chosen, as it can simulate one-, two-, and three-dimensional geometric configurations, including cylindrical shapes through body-fitted coordinates (BFC). The S2S model facilitates radiative heat transfer simulation in both laminar and turbulent regimes and allows the specification of imposed heat flux, temperature, or radiative properties on surfaces [59]. Its operation is based on subdividing surfaces into zones of uniform temperature, requiring the evaluation of geometric or view factors to quantify radiative heat flux exchange. Regarding the solution methods, a model using a velocity-pressure coupling scheme (coupled) was selected, as it enables faster convergence compared to a solver that does not couple velocity and pressure. In this analysis, an important factor is the interpolation of numerical methods, which is necessary for evaluating diffusion fluxes, calculating velocity gradients, and applying higher-order discretization schemes. The least-squares cell-based method was chosen, as it is recommended for hexahedral meshes. For pressure analysis, the body force weighted method was selected, as it is the most suitable in the case of natural convection with a high Rayleigh number. Numerical solution strategies included a velocity-pressure coupling scheme, favored for optimizing the convergence rate compared to segregated methods. Interpolation techniques, essential for evaluating diffusion fluxes, velocity gradients, and within higher-order discretization schemes, constituted a key element of the analysis. For geometries discretized with hexahedral elements, the \"Least-Squares Cell-based\" method was selected, while the \"Body Force Weighted\" method was applied for pressure field calculation, recognized for its efficiency in simulating natural convection phenomena at significant Rayleigh numbers. Regarding momentum evaluation, the upwind scheme was implemented, known for its simplicity and robustness, although it introduces more pronounced numerical dissipation dependent on flow properties. The precision difference between first-order and second-order discretization methods is considerable, with the second-order upwind scheme ensuring superior accuracy. For a rapid estimation of the flow field--including variables such as velocity, pressure, temperature, turbulence, and volume fractions--hybrid initialization was employed initially. This technique combines various methods and is based on Laplace's equation.