## 2 Methodology
### Overall of the CFD Design  
Figure 1 shows the overview of the three-dimensional (3D) simulation model of the offshore cabin, where the ventilation module consists of an air inlet part, a heating unit, and an exhaust vent. The air flow motion follows three laws of conservation in physics [13], namely, the laws of conservation of mass, conservation of momentum, and conservation of energy. These laws provide the theoretical basis of the numerical calculation for the ventilation design. The dimensions of the 3D model were \(18.8\times 18.3\times 7.7\) m in length, width, and height. The total volume of the cabin was 2003.26 m\({}^{3}\). In order to make the boundary conditions of the cabin model more realistic, reverse engineering was adopted to establish the 3D model. To be specific, the air basin was an entity in the operation domain, while in the noncomputational domain the heat dissipation path, the base gantry, and the auxiliary equipment were hollowed out. The arrangement inside the cabin model is shown in Figure 2. Considering that the diesel engine in the full load condition inhales 12% of the ventilation air [14], the gas inlets were set to both sides of the diesel engine. Due to the high temperature of the exhaust gas, the exhaust vent was placed at the roof of the model. In the model meshing process, in order to make a tradeoff between calculation complexity and accuracy, the boundary layer mesh was not adopted. Considering the surface complexity of the heating components and the exhaust port, the unstructured/flexible grid method was adopted, namely, large grid elements were used in the areas where the computing accuracy requirement was low, while grid refinement was adopted in the areas where heat or gradient changes occurred. By doing so, a good tradeoff between the calculation accuracy and complexity can be achieved. Figure 1: Three-dimensional model of the main cabin of the offshore platform. Figure 2: _Cont._  
The grid-independence was carried out to determine the grid number of the model. Table 1 shows the evaluation results. As can be seen in the table, when the grid number increased to 1,490,000 the temperature difference \(\Delta T\) between the inlet and outlet of the ventilation system was 7.54 \({}^{\circ}\)C, and the output ventilation volume \(V_{o}\) was 6.94 m/s. When the grid number kept increasing to 1,840,000, the temperature difference \(\Delta T\) decreased significantly to 6.32 \({}^{\circ}\)C, and the ventilation volume \(V_{o}\) increased to 8.37 m/s. However, when further increased the grid number all along to 2,170,000, \(\Delta T\) and \(V_{o}\) changed a little, which suggested that the ventilation reached a stable condition from the inlet to the outlet. As a result, this study selected a mesh size of 2,192,711 elements and 387,897 nodes in total, to make the CFD solution mesh-independent [15; 16; 17]. There are four types of turbulence model in FLUENT, namely Standard k-\(\epsilon\) model, Re-normalisation group (RNG) k-\(\epsilon\) model, Standard k-\(\omega\) model, and shear stress transport (SST) k-\(\omega\) model. In order to select the most suitable model for the CFD simulation in this study, a comparison was performed using these four turbulence models with the same CFD setting [16]. The Reynolds number in different regions of the cabin model varied from \(5\times 10^{5}\) to \(1\times 10^{6}\). Table 2 shows the comparison results. As can be seen in the table, the standard k-\(\epsilon\) model produced the least temperature difference, \(\Delta T\) 6.32 \({}^{\circ}\)C, while the SST k-\(\omega\) model generated the largest output ventilation volume, \(V_{o}\) 8.90 m/s, among these four turbulence models. Considering that the computation time of the standard k-\(\epsilon\) model is less than that of the SST k-\(\omega\) model, this study adopted the standard k-\(\epsilon\) model in the CFD simulations.