## 3 Materials and Methods
### Numerical Modeling
#### 3.3.4 Mesh Generation  
A mesh refinement strategy was adopted to balance computational efficiency and result accuracy, prioritizing denser elements in critical regions while using coarser elements in areas with lower structural influence. The mesh density for each model part was determined separately based on a mesh sensitivity analysis. This study was conducted by progressively reducing the element size until the differences between the finite element (FE) model results and experimental data were minimized. This approach ensured that the mesh was not excessively refined, which would significantly increase computational time, nor too coarse, which could compromise result accuracy [56; 57].  
Figure 11 illustrates that different mesh densities were applied according to structural importance. A finer mesh was employed in the connection region, where stress concentration and deformation behavior were of greater interest. The mesh density varied between fine (2 \(\times\) 2 mm\({}^{2}\)), medium (5 \(\times\) 5 mm\({}^{2}\)), and coarse (10 \(\times\) 10 mm\({}^{2}\) to 20 \(\times\) 20 mm\({}^{2}\)), ensuring appropriate resolution in areas where precision was essential. Conversely, coarser elements were applied to regions farther from the connection, optimizing computational cost without compromising result accuracy [50; 58]. All the elements used in the modeling were second-order, allowing for greater displacement interpolation accuracy and improved solution convergence.  
The mesh was generated using the multizone method, improving discretization quality by reducing element geometric distortion. This method combines mapping techniques  
Figure 11: Mesh representation applied to the structural model: (**a**) overview of the structural assembly, highlighting the variation in mesh density between critical and less relevant areas; (**b**) enlarged detail of the connection region, showing the refined mesh.  
with automatic geometry subdivision, ensuring an efficient mesh for complex structural analyses [21; 27]. The multizone technique is particularly advantageous for models involving multiple contact interfaces, as it allows the generation of structured hexahedral dominant meshes while preserving geometric fidelity and minimizing numerical artifacts across surfaces under contact conditions [30]. Additionally, the Inflation method was explicitly applied to nuts and bolts, particularly at the bolt head, as the hexagonal model was adopted to represent the actual fastening geometry. This approach enabled mesh refinement in contact regions, ensuring a smooth transition and accurately capturing stress gradients on these surfaces [27; 54].  
The bolts used in the model corresponded to M12 class 8.8, following normative specifications. The bolt head and nut were modeled in their original hexagonal shape, without the inclusion of threading on the bolt shank, as illustrated in Figure 12. This simplification was adopted to optimize processing time without compromising the structural behavior representation of the bolted connections [58].  
Although finer mesh elements increase processing time, the estimated time for executing each analyzed model ranged between 4 and 6 h, depending on the complexity of the model being calculated. The finite element models (FEM) were implemented on a high-performance server, utilizing 62 processing cores, ensuring computational efficiency and greater capacity for detailed simulations [56]. The server configuration consisted of 2 AMD EPYC 7513 Processors at 2.6 GHz, a Dual MZ92-F50 Board, 32 memory banks, 512 GB of DDR4/3200 MHz ECC Reg. memory, 1 \(\times\) 2 TB SSD, 1 \(\times\) 16 TB Seagate Hard Drive (ST16000 NM), and a 2U Rack R282-Z93 with a redundant power supply.  
This meshing strategy ensured that the numerical model achieved a high level of accuracy while maintaining computational feasibility, allowing for reliable structural simulations within a reasonable processing time [21; 57].