# Comparing Bol Implementation Methods in Vibration Testing for Accurate Dynamic Behavior Analysis
## 2 Materials and Methods
### Finite Element Analysis
The screw connection method (Figure 3e) models bolts as line bodies and connects the contact areas using Rigid Body Element 2 (RBE2) constraints. RBE2 ensures that all connected nodes behave as a rigid body, maintaining identical displacements and rotations across the nodes. In the screw connection method, bolts could be created simply without requiring additional contact conditions or the need to locate bolt positions. This method simplifies fastening, enabling efficient modeling and analysis. This connection method was implemented using the \"Fastener\" tool in the Inspire analysis program. The fixed bolt connection method (Figure 3f) also models bolts as line bodies and connects the contact areas using RBE2 constraints. Unlike the screw connection method, the nodes at the top and bottom of the CBAR are designated as fixed points, ensuring that both ends of the bolt remain completely fixed. Similar to the screw connection method, the fixed bolt method allows bolts to be created simply without assigning additional contact conditions or locating bolt positions. The fixed bolt method provides a fastening method that simulates connections where rigidity is relatively important. This connection method was implemented using the \"Fastener\" tool in the Inspire analysis program. For the representation of line bodies, BEAM188 elements were used in ANSYS analysis, while CBAR elements were used in Inspire. BEAM188 elements have the characteristic of allowing thickness information to be input for one-dimensional structures. Additionally, these elements have six degrees of freedom and can account for axial forces, shear forces, bending, and torsion moments. CBAR elements have the same degrees of freedom and can similarly represent the physical properties of bolts. In general, computational analysis results tend to indicate higher natural frequencies compared to experimental values, as they cannot perfectly account for all conditions. To address this, contact friction between contact areas, excluding bolt joints, was not considered in the contact conditions. This assumption was based on the relatively small contact area between the ribs. In addition, the bolts, positioned at 30 mm intervals, were considered sufficient to provide the necessary structural strength for the connection [24]. Moreover, the preload of the bolts was excluded, as it could excessively influence the computational analysis results by further increasing the structural strength. Figure 5 shows the finite element model of the entire jig. The FE model of the jig was constructed using SOLID185 in ANSYS, 8-node solid elements. This element uses the simplified enhanced strain formulation. Enhanced strain formulation modifies gradient tensor and strains in lower-order elements to prevent shear and volumetric locking [25]. The model consisted of 1,094,136 nodes and 627,725 elements, with an average aspect ratio of 2.31 and an average Jacobian ratio of 0.97, indicating sufficient mesh quality [26]. The detailed calculations are provided in Appendices A and B. The bolt material properties were assigned based on AISI 304 stainless steel (density: 8 \(\times\) 10\({}^{-6}\) kg/mm\({}^{3}\), Young's modulus: 195.0 GPa, Poisson's ratio: 0.29, and yield strength: 215 MPa). The jig material properties were assigned based on Aluminum Die Casting (ALDC) (density: 2.75 \(\times\) 10\({}^{-6}\) kg/mm\({}^{3}\)  
Young's modulus: 69.6 GPa, Poisson's ratio: 0.33, and yield strength: 165 MPa). The analysis was conducted using the ANSYS 24 R1 and Inspire 2023 programs. A personal computer (Intel i9-12900K, GPU: GEFORCE RTX 3080, RAM: 64 GB, Santa Clara, CA, USA) was used for the analyses.