## 2 Materials and Methods
### Finite Element Analysis Procedure  
The CAD model of the instrument was prepared for the FEA procedure and imported into the FEA code. The mechanical module of the ANSYS Workbench (v 2022R2) commercial FEA code was utilised for the deformation analysis. The original geometrical details of each component were included in the analysis to simulate realistic deformation behaviour under pre-defined boundary conditions. Three different playing tunes (B2 (Si) (123.5 Hz); C3 (Do) (130.8 Hz); and D3 (Re) (146.8 Hz)) corresponding to different string tension forces were set up in the simulation study. The boundary condition was set up by considering the real-life environment. In the context of the musical instrument, the strings are fastened between a string holder (string tie) on the soundbox and the pegs. These pegs apply tension to their corresponding strings during the tuning process. To replicate this scenario, the instrument was fixed from the string holder (string tie) and the nut. Subsequently, the pre-calculated string tension forces for each string bearing on the bridge were separately applied, including the standard earth gravity effect (9.81 m s\({}^{-2}\)). Realistic contact conditions were also considered between the parts. Frictional contact definitions were assigned between the bridge and the soundboard, and the friction coefficient between these components was assigned as 0.25 [29]. The contacts between the other components were defined as bonded contact, as it was utilised in the instrument making. The literature on non-linear FEM-based analyses explores non-linearity in three main categories: boundary conditions (contact) nonlinearity, material nonlinearity, and geometry non-linearity. This FEA study focuses on boundary conditions, specifically the non-linearities arising from geometry and contact [30; 31]. The FE model (mesh structure) was constructed using the FEA code's meshing functions. To ensure accurate results, curvature-based meshing approaches were employed, and smaller element sizes were assigned to specific components such as the string holder, bridge, and head nut. The appropriate element size for the FE model was determined via pre-trials. To assess the accuracy of the FE model and to make internal verification, a skewness metric was employed, which measures the deviation of the elements from equilateral cells. A skewness value of 0 indicates perfect cell quality, while a value of 1 indicates fully degenerated cells (0: equilateral; >0-0.25: excellent; 0.25-0.50: good; 0.50-0.75: fair; 0.75-0.9: poor; 0.9-<1: bad; 1: degenerate) [32; 33]. The FE model had an average skewness metric value of 0.241, which is considered excellent cell quality. The instrument consists of various components made from different materials. The materials utilised for the instrument components were separately assigned. Most importantly, wood-based materials exhibit anisotropic material behaviour because of the nature of their inner structure, and this may result in some limitations such as converging problems, increasing solving time, etc., in engineering simulation studies. Therefore, some assumptions are inevitable. In this regard, the critical components, such as the soundboard and neck, were defined using a homogeneous linear orthotropic material model, which takes into account their susceptibility to deformation. The remaining components were assumed to be made of homogeneous linear isotropic material [34; 35; 36; 37; 38; 39; 40; 41]. The material properties assigned to the instrument's components in the analysis setup are given in Table 2. The description of the boundary conditions, including forces acting on the bridge, and visual and numerical details of the FE model are given in Figure 3, Table 3, and Figure 4, respectively. Figure 3: Boundary condition.