## 2 Materials
### Finite Element Modelling  
In this step, the edited STL files were exported to Hypermesh (Altair, Troy, MI, USA) for mesh generation. When considering the types of elements to use when meshing the cervical spine, two are generally preferred, namely, tetrahedral and hexahedral elements. The first type facilitate mesh generation on the vertebrae's curved surfaces, but are limited by the fact that they are more computationally expensive and can be excessively stiff [21]. Hexahedral elements are generally preferred for 3D nonlinear analysis. However, they require more time during mesh generation, and if the surface smoothing is not performed proficiently it may cause edge discontinuities. Because hexahedral elements can be beneficial if properly meshed, they were used to mesh most of the cervical components. When generating the mesh, two parameters were taken into consideration: the desired element size and the minimum Jacobian. The desired element size for the vertebrae was set to 0.6 mm, while the intervertebral discs were set to 0.5 mm. Different element sizes were tested; the values selected guaranteed the best convergence without compromising the overall CPU cost in subsequent simulations. The minimum Jacobian was set to 0.3 in all the components in order to ensure acceptable element aspect ratios. Afterwards, the vertebrae were separated into two types of bones, namely, cortical and cancellous. In this work, the posterior elements of the vertebrae, for example, the spinous process, were not considered to be different types of bones and were not modelled as such [12; 22]. The cortical bone, as the outer layers of the mesh on the vertebrae, was considered to achieve a thickness of approximately 0.5 mm, the average thickness found in the literature [23]. The intervertebral discs were separated according to their different type of materials, these being the AF ground substance, the nucleus pulposus, and the cartilaginous endplates. It was decided that the AF fibers would not be included in order to simplify the first simulations of the cervical FEM [16; 24; 25]. The endplates were modeled as the top and bottom layers of the intervertebral disc. The rest of the disc was divided into AF grounds (60%) and nucleus pulposus (40%) [16]. The next step was the formulation of the facet joint. These were modeled by assigning contact integration properties to the superior and inferior articular cartilages. The cartilage geometry was generated based on anatomical descriptions from the literature [26] and on the superior and inferior articular process surfaces (for the inferior and superior cartilages, respectively) of each corresponding vertebrae. Most components were modeled with eight-node brick elements with reduced integration (C3D8R) with the exception of the facet cartilage, which was modeled with general purpose linear brick elements (C3D8), and the nucleus pulposus, where hybrid reduced integration hexahedral elements (C3D8 RH) were used. In the first case reduced integration elements could not be used, as they perform poorly during contact, and the general-purpose elements showed the best results when simulating, while in the second case the hybrid formulation was used, because the software can only represent incompressible materials using these elements. Figure 1 shows a summary of the methodology used to create the geometry and mesh of the cervical spine model. Functional Spinal Unit Model  
Considering that the complete model (without the ligaments) consisted of 655,924 elements and 740,471 nodes, a full simulation would take a significant amount of time. As seen in previous studies, it is possible to first analyze a section of the spine before simulating the entire model, or even to simulate the entire model by dividing it into segments. [PERSON] et al. [10] created a complete model of the lower cervical spine (LCS) while first testing a reduced FSU comprised of the C4-C5 segment before simulating the complete model. [PERSON] et al.