## 2 Materials and Methods
To enhance FEM accuracy, local mesh refinement was introduced in high-stress regions. A minimum of two elements per section thickness is required for reliable FEM analysis; in this case, at least three finite elements per implant wall thickness and five per bone fixation plate thickness were achieved, ensuring an adequately refined mesh for precise results and accurate stress-strain calculations. The element statistics option in ANSYS was used to provide detailed information on the types of elements applied (Figure 5). The final implant mesh contained 531,644 nodes and 338,239 tetrahedral elements. A non-coherent mesh interface was used between the implant wall and bone fixation plates due to their complex geometry. Attempts to create a node-to-node connection failed due to the intricate implant and plate shapes. Non-coherent connections allow load transfer, though local finite element artifacts at interface boundaries should be disregarded, similar to sharp edges or nodes on material interfaces [8]. FEM simulations were conducted in ANSYS within the linear elasticity range on an available computer with average computational power, equipped with a 3.0 GHz processor and 32 GB RAM. The calculations were divided into two threads to enhance performance. The linear behavior was applied to both materials and contact conditions, which were considered either as non-existent or as a bonded condition between the implant and the bone. The evaluation criterion was the stress in the titanium implant during the transmission of the same bite force in terms of direction and magnitude, caused by muscle activities tested in the pilot study. In the assessment, the criterion of equivalent stress according to the maximum distortional strain energy density (based on [PERSON]'s theory) was applied. Principal maximum and minimum stresses were also presented to better understand whether, in critical areas, the equivalent stress arises from a single dominant stress component or from the difference between tensile and compressive stresses. The following material parameters were adopted for the mandible:  
* Cortical bone: [PERSON]'s modulus E = 14,000 MPa, Poisson's ratio \(\
u\) = 0.3;
* Cancellous bone: E = 500 MPa, \(\
u\) = 0.33 [9; 10]. Numerical studies were conducted for four variants of load transfer and implant fixation with the mandibular stumps:  
* The first variant assumed osseointegration at the interface between the implant and the bone stump for a model supported in both joints (Figure 4g);
* The second variant assumed osseointegration at the interface between the implant and the bone stump for a model supported in one joint on the side opposite to the occlusal load (Figure 4f);
* The third variant assumed no osseointegration and connection exclusively through anchoring screws for a model supported in both joints (Figure 4g);
* The fourth variant assumed no osseointegration and connection exclusively through anchoring screws for a model supported on one side in the joint opposite to the occlusal load (Figure 4f). The study of ideal osseointegration aimed to determine whether the assumption of bilateral joint support or optimistic osseointegration has a greater impact on the results.