## 2 Materials and Methods
### Finite Element Analysis
#### 2.1.1 CAD and FEM Model  
The used CAD model obtained from a 3D scan and the bone model used in the experiment are not 100% identical; nevertheless, they are sufficiently similar to allow experimental verification of the calculation results; see Figure 6. The model of the whole bone is not necessary for our purposes and, for this reason, only the proximal part of the tibia was used in this calculation. This proximal part was then \"cut\" in two at the site of the epiphyseal plate. The staples were virtually placed in the bone in the way they usually are during epipbysidesis, i.e., in the general area bridging the physics.  
The CAD model of staple provided by MEDIN a.s. contains notches, which are not suitable for FEA. For this reason, sharp edges were rounded; see Figure 7. However, these sharp edges are important for properly inserting the staple in a bone.  
Figure 6: 3D CAD model of the bone and staples with main dimensions (mm).  
Figure 7: 3D CAD model of the staple with rounded sharp edges (mm).  
The radius size of 0.25 mm, according to Figure 7, is quite small, because this part of the staple is relatively thin, and using bigger radius size (e.g., 0.5 mm) would result in near complete removal of this part.  
In this paper, we used only the bone model and staples for FEA. The reason for this acceptable simplification lies in the fact that the limb growth is primarily determined by the bone (or, more accurately, epiphyseal plate). The bone is intact (i.e., without fracture); therefore, the influence of the muscles, ligaments, menisci, and synoxia on bone growth is negligible compared to the load on the bone.  
Muscles, ligaments, menisci, and synoxia could play a small role in restricting the staple migration, but this effect is not noticeable in our study and hence is considered negligible. Thus, muscle and other tissues and fluids were omitted in this paper.  
The influence of anatomical parts in cavitas articularis (i.e., mentioned muscles, ligaments, menisci, and synoxia) might play significant role in ambulation of patients with Blount staples, see [23].  
The transformation of the CAD model into the FEM model is presented in Figure 8. Considering the complexity of the bone shape, the tibia was discretized by tetrahedral elements (SOLID187 in Ansys sw) with a global maximum size of 2.5 mm. The element size in holes for staples was locally refined to mirror the element size of the staples. In addition, a refinement to 0.5 mm was performed in a small circular area in the immediate vicinity of holes for staples. The global element size is relatively large as we are focusing on and evaluating only the staple response, not that of the bone. The _corticalis_ and _spongiosis_ FE meshes are continuously connected by nodes and elements sharing faces (i.e., conformal mesh achieved by shared topology function in Ansys SpaceClaim sw), see [21].  
Staples were discretized by a hex-dominant mesh (SOLID186 + some SOLID187 elements) with a global maximum element size of 0.5 mm. The element size was locally refined on radii and in the immediate vicinity of these areas; see Figure 9.  
The presented mesh in its final form was used for the final calculation and result evaluation. The sensitivity analysis started with a coarse mesh, and after each computation, a new, refined, mesh with half the element size of the previous mesh was created. This process was repeated until results for two different meshes were close (within a 1% margin of error); in this way, the mesh sensitivity analysis was performed.  
Additional information about FE mesh regarding the number of elements and nodes is presented in Table 2.  
Figure 8: FEM model of the bone and staples.