## 2 Materials and Methods
### FEM Model  
The geometric conditions of the applied forces are, as far as possible, the same in experimental studies as in numerical analyses. Polypropylene was selected as the material of the exterior body (\(E\) = 1000 MPa, \(v\) = 0.2) [13; 14]. The inner layer was modelled with soft foam (\(E\) = 100 MPa, \(v\) = 0.45) [14]. The 10-node tetrahedral element (SOLID187) was used to generate the FEM model. A relatively fine tetrahedral FE mesh (Figure 5a) was generated to demonstrate in detail the values and the distribution of directions of the principal stress vectors in each element separately. The tetrahedral shapes appear fairly regular, in spite of the complicated geometry of the orthoses. The mesh was also made more dense at critical locations with more complicated geometries to increase the accuracy of the calculation of the stresses arising during orthosis loading at these locations. Discretisation was carried out until further densification of the mesh of nodes did not change the resulting von Mises stress by over 3% [23]. Once concentration of the mesh was achieved, 199,187 nodes and 104,742 FE were obtained with a maximum edge dimension of 8.0 mm (Figure 5a). A relatively fine mesh of tetrahedral finite elements (Figure 4a) was generated in order to show in detail the distribution of directions and values of the principal stress vectors, shown after solving the problem in each element separately. The shapes of the tetrahedrons appear quite regular, despite the complex geometry of the brace. After generation of the FE mesh and definition of the brace model's parameters, the boundary conditions that were applied in the experimental tests conducted as part of this research were introduced (Figure 5b). The three-point system of forces was implemented through the application of supports \(B\) and \(C\) and pre-loading force \(A\) (Figure 5b). Two immobile supports were set, defined as small surfaces \(B\) and \(C\), immobilised in space. Preliminary loading of the brace was implemented as the application of load \(A\), with a value of 36.25 N. The load of force A fits within the range of actual forces found in orthoses [24]. The application of the preliminary load was indispensable for stabilising the brace's position on the experimental test stand, which is described in Test stand for experimental verification of FEM results section. The orthosis immobilised in this way is also affected by the gravitational force \(E\). To best represent the real conditions of the experiment, the gravitational force is included, although it does not appear to play much of a role. The displacement field has been calculated with the loads and supports thus defined. After performing the first step of the calculation as previously described, an extra force \(D\) of 0.1 N, corresponding to the experimental conditions, was added to the brace in the direction of the applied force \(A\). The application of a secondary force, low in value, corresponded to the conditions of the experiment, based on determining the field of small displacements for the brace, measured by an interferometer with a narrow measuring  
Figure 5: Numerical orthosis model: (**a**) tetrahedral FE mesh generated, (**b**) boundary conditions applied to the geometric model that has been imported; mathematical description (NURBS): \(A\)—pre-loading force corresponding to the action of the torso on the brace, \(B\) and \(C\)—fixed supports, \(D\)—additional force added after pre-loading of the orthosis, \(E\)—gravitational force. range. As shown later in the paper, the orthosis's material operates in a linear range for typically applied loads acting on the orthoses. Thus test results of small displacements at low loads can be related linearly to findings corresponding to higher operating brace loads. The final simulation result was obtained by calculating the displacement difference prior to and after the introduction of force \(D\).