## 3 Results  
The calculations of the detailed sandwich panel were taken from [63]. The following data was adopted for the calculations: \(l_{x}=300\) cm, \(l_{y}=180\) cm, \(\delta=5\) cm, \(2\)h = 8 cm, \(E=2.6\cdot 10^{4}\ \mathrm{MN/m^{2}}\), \(G_{w}=3\ \mathrm{MN/m^{2}}\). The load was assumed as evenly distributed with a value of \(q=10\ \mathrm{kN/m^{2}}\). For a better image, the above parameters are shown in Tables 1 and 2. Figure 2 shows the markings, the adopted partition grid, and the boundary conditions for the analyzed slab. \begin{table}
\begin{tabular}{c c c c} \hline \(l_{x}\) & \(l_{y}\) & \(\delta\) & \(2h\) & \(q\) \\ (cm) & (cm) & (cm) & (cm) & (kN/m\({}^{2}\)) \\ \hline
300 & 180 & 5 & 8 & 10 \\ \hline \end{tabular}
\end{table} 
Table 1: Geometric dimensions of the sandwich panel and applied external loads. \begin{table}
\begin{tabular}{c c c c} \hline \hline  & \(E\) & \(G_{w}\) & \(\boldsymbol{v}\) \\  & **(MN/m\({}^{2}\))** & **(MN/m\({}^{2}\))** & **(\(-\))** \\ \hline External layers & \(2.6\times 10^{4}\) & \(4.33\times 10^{3}\) & 0.2 \\ \hline Middle core & 6 & 3 & 0 \\ \hline \end{tabular}
\end{table} 
Table 2: Material parameters of the external layers and middle core. Using the described method of finite differences (Equations (4)-(6)), a global matrix was built to determine the displacements. A rectangular slab, simply supported on two opposite edges and two free edges, with a cut in one of the free edges, was taken as an example of a slab. Earlier, the paper described the boundary conditions for the free edge (Equations (7)-(17)) adopted for the calculations. After using the symmetry of the plate, a system of equations with 110 unknowns was obtained to solve. In order to calculate the reference deflections, several three-dimensional models of the sandwich panel were created, defining the cross-section and material properties in different ways. Commercial FE software (ABAQUS FEA) was used for calculations. The results obtained from the 3D model were compared with the results obtained in an analytical manner and with the method of numerical homogenization. A multi-layer slab with the dimensions shown in Figure 2 was modeled as a freely supported slab. The slab consisted of concrete external cladding and a foam core. The material parameters were adopted as in the analytical approach. Boundary conditions in both 3D numerical models of a simply supported type were applied at two opposite shorter sides. The slab was loaded with a load evenly distributed over the entire surface of the slab, with a value of 10 kN/m\({}^{2}\) (the same as the plate shown in Figure 2). The first model (Model 1) is a full 3D model of the plate. Its height was modeled as 18 cm and then divided into 3 parts with appropriate layer heights, i.e., 5 cm, 8 cm, and 5 cm, using partition cells. The model discretized 3D solid elements of C3D20R (20-node brick elements with three degrees of freedom in each node with a reduced integration scheme) with dimensions of 300 mm in the plane and seven elements in thickness. The second model (Model 2) was created from a combination of 3D solids and skins. The concrete surface layers were modeled as skin and the foam core as a 3D solid structure. The core was divided into solid C3D20R elements, and skins into shell elements S4R (4-node general shell with reduced integration) with dimensions of 300 mm in the plane. The third model (called Model 3) was created analogously to Model 1. The only difference was the discretization of the model; elements of the CSS8 (continuum solid shell elements) type were used here. Another model of the plate (Model 4) was modeled as a shell element with external dimensions as given earlier. The material properties were assigned using a composite section, and the plate was meshed with S8R elements (8-node shell elements with reduced integration scheme). In order to perform numerical homogenization, it was necessary to correctly define the stiffness matrix of a representative volume element (RVE).