## 2 Methods and Materials
### Numerical Investigations  
The experimentally obtained load-deflection curves were recalculated with the Finite-Element Method (FEM) by using the software Ansys [21]. To get the most realistic results, geometrically nonlinear simulations were performed, including the measured imperfections from Table 2 (GNIA). First, the perfect geometry was generated and meshed. Then, the imperfections were created by moving the nodes of the mesh. This was done by using the programming capabilities of the used software. In doing so, a stress-free but imperfect mesh was created. The whole system was discretized with volume elements SOLID 185, using enhanced strain and mixed u-P formulations. This also corresponds to the recommendations in the ANSYS Helpfile [21] for such problems. In order to realize the most realistic stresses, all boundary conditions, including the real POM-C layers, were taken into account. The steel parts at the support are much stiffer than the POM-C layers and could be assumed as rigid. Therefore, and to reduce the size of the FE-mesh, these parts were not modeled. Instead, the corresponding degrees of freedom of the POM-C layers (corresponding displacements v and w) were fixed. For numerical reasons, some vertexes of the POM-C layers were also fixed in the \(x\)-direction, but this does not influence the results. Each contact between the POM-C layers and the glass beam were realized with a frictionless contact behavior. This approach seemed to be sufficient because the glass beam was supported in all directions by POM-C layers, so no relevant relative displacements between the glass and the POM-C layers could occur. Therefore, also the influence of friction between the glass and the POM-C layers seemed to be negligibly low. Due to the clamping at the support and the precisely fitting POM-C layers, no gaps occurred in the experiments; therefore, the contacts were also modeled without any gaps. The real loading situation was considered with a simplified geometry, which means that the real joint was modeled as an ideal universal joint between the two steel plates. The FE-model, including the mesh and the boundary conditions, can be seen from Figure 3. In order to guarantee mesh-free results, studies on different mesh sizes, as well as different time size settings and also comparative calculations with another element type (SOLID 186), were performed (details can be found in [22]). Figure 2: Testing device and procedure exemplary for a fully tempered (FT) glass panel: (**a**) Failure of the first glass panel, (**b**) total failure of all three panels. A linear-elastic material behavior was assumed for all parts. The used material parameters (elastic-modulus E and Poisson's ratio \(\
u\)) are given in Table 3. A special problem was the considerations of the creep behavior of the PVB-interlayer. There can be found different databases in the literature on the value of the shear modulus (a summary is given in [23]). Most of the values were obtained from small test specimens. The values given in [11] were determined from larger test specimens, which seems to provide the most realistic results. Therefore, this database was used for the recalculations. Figure 4 (taken from [11]) shows the creep behavior of PVB-foils over time. Depending on the real loading duration from Tables 5 and 6, the shear modulus was calculated for each test. The shear modulus has a strong influence on the structural behavior of the system. Due to the large relative deviations of the shear-modulus (see Figure 4), all calculations were carried out with two different values. Firstly, the minimum shear modulus \(\mathrm{G_{min}}\) from the formula for the lower limit given in Figure 4 was used. The calculated values are all in a range of \(\mathrm{G_{min}}=0.32\)-\(0.35\) MPa, due to the similar loading durations. The formula for the upper limit given in Figure 4 seemed to be very high (maybe outliers). Therefore, an approximated mean value of \(\mathrm{G_{mean}}=0.70\) MPa was used for further comparisons.