## 2 Materials and Methods
### Finite Element Method  
FE Analysis was performed using an explicit thermal and mechanical solver in the commercial LS DYNA software. The flow behavior of the material is modeled via the classical *MAT_024_PIECEWISE_LINEAR_PLASTICITY model [23] using different flow curves in order to consider strain-rate-dependency. The flow curves used for the simulation are shown in Figure 10. Damage and failure strain rate effects are considered via the GISSMO damage and failure model developed by [PERSON] et al. [24]. This model combines the damage description, which is used to calculate the crash simulations, and an incremental formulation for the description of the material instability and localization. It is implemented in LS-DYNA by keyword *MAT_ADD_EROSION and enabled by setting IDAM = 1, the functions \(\varepsilon_{f}(\eta)\), \(\varepsilon_{kit}(\eta)\), and \(\alpha(L_{e})\) are defined as input parameters by keyword *DEFINE_CURVE and the parameters n and m are defined directly on the material card. The fracture parameters listed above were revealed by a combination of experimental studies of different sample geometries (in order to cover different triaxial states) and inverse modeling performed in LS-OPT. In more detail, these calculations are given in [15] but the basic fracture curves as well as the m and n parameters are presented in Figure 4.  
Figure 2: Experiment setup including high-speed thermal camera and pyrometer. The consideration of the nonlinearity of the strain path for the GISSMO model can be based on the fact that the damage is quantitatively accumulated stepwise for each change in the strain path [25]. The main focus of this study is the plastic component of the existing material model, namely, expanding it by adding yield curves for different strain rates. The input parameters used in the simulation were the data obtained experimentally, namely, the path of the traverse during the tests and the distance between the markers, which was measured with an extensometer. The experimentally determined input parameters for the simulation, in the form of the traverse displacement, are shown in Figure 5.  
The simulations of the specimen tests were performed with fully integrated solid elements (ELFORM 2) with edge lengths of 0.5 \(\times\) 0.5 \(\times\) 0.1 mm and LS-DYNA R12.0.0. The geometry with dimensions of the sample used for simulation is shown in Figure 1. The choice of this finite element mesh size was justified by the fact that, even in preliminary work, this ratio allowed to obtain the best results for the fracture model in relation to the temperature distribution. In addition, the most exact comparability for the GISSMO fracture model is optimized for these element sizes in the previous work [15]. The used model included 30810 elements. One of the edges of the sample was fixed in place using the *BOUNDARY_SPC_SET* command and the other side was given an experimental  
Figure 4: Damage parameters (failure strain). Figure 3: Experimental setup of temperature measurement with a pyrometer. (**a**) before the test and (**b**) after the test. motion using *BOUNDARY_PRESCRIBED_MOTION_SET* obtained from the traverse of the high-speed testing machine as shown in Figure 6a. In order to provide good comparability of the measured and the numerically determined data, the determination of the change in the parameter, l\({}_{0}\), in the sample was carried out similar to the measurement principle of the extensometer. As shown in Figure 6b, the elongation of the sample was evaluated by tracking the displacement of two points in the center of the sample, using the *HISTORY_NODE*. The temperature distribution is calculated via the dissipated forming energy according to Equation (2) based on the temperature increase, \(\Delta\vartheta\), the specific heat capacity, \(c_{\vartheta}\), the Taylor-Quinney factor, \(\kappa\)[26], and the forming work performed, \(\Delta W_{\text{dis}}\). The Taylor-Quinney factor is used to define the fraction of plastic stress power that is not converted into heat.