## 4 Numerical Simulation
### Numerical Simulation of Singular Finite Element  
Initially, to verify the accuracy of the analytical model in FE simulations, a single 8-noded cubical-shaped C3D8R element measuring 1 mm\({}^{3}\) was modeled, and suitable boundary conditions were applied to simulate biaxial symmetry in the two axes perpendicular to the loading direction. To maintain a stress triaxiality ratio \(\eta^{*}\) of 0.333 throughout the tensile test, the bottom four nodes were restrained in the direction of applied force, and four nodes on each of the two faces perpendicular to the loading axis had their movement in the two orthogonal axes restrained, respectively, as can be seen in Figure 13a. The top four nodes were free to move in the direction of loading, and to achieve that a velocity-based loading condition was applied.  
Similarly to the experimental procedure, loading speeds of 0.1-200 mm/s were applied to the top four nodes simultaneously. To reduce inertia-related effects at the beginning of the simulation, velocity amplitude was smoothly applied to the simulation for the first 1/10 th of the overall step's duration and then kept constant until the completion of each test (Figure 13b). Duration of the tensile phase of the simulation was adjusted each time according to the required strain rate in order to allow for sufficient simulation time and up until the complete damage being registered at the tested element.  
In Abaqus, several ductile material models are available that can accurately capture the deformation of steel materials, but in this work, the JC flow stress model and, correspondingly, the JC damage model was utilized using material parameters that were calculated in previous sections. Along with the data presented in Tables 3 and 4, for this material, according to the manufacturer's specifications, [PERSON]'s Modulus \(E=210\) GPa and Poisson's ratio of \(\
u=0.28\), and furthermore, the density was set as \(\rho=7.85E-09\) tonnes/mm\({}^{3}\).  
In Figure 14, a comparison between the experimental true stress-strain curves for different strain rates of Table 2 with the results obtained from a singular finite element are presented. Overall, good accuracy was achieved between experimental and numerical results with the exception of 1 s\({}^{-1}\) strain rate results in which although the failure strain was similar, the ultimate stress value had a difference of approximately 8%. It is believed that this is due to the non-monotonic nature of failure strain as well as ultimate stress that was observed during the experimental procedure (Figure 6b).  
To accurately model the material softening behavior past the damage initiation point [27] represented in Figure 15a, in which \(\sigma_{\text{30}}\) is the yield stress, \(\bar{\varepsilon}_{0}^{pl}\) is the equivalent plastic strain at the damage initiation point, and \(\bar{\varepsilon}_{f}^{pl}\) is the equivalent plastic strain at failure when the scalar damage parameter \(D=1\) (Equation (8)), damage and strain are correlated. For modeling of post-damage-initiation softening until element failure data, post-peak stress \(\sigma_{D}\) is calculated based on the difference between experimental and JC analytical prediction (Figure 10). Based on the difference between relevant stress value \(\sigma_{D}\) and from Equation (9), sets of \(D-\varepsilon\) were calculated. Their respective correlation is presented in Figure 15b, showing the correlation between damage parameter and equivalent plastic strain used to model softening behavior of the material in this work under reference conditions.  
Figure 13: (**a**) Singular element’s boundary conditions used in FE simulation; (**b**) smooth piecewise application of velocity amplitude.