# Localized Necking Model for Punching Fracture Simulation in Unstiffened and Stiffened Panels
## 4 Validation of Fracture Model
### Numerical Simulation  
The numerical simulations for the punching tests were carried out using Abaqus/ Explicit with user-defined material subroutines VUMAT for the HC-DSSE model. The effective parts of the punching test specimens were meshed with four-node reduced integration shell elements (S4R in the Abaqus element library), while the indenter was modeled with a rigid element (R3D4 in the Abaqus element library) and located at the specimen center. The general contact option in Abaqus/Explicit was adopted to define the contact between the indenter and specimen, including the friction property, and the friction coefficient was set as 0.23. Abaqus uses five integration points through the thickness of an S4R by default. The first section point is located at the bottom surface of the shell element, and the five-section point refers to the top surface. The damage indicator must be calculated at all the integration points. Subroutine vumatXtrArg with a user-defined material subroutine VUMAT was used to control the state variables in each through-thickness integration point. An element is deleted when one in five thickness integration points meets the condition \(D_{DSSE}\geq 1.0\) or \(D_{HC}\geq 1.0\).  
A uniformly sized element with four different element lengths (\(l_{e}=2.5\) mm, 5.0 mm, and 10.0 mm) were used in the finite element models. The FE model was only generated in the effective parts (600.0 mm \(\times\) 600.0 mm). Figure 14 shows the FE models of all the specimens and the number of nodes and elements. The boundary condition of fully clamping the edge was used. The mass scaling option was used to decrease the computational cost, and the total simulation time was 0.4 s, which was long enough to neglect the dynamic effect.  
Figure 12: Dimensions of the specimens and indenter (unit: mm).  
Figure 13: Images of the punching test specimens.  
cases, the fracture simulation with a mesh size of approximately 2.5 times the thickness of the plate (1.9 mm) most accurately predicted fracture initiation from the experiments.  
Figure 16 shows a comparison of the experimental post-fracture shape and numerical simulation \((l_{e}=5.0\) mm). Table 4 presents the experimental and simulated dimensions of the failure surface for an element length = 5.0 mm. It is confirmed that the presented  
\begin{table}
\begin{tabular}{c c c c c c c} \hline \hline  & **Case** & & \(\mathbf{d_{f}}\)**(mm)** & **Error (\%)** & \(\mathbf{F_{max}}\)**(kN)** & **Error (\%)** \\ \hline \multirow{4}{*}{\
\begin{tabular}{c} Unstiffened \\ panel \\ \end{tabular} } & Test & 72.4 & - & 82.8 & - \\  & \(l_{e}=2.5\) & 65.9 & 9.0 & 81.2 & 1.93 \\  & \(l_{e}=5.0\) & 69.1 & 4.6 & 82.6 & 0.24 \\  & \(l_{e}=10.0\) & 86.1 & 18.9 & 103.1 & 24.5 \\ \hline \multirow{4}{*}{
\begin{tabular}{c} Stiffened \\ panel \\ \end{tabular} } & Test & 71.9 & - & 97.6 & - \\  & \(l_{e}=2.5\) & 94.5 & 31.4 & 84.1 & 13.8 \\  & \(l_{e}=5.0\) & 74.1 & 3.06 & 98.2 & 0.6 \\  & \(l_{e}=10.0\) & 81.3 & 13.07 & 107.6 & 10.25 \\ \hline \hline \end{tabular}
\end{table}
Table 3: Comparison of maximum force and displacement at fracture between experimental and numerical results.  
Figure 15: Comparison of numerical results with the test results.  
fracture model with shell elements has an effective predictive capability of not only fracture initiation but also the shape of the fracture surface.