## 3 Finite-Element Modeling (FE) and Validating  
In the modeling process, ABAQUS was used. During the modeling, the program automatically generates a Python script for the given modeling task, which contains the steps required to complete the work. The goal of the modeling was to create a model that allows for extensive modifications and enables the examination of the questions presented in the literature review. In traditional methods, for example, relocating a stud, results in a considerable amount of modeling work (even 1-2 days), as this requires changes not only in the assembly module but also in the concrete geometry, since a hole must be created in the concrete where the stud is located. When such a change is made, it essentially requires restarting every step, such as geometry, assembly, loading, steps, interactions, and mesh. In such a complex model, manually modifying these kinds of changes can introduce many errors into the model. For this reason, other studies typically created only a few types of models and limited their examination to the effects of certain parameters. Our model was designed in such a way that the Python script generated during the design process can be easily modified and parameterized. In other words, a single change automatically updates the necessary model settings, ensuring that the model remains consistent in all aspects (e.g., mesh). Essentially, we have created a model in which any parameter can be simulated, such as stud placement, reinforcement bar locations, geometry, and materials. The finite-element modeling approach integrated advanced features, including the consideration of geometric nonlinearity and the application of a Concrete Damage Plasticity  
Figure 2: Laboratory experiment setup. (CDP) model to accurately represent the behavior of concrete. These methods allow for the accurate modeling of the behavior of complex structures--such as this steel-concrete composite connection--focusing on stress conditions, deformations, and failure modes. The steel stud was simulated using a bilinear isotropic hardening model, which is governed by the [PERSON] yield criterion. The interaction between steel and concrete is modeled using the Coulomb friction approach to observe sliding and separation at the interfaces. Geometric nonlinearity is utilized to account for deformation, buckling, and bending effects. The push-out specimen consists of four parts, as shown in Figure 3: steel girder, concrete, steel studs, and steel reinforcement. The concrete slab, steel studs, and steel components were represented using the C3 DRR solid element from the ABAQUS 6.25 software library. This element is an eight-node brick configuration with reduced integration stiffness, which has been widely validated for modeling concrete behavior under intricate stress states [39]. The C3D8R element is used for performing nonlinear analysis, which includes modeling contact interactions, large deformations, plasticity, and failure mechanisms. Each node in the element has three translational degrees of freedom (DOFs). The steel studs and girder were modeled separately and meshed together using the C3D8R solid element [40]. To model the reinforcement bars, a 3D beam element, specifically the 2-node linear beam in space (B31: Timoshenko beam), was used. An embedded region constraint was applied to simulate the bond between the longitudinal and transverse reinforcements and the surrounding concrete, ensuring accurate force transfer and interaction between the reinforcements and the concrete matrix. Boundary conditions were imposed in accordance with the experimental constraints. The model shown in Figure 1 was constructed by systematically assembling and precisely positioning the components. A mesh sensitivity analysis was conducted to evaluate the impact of mesh size on both computational accuracy and time efficiency. The results of mesh sensitivity analysis indicated the utilization of a finer mesh size at locations where high stresses were expected.