## 3 Finite-Element Modeling (FE) and Validating
At the applied mesh refinement level, the structural behavior could already be observed with high precision, and further refinements would not significantly alter the response but would considerably increase computation time. Finer meshes were employed in areas expected to experience high stress, ensuring greater precision in the results. Areas with significant expected deformations, such as the loaded steel girder, were also refined with finer meshes. As illustrated in Figure 3d, the stud and its adjacent concrete region were assigned the finest mesh. In the concrete, a more refined mesh was applied near the shank of the stud, extending to its endpoint. The finite-element boundaries along the stud and surrounding concrete were aligned to ensure convergence and accuracy in the simulation. Meticulous attention was given to maintaining complete symmetry of the mesh throughout the specimen. Appropriate separations and sets were used to create the most accurate mesh possible. The model's mesh comprised roughly 867.012 variables in total. Figure 4 illustrates the interactions within the FE model. The model exhibited high accuracy in effectively simulating the contact behaviors. A surface-to-surface interaction was modeled, with the tangential behavior governed by a penalty friction formulation. Hard contact with a friction coefficient of 0.2 was defined for the interface between the shank of the steel stud and the concrete component. Furthermore, hard contact with a friction coefficient of 0.3 was applied at the interface between the steel and concrete, in accordance with relevant literature [41; 42; 43] and prior empirical observation [44]. Additionally, [PERSON] et al. [38] calibrated and validated their numerical model in their research, using iterations of the same friction coefficient values between the steel girder-concrete deck slab and the concrete deck slab-steel stud connections. [PERSON] et al. [45] examined the variation in Coulomb friction parameters under high-temperature conditions, taking into account the complex interaction between steel and concrete. This numerical model is applicable solely  
to ambient temperature, as high-temperature effects are not considered in the analysis. However, all structures must be evaluated under both ambient and high-temperature conditions, where adjustments to the applied parameters, including Coulomb friction parameters, may be required. Figure 3: Details of the FE model and the meshing: (**a**) steel stud; (**b**) reinforcement; (**c**) concrete block; (**d**) details of the stud and surrounding concrete; (**e**) steel beam; (**f**) full of the FE model. During the modeling process, Newton-Raphson iteration was applied using a displacement-controlled approach, with nonlinear analysis and a nonlinear material model. External loads were applied through imposed displacements corresponding to the experimental test setup. Figure 5 presents the load and boundary conditions utilized in the FE model, which are identical to those implemented in the experimental test. The concrete part at the bottom were set as fixed. The compressive properties of concrete are presented in Figure 6, while the tensile properties are shown in Figure 7, both of which were utilized in the modeling process. The concrete damage plasticity (CDP) model is commonly used in finite-element (FE) modeling to accurately describe the nonlinear behavior of concrete, incorporating plastic deformation and damage under various stress conditions. The concrete damage plasticity model used in the current simulation is characterized by the following parameters: [PERSON]'s ratio of \(v\) = 0.2, [PERSON]'s modulus of \(E_{0}\) = 35,000 N/mm\({}^{2}\), dilation angle of 33\({}^{\circ}\), an eccentricity value of 0.1, a f\({}_{00}\)/f\({}_{00}\) ratio of 1.12, and a viscosity parameter (\(K\)) of 0.667. Figure 4: Interactions of the FE model. Figure 5: Load and boundary conditions of the model.