# Global Buckling Resistance of Cold-Formed Steel Beams with Omega-Shaped Sections
## 4 Numerical Models
### Development and Validation of the ABAQUS Model  
The omega-shape profiles were simulated using a shell model, using the SR8 reduced integration finite element type available in ABAQUS, representing the mid-surface of the profile's geometry. The length of the profile was generated by applying the extrusion command. The holes that exist along the profiles, whether circular or oval-shaped, were also included in the model. In the material characterization, yield, and ultimate stresses, as well as the ultimate strain of the material, were considered. The simulation of the material's non-linear behavior used stress-strain curves defined by the Ramberg-Osgood model [26]. All the other components that were used in the model were simulated with solid parts made to replicate the laboratory setup (Figure 9). The material for these parts was assumed to be linear elastic. The modeling of the loading and boundary conditions for the two layouts used in the experimental campaign is detailed in [27]. The contact between the neoprene bands that were placed between the omega profiles and the other test setup parts was modeled using General Contact with a friction coefficient of 0.35, representing the friction between steel and rubber. Initially, the friction coefficient specified in the American standard ANSI AISC 360-22 [28], set at 0.30, was used, which represents the friction coefficient for steel surfaces free of oil, grease, or painting. Subsequently, the value established in the Brazilian standard ABNT NBR 8800:2008 [29] for the same steel surfaces, set at 0.35, was adopted. The use of this latter value resulted in greater consistency between the numerical results and those obtained experimentally. The loading was applied to accurately replicate the experimental tests. To simulate the hydraulic actuator used in the experiments, the load was applied at a single point. Subsequently, it was evenly distributed onto the four loading plates using a coupling-structural-uniform restriction (see Figure 10). The contact plates were steel plates with the dimensions of 15 cm \(\times\) 10 cm \(\times\) 1 cm, as described in Section 3.2 (Test setup). The boundary conditions vary depending on the profile size. For larger sections, it is necessary to model the cylinders to account for local deformation occurring at the supports. The cylinders modeled to simulate the supports are steel elements with a 2 cm radius and 30 cm length. In the case of smaller profiles, restraints are applied at four points, corresponding to the contacts with the supports, where vertical displacements (UY) and lateral displacements (UX) are fixed (Figure 11a). In contrast, the larger profiles interact with cylinders through friction, and the cylinders are fixed against all displacements (UX, UY, UZ), as illustrated in Figure 11b. Additionally, in some tests, lateral displacements needed to  
Figure 10: Modeling of the loading scheme for the 170 \(\times\) 2.0 profile (Layout 1). Figure 9: Parts used in the models: (**a**) profile section 300 \(\times\) 2.5, (**b**) contact plate with the profile, and (**c**) support cylinder. be restrained to address instability during upward loading. In such cases, lateral displacements (UX) were fixed at the same locations on the profiles as in the experimental tests. For the 70 \(\times\) 1.5 profile, these locations are at the supports, immediately after the occurrence of the maximum moment (see Figure 3c), where punctual bracing was applied, and at the mid-span. In the case of the 170 \(\times\) 2.0 profile, the locations are the same as for the smaller profile, except for the mid-span. Another noteworthy aspect is the meshing process. Given the hole pattern and bends present in the profile, a refined mesh is necessary. A mesh size of 5 \(\times\) 5 mm\({}^{2}\) was chosen to ensure reasonable consistency throughout the generated mesh. The experimental results were collected from various points of the profile.