*2.4. Numerical Model—General Description*

A 3D numerical model of the experimental research was built in ABAQUS software [21]. Geometrically and materially non-linear static analysis was performed. An elastic-plastic model of the material (steel S250GD + Z) was reflected by the following properties: elastic modulus *E* = 210 GPa, Poisson's ratio ν = 0.3 and yield stress *fy* = 250 MPa.

The frame members and corrugated sheets were modelled by 20,100 shell elements with four nodes and four integration points (S4) and the size of 8–12 mm. Profiles were built with sharp corners (radius of curved elements equal to zero). The meshed structure is presented in Figure 5a.

**Figure 5.** Numerical model: (**a**) view of the whole model with global coordinates; (**b**) detail of the frame hinge.

The frame members were modelled in a simplified way. Each of the RHS profiles, which in tests were the supports for the sheeting, was built as one element together with the U-shaped cold-formed plate. The thickness of the U-shaped plate (0.5 mm on the sides, 1.5 mm on the top) was assigned, so that the stiffness of the profile was mapped. Hinge connections in the frame were included using four reference points (RP in Figure 5b) in four axial nodes of the frame, which were tied (six degrees

of freedom fixed) with four corners of the shell frame element. This way allowed us to model the hinge without the necessity of building the details of the connection. The connection is presented in Figure 5b.

Fasteners (self-drilling screws) were mapped using tie connections between nodes (six degrees of freedom fixed). The propping effect was included by modelling the contact between the sheeting and the frame (with the separation allowed after contact).

Boundary conditions were assigned using references points. In nodes 1 and 3 the displacement in y direction was fixed; in node 4—displacements in *x*, *y* and *z* directions were fixed (for numbers of nodes see Figure 1). In node 2 the displacement increase was applied in the direction of the frame diagonal until the failure of the panel. Stress maps were obtained. The numerical analysis results are presented in Section 3.2.
