# Behaviour of Steel Tubular Knee Joint in Aluminium Frames with Tension-Tie Element
## 3 Numerical Analysis  
### General Overview of the Numerical Model  
Numerical modelling was conducted in software package ANSYS 17.0 [23]. Geometrical properties of the numerical model were determined according to laboratory measurements to achieve more realistic behaviour. Thicknesses of the steel tube sections were determined as an average of measured values [22]. To apply different material properties to various parts of the numerical model and to generate more precise mesh, the numerical model was divided into several geometrical parts (Figure 12). Only solid finite elements were used in the analysis, both tetrahedral and hexagonal. Finite element size in the model was 7.5 mm, which was enough to achieve mesh convergence. In the contact regions, mesh was refined to 2.5 mm element size to achieve more accurate results. Nonlinear behaviour of the base material was included using multilinear stress-strain curves analogous to those obtained by coupon tensile tests, Figure 4. All the stress-strain curves were transformed into true stress-strain curves by common rules to achieve more accurate results. It must be noted that no tensile tests were performed for the tie element; therefore, to model the behaviour of the tie element, the same mechanical properties were used as for the RHS 180 \(\times\) 80 \(\times\) 3 element. Since no plastic deformations of the tie element were recorded during laboratory tests, such simplification had a negligible effect on the  
Figure 11: Force in the piston-force in the tie element relationship. overall behaviour of the steel specimen. Nonlinear behaviour of the bolts was included using a multilinear stress-strain curve. Since bolts were not tested, nominal strength values for the 8.8 quality bolt class were used. Prior to reaching a bolt yield strength of 640 MPa, material behaviour was modelled as linear elastic with E = 2 \(\times\) 10\({}^{5}\) MPa. The ultimate strength of 800 MPa corresponds to plastic deformation of 1%, followed by a plateau region up to an ultimate deformation of 2%. Initial geometrical imperfection of the steel specimen around the butt-welded connection was included in numerical models as well. To prevent the penetration in the contact region between the two parts of the model, contact interaction between the surfaces was defined or the addition of the contact elements was introduced. Numerical modelling was conducted using three-dimensional solid elements only. To reduce the number of finite elements in the model and to shorten the calculation time, symmetry around the vertical plane was used [21]. Boundary conditions in the numerical model were defined to represent those of the laboratory test as accurately as possible. At both ends, the steel specimen was free to rotate around the horizontal axis while translations at both ends were restricted in all directions except for vertical displacement at the free end of the beam to allow the introduction of the load in the specimen in the form of a 30 mm vertical displacement. It must be noted that 2 mm displacement of the supporting structure in the horizontal direction occurred during the loading phase, which corresponds to approx. 2 mm displacement in the vertical direction at the piston. That was included in the numerical results as 2 mm translation of the numerically obtained force-piston displacement curve (Figure 13a). All the boundary conditions in the model were assigned on the perimeter of the pin hole. Figure 12: Numerical model (3D view). Figure 13: Comparison between experimental and numerical results: (**a**) load-displacement; (**b**) moment–rotation curves. Loading of the steel specimen was modelled in two steps. Prestressing of the bolts to a value of 10 kN that corresponds to manual tightening of the bolts as well as out of plane line pressure of 40 N/mm at the line of the web welds to represent initial deformations in the HAZ were modelled in the first load step. Linearly increasing displacement of 30 mm in the vertical direction at the free column end was modelled in the second loading step.