# Numerical Simulation of T Joints Constructed from Hollow Steel Sections
## 3 FEM Modeling  
The commercial software ANSYS R14.5, which is based on FEM, was utilized to perform numerical analyses. Two solid bodies were assembled to represent the joint in the model. The chord element was represented by the second body, whereas the perpendicular brace and fillet weld were comprised of the first body. The weld was only represented at the brace's straight sections in order to simplify the model. As mentioned in Table 1 and shown in Figures 2 and 3, the boundary conditions were carefully chosen to replicate the experimental conditions. Surfaces that made contact with the experimental rig's fixed parts were configured to move zero degrees in the direction perpendicular to the contact surface. By defining a bonded contact pair between the surfaces of the two bodies, the contact between the brace/fillet weld and the chord was established.  
The automatic mesh generator included with ANSYS Mechanical was used to create the mesh. The command body sizing was used to control the element's size. Automatic mesh refinement was applied at the surface level, set to half of the body element size, in the high-stress areas, namely at the brace and chord contact. By changing the element size at the body level, this method made the mesh convergence research easier to complete. For element sizes of 15 mm, 10 mm, and 5 mm, calculations were made. Meshing was performed using SOL-ID187 elements, which are higher-order 3-D, 10-node elements with quadratic displacement behaviors appropriate for modeling irregular meshes. According  
\begin{table}
\begin{tabular}{c c c} \hline \hline
**Notation in** & **Type of Element** & **Fixed Displacement(s)** \\
**Figure 2** & & \\ \hline A & Surface & \(Z=0\) \\ \hline B & Line & \(X=Y=Z=0\) \\ \hline C & Surface & \(Y=0\) \\ \hline D & Line & \\  & (both sides of the chord) & \\ \hline E &
\begin{tabular}{c} Node \\ (middle of the top surface of \\ the solid plate) \\ \end{tabular} & Load as nodal displacement \(Y=Z=6\) mm \\ \hline \hline \end{tabular}
\end{table}
Table 1: Boundary conditions.  
to the mesh convergence investigation, there was no discernible difference between the two finer-meshed models' estimations for the development of total strain with increasing load. Thus, both meshes were to be sufficient.  
The following basic input data were applied to the material, taking into account both geometrical and material non-linearity in the numerical analysis:  
The yield strength and ultimate strength of the steel material were modeled as described in Section Material Parameters of Joined Elements, with the following applied values: for the chord element, the yield strength was set to \(f_{y}=282\) MPa and the ultimate strength to \(f_{u}=381\) MPa; for the brace element, the yield strength was specified as \(f_{y}=255\) MPa and the ultimate strength as \(f_{u}=355\) MPa.  
* Modulus of elasticity \(E=2.1\times 10^{5}\) MPa;
* Tangent modulus of elasticity was calculated according to [30], and equal to  
Figure 3: Local deformations of “T” connection in mm for ultimate bearing capacity of connection determined by EC 3 with nominal yield strength.  
Figure 2: Boundary conditions of the model.  
\[E_{T}=\frac{1}{12.5}\cdot E=0.168\times 10^{5}\ \text{MPa}\]
* The applied Poisson's ratio value was 0.3;
* Based on the suggestions made in [30], traditional bilinear kinematic hardening, or BKIN, was used to represent the non-linearity of steel. Cases with minor strains and materials meeting the von Mises yield criterion are suitable for this model. The selected option incorporates the Bauschinger effect and assumes that the entire stress range is equal to twice the yield stress. For analyzing the type of link that is being offered, this makes the BKIN model relevant;
* Applied yield criteria: von Mises/Hill.