# Behavior of Two-Chord Steel-Concrete Composite Columns under Axial Compression
## 5 Numerical Modeling  
### FEM Model  
A simulation of the tested specimens was conducted utilizing the finite element method (FEM) using ANSYS Mechanical R17.0 software. The modeling included the nonlinear behavior of the steel and the concrete, the contact of the concrete fill with the steel tube, and the global buckling of the specimen using initial imperfections. The steel tubes, the concrete infill, and the top and bottom rigid plates of the TCCFST column were modeled. Using symmetry conditions allowed for only one-half of the model to be simulated (Figure 17a). The concrete infill was modeled with the SOLID65 element, while the steel elements, which included the cords, the battems, and the upper and the lower loading rigid plates, were simulated using the SOLID181 element. The interaction between the concrete infill and the steel parts of the column was modeled using the contact elements CONTA174 and TARGE170. The contact of the concrete core with the bearing plates and with the inner part of the steel tube was simulated as a frictional connection with a friction  
Figure 16: Codes’ predicted sectional capacity vs. experimental sectional capacity.  
coefficient of 0.7. All other connections between the column parts were modeled as bonded contact to simulate fully welded connections.  
The FEM model consisted of 179163 elements with 64227 nodes. The quality of the mesh was tested in order to optimize the accuracy of the solution with computational time. The concrete was modeled with 10 mm elements, while the load-bearing plates were modeled with \(8\times 8\times 5\) mm elements. Since the geometry of the steel chords and battens was complex, the adaptive mesh size was applied. Two or three layers of solid finite elements were used to model the wall thickness of the steel chord and batten tubes to evade any issues with the computational stability of the solution (Figure 17b). The boundary conditions included the suppression of all degrees of movement and rotation for the lower bearing plate (\(\mathrm{u_{x}=u_{y}=u_{z}=0}\) and \(\mathrm{\varphi_{x}=\varphi_{y}=\varphi_{z}=0}\)), while the upper bearing plate was only free to move in the y-direction (\(\mathrm{u_{x}=u_{z}=0}\) and \(\mathrm{\varphi_{x}=\varphi_{y}=\varphi_{z}=0}\)). Movement u and rotation \(\mathrm{\varphi}\) are the model's degrees of freedom in the global coordinate system. The force imposed on the specimen during the experiment was applied to the FEM model over the top bearing plate as a 1 MN concentric force in the direction of the y-axis. A linear buckling analysis was used to define the initial geometrical imperfections of the model, and a scale factor of \(L/1000\) was applied as a multiplier for the first modal shape. The results were used to simulate the deformed geometry of the model. Because of the expected significant deflections of the model, a nonlinear response was simulated with a large deflection behavior employing the arc-length control and the full Newton-Raphson option. Since the stiffness matrix becomes asymmetrical when a coefficient of friction is applied, an unsymmetrical solver was used in the simulations [38].