## 3 Analysis of the Flexural Performances of CCFSts with Gaps
### Numerical Model Configuration
The tensile behavior is assumed to be linear until the tensile strength of the concrete is met, which was taken as \(0.1\times f_{c}^{\prime}\). Beyond the tensile strength, a softening method can be characterized by the fracture energy, \(G_{f}\)[56]. The definition of \(G_{f}\) is shown in Equation (20):  
\[G_{f}=\left(0.0469d_{\max}^{2}-0.5d_{\max}+26\right)\left(0.1f_{c}^{\prime}\right) \tag{20}\]  
where \(d_{\max}\) is the maximum coarse aggregate size in the core concrete. According to [PERSON] et al. (2013) [56], it is set at 20 mm in this study. As a simplification, the ideal bilinear isotropic elastoplastic model [59] was applied for the steel with an elastic modulus of \(2.1\times 10^{5}\) MPa, Poisson's ratio of 0.3, and yield stress of 335 MPa. The [PERSON] yield criterion was applied to describe the elastic-plastic behavior in ABAQUS, which is defined in Equation (21), as follows:  
\[F=\sqrt{3J_{2}}=\frac{1}{\sqrt{2}}\sqrt{\left(\sigma_{1}-\sigma_{2}\right)^{2 }+\left(\sigma_{2}-\sigma_{3}\right)^{2}+\left(\sigma_{1}-\sigma_{3}\right)^{2}} \tag{21}\]  
where \(J_{2}\) is the second invariant of the deviatoric stress tensor, and \(\sigma_{1}\), \(\sigma_{2}\), and \(\sigma_{3}\) are the maximum, intermediate, and minimum principal stresses, respectively. The yield criterion for the steel tube was modeled using the associated flow rule. The cement mortar interlayer was simulated by the cohesive elements, and the related properties were defined via the user self-defined subroutine in ABAQUS software [60]. The Mode I and Mode II fracture energies of the mortar interlayer was determined according to [PERSON] and [PERSON] [61], and the initial stiffness and strength are derived by the test data [62]. The friction coefficient is set as 0.6 [63]. The material properties are shown in Table 2.  
The CCFST mode adopted a circular section with an outer diameter of 170 mm, steel tube thickness of 2.5 mm, and length of 2000 mm. The distances between the two lower supports was 1800 mm, and the upper indenter was placed at the midpoint of the specimen. The cross-section and front view are illustrated in Figure 5a,b. The concrete core and the outer steel tube were firstly established and then the 8-node zero thickness elements were inserted into the interface between the concrete core and the outer steel tube. The finite element model is shown in Figure 5c. A quasi-static analysis was adopted, and the influence of the loading speed can be ignored. The contacts along the surfaces surrounding the coronal gap were set as the normal \"hard\" contact model, with a tangential penalty friction coefficient of 0.6 [63]. Meanwhile, the contacts between the steel tube and the supports w treated in the same way as above. The friction coefficient should be enough to prevent structural instability. A displacement-control vertical load of 80 mm was applied on the upper indenter to realize the bending deformation of the structure until the peak force was reached. In this study, the ABAQUS software was employed to conduct finite element analysis. The general static procedure in ABAQUS was used to solve the equilibrium state of the model under the applied loads. This technology was appropriate for time-independent problems, where the system response was analyzed after it has reached equilibrium under the given loading conditions. During this procedure, ABAQUS used an incremental-iterative method to solve the system of equations and find the equilibrium state. Specifically, the total applied load was divided into multiple load increments. In each increment, ABAQUS iteratively solved the equilibrium equations for the current step. When the convergence criteria were met, the system proceeded to the next increment until all load increments were completed.