## 3 Results and Discussion
### Finite Element Analysis  
Simulations were performed in the ANSYS _Static Structural_ analysis system. With account of the symmetry, only a quarter of the model was analysed, which then was meshed with the higher-order tetrahedral ten-node _SOLID187_ elements (Figure 6). After performing a mesh convergence study, different mesh sizes were used: 3 mm for bolts; 5 mm for extended parts of the endplate; 15 mm for the middle part of the endplate; 2.5 mm for fillet welds; 10 mm for the steel tube; 15 mm for the middle part of the concrete core. For the other parts, the default global mesh size of 83 mm was left. Additionally, mesh refinements were implemented near the welds and in the tension zone of the steel tube. In these critical areas, mesh size was decreased in such a way that the endplate and the bolt hole would be meshed with four layers of elements along their thicknesses, which exceeds recommendations of [PERSON] et al. [29]. Another plausibility of assessing the mesh quality is to directly compare FEA results with the experiments [30; 31]. The material model for the concrete was assumed to be linear elastic. In contrast, bolts and beams were modelled with elastic perfectly plastic material. Moreover, for the column tube, the multi-linear isotropic plasticity model (Figure 7) was chosen to overcome problems with the convergence, which are related to the simulation of the punching shear fracture. Geometrical nonlinearities were not considered. The model was loaded in a similar sequence as the one in the experiment: the axial force in the column was introduced by displacement control loading during the first step, and a vertical force was applied to the end of the beam during the second step. In addition to this, the bolts were preloaded during the first step. Fourteen frictional contact pairs were introduced: between the endplate and the column; the bolt heads and the endplate; the nuts and the inner surface of the column; the bolt shanks and the bolt holes; the concrete and the inner surface of the column. Additionally, the nut of the bolt in tension zone was split into six surfaces (Figure 8) to even out concentration of the force. Augmented Lagrange formulation was used for all contacts with stiffness update at each iteration. The initial contact interface treatment was set to the \"adjust to touch\" option and all friction coefficients were set to 0.2. Figure 6: FEA model of the moment resisting joint with curved endplates. Four models with the different gaps were additionally created in order to study the effect of the not firm contact. The endplates were modelled on a single Gaussian curvature, as the main cause of such imperfection is the difference in radii of the surfaces in contact. This difference can be positive (gap in the middle), negative (gap at corners), or absent (zero). Results of the Finite Element Analysis  
The parametric study has shown that connections with the gaps in the middle of the endplate have not only the lowest values of the initial rotational stiffness, but also the lowest \"ultimate\" bending resistance. This may be caused by the prying action in tension zone and the warping of the endplate in compression zone. Warping occurred with the closure of the gap, when the corners of the endplate deformed outwards (Figure 9c,d). In contrast, in the connections with the firm contact and connections with the gaps at the corners, prying did not occur due to clamping force in the initial loading stage and limited contact area in its final stages. Moreover, warping of the endplate in compression zone was also limited. This is evident from the formation of the plastic hinges, which were forming near the weld line (Figure 9a,b). This resulted in higher values of initial stiffness and bending resistance. Figure 8: Division of the nut surface. Figure 7: Stress-strain curve used for circular hollow section (CHS).