## 2 Finite Element (FE) Model and Verification
### Verification  
To verify the accuracy of the FE model, the mesh sensitivity analysis is first carried out so as to eliminate the adverse influence of element size on the calculation results. The element size of the FE model are set to be 40 mm, 30 mm, 20 mm and 12 mm, which results in the total element number of 3240, 6320, 21,666 and 90,720, respectively. The numerical simulation is run by a workstation installed with an Intel Xeon Gold 6154 CPU. The calculation time for each model is 35 min, 40 min, 72 min and 333 min.  
The hysteresis curves of three models are plotted in Figure 7. It can be seen from the figure that the hysteresis curve of 20 mm model is nearly identical to that of 12 mm model, while the curve of 40 mm model is quite different from that of the model with the finest mesh. Therefore, the model with element size of 20 mm can be regarded as a preferable one and used in the following section since it provides almost the same results with the finest model and takes only 22% calculation time of the latter model.  
The experimental hysteresis curves from Lin [22] and from the model with element size of 20 mm are plotted in Figure 8 for clearly comparison. It can be seen from Figure 8 that the hysteresis curve of this study is reversed Z-shaped and well reflect the pinch effect of the timber frame. However, the unloading stiffness is about 35% smaller than the experimental results, which is also seen in [24]. Figure 8 presents the skeleton curves of both experiment and simulation, and both of the curves show the nonlinear behavior when the displacement amplitude is larger than 20 mm. At the positive loading process, when the displacement reaches +120 mm, both skeleton curves begin to slightly decrease. While the descending displacements at the negative loading process of the experiment and the simulation are \(-\)140 mm and \(-\)120 mm, respectively.  
During each cycle of loading, the stiffness is calculated according to Equation (2), in which \(F_{\text{imax}}\) is the force corresponding to the maximum positive displacement \(\Delta_{\text{imax}}\) in the \(i\)th cycle, and \(F_{\text{imin}}\) is the force corresponding to the maximum negative displacement \(\Delta_{\text{imin}}\) in \(i\)th cycle.  
\[K(\Delta_{i})=\frac{|F_{\text{imax}}|+|F_{\text{imin}}|}{|\Delta_{\text{imax}} |+|\Delta_{\text{imin}}|} \tag{2}\]  
For a given cycle \(i\), the dissipated energy due to plastic deformation and friction equals to the area enveloped by the hysteresis curve.  
Figure 7: Hysteresis curves of models with different element sizes.  
Figure 9 shows the stiffness and dissipated energy of each cycle derived from both the experiment and the numerical results of this study. In Figure 9a, the two curves have the identical changing trend except the points of the first cycle. The error of 0.381 between the two points can be attributed to the tightness between the mortise and tenon during installation in the experiment, which exerts some pre-stress on the joints and leads to the increase of rotational stiffness of the experimental model. With the first point excluded, the numerical results well reflect the stiffness degradation of the timber frame. The dissipated energy of each cycle is plotted in Figure 9b, and it shows that the two curves have similar variation tendency, although the energy dissipation capacity of FE model is lower than the experiment. The hysteresis curves of the experiment when the displacement amplitude is less than 80 mm are full as can be seen in Figure 8a, while the enveloped curves of the simulation are reversed Z-shaped, which leads to the errors larger than 0.2. When the displacement amplitude reaches 100 mm, the errors are all within 0.15. Therefore, to a large extent, the FE model of this study can well simulate the hysteresis properties of the real timber frame with straight mortise-tenon joints.