## 3 Analysis of Test Results
### Numerical Simulation of Experimental Tank Model  
ANSYS software was used to simulate the experimental storage tank model, and the differences between the numerical results and the experimental results are compared to verify the validity and reliability of the finite element model, paving the way for further study on seismic performance of large LNG storage tanks. The bilinear kinematic hardening model was used for the concrete outer tank, dome and pile foundation. The material parameters of the numerical model are based on those of the test tank, and the parameters of the lead-core rubber bearing are shown in Table 2. The storage tank is simulated by the SOLID186 element. The pile foundation is simulated by the BEAM188 element. The contact element is used for connection between the pile foundation and the storage tank. [PERSON] et al. [12; 28; 29; 30] have conducted in-depth research on the numerical simulation of LNG storage tanks. Their article gives detailed information about the meshing method and mesh element selection. The results show that by dividing two elements along the thickness direction and ensuring that the element shape is a cube as much as possible, the simulated results can have high computational accuracy. Therefore, the finite element model of the LNG storage tank in this paper was divided into 2 elements in the thickness direction, 64 elements in the hoop direction, and 21 elements in the height direction; the mapped meshing method was used for the mesh division. The selected element is SOLID186 element, which is a high-order element with 20 nodes and three degrees of freedom, with a total of 10,169 elements. In the element library of ANSYS, there is no element that can directly simulate the mechanical properties of lead-core rubber isolation bearings. Therefore, it is necessary to simplify the mechanical properties of the isolation bearing and conduct a reasonable simulation according to mechanical behavior of the isolation bearing. The lead-core rubber bearing has good hysteresis performance and can be simulated by a bilinear model. The mechanical properties of the lead-core rubber bearing in the horizontal and vertical directions are very different. The lead-core rubber bearing will yield in the horizontal direction, but will not yield in the vertical direction. According to this characteristic, nonlinear spring (Combin40) and linear spring (Combin14) are used to simulate the horizontal and vertical performances of the lead-core rubber bearing, respectively. The basic parameters of lead rubber bearings are: stiffness before yield K1, stiffness after yield K2, yield load Q, and damping ratio. The main real constants of COMBIN40 element are: Ku (stiffness before yielding), C (damping coefficient), M (mass), GAP (gap size), FSLID (shear force at yield), and Kd (stiffness after yielding). COMBIN40 is a two-stage spring. When the limit force (FSLID) is reached, K1 does not work, and the stiffness becomes K2. If there is no K2, it is equivalent to the spring being pulled off, so the COMBIN40 can simulate the bilinear model. A lead-core rubber bearing consists of three spring elements, COMBIN40 (X-direction), COMBIN40 (Y-direction) and COMBIN40 (Z-direction), where the COMBIN40 element in the X- and Y-directions should consider the bilinear model. When establishing three spring elements, the thickness of the lead-core rubber support can be ignored, and the node positions of the elements can be coincident. Then, the direction of spring element can be specified by changing the key option of the spring element. When the element is established, the nodes of spring element are coupled with the SOLID186 element simulating the bearing platform. The other end nodes of the horizontal spring in X- and Y-directions constrain all the degrees of freedom, and the other end nodes of the Z-direction spring element couple the degrees of freedom with the upper node of the BEAM188 element that simulates pile foundation.