## 2 Finite Element Model
### ABAQUS-FRANC3D Co-Modeling  
In this paper, FEM was used to study the stress field at the crack tip. Finite element analysis software ABAQUS and crack analysis software FRANC3D were selected as simulation platforms. Among them, ABAQUS was used as modeling tool and solver, and FRANC3D was used as crack treatment tool [23]. The ABAQUS is a nonlinear finite element analysis software from Dassault SIMULIA, which is used for finite element modeling, model segmentation, and solution analysis and post-processing of stress-strain results [24]. FRANC3D is a new generation of crack analysis software developed by American FAC company, which is used for crack implantation, mesh repartition, model splicing and transformation of stress field results to fracture parameters. This joint simulation method combines the characteristics of the two software, has the advantages of free modeling and free crack addition, and can directly obtain the SIF J integral and other fracture parameters of the whole crack tip [25]. The workflow is shown in Figure 2. The specific operation steps are as follows:  
* Build the finite element model in ABAQUS, and define the corresponding model size, material properties, assembly form and grid division;
* In ABAQUS, the model is divided into the regions to implant cracks and the complementary remaining regions;
* In FRANC3D, the area to implant the crack is imported, and the corresponding crack is implanted at the predetermined position. The appropriate mesh refinement parameters are selected. * Import the splicing new model into ABAQUS, define contact properties, apply bending load and boundary conditions, create a calculation file, add necessary keywords and submit the calculation;
* The calculation results were extracted in ABAQUS to obtain the stress-strain field of the finite element model, and the fracture parameter report of the crack tip could be obtained in FRANC3D. The finite element model of the simplified structure of the wing integral panel is shown in Figure 3. Due to its high strength and good fatigue strength, 2024 aluminum alloy [26] is widely used in aircraft structure, especially where the wing and fuselage structure are subject to tension. The integral underside panel of the wing is mainly subjected to tension due to bending load. Therefore, the panel was made of 2024 aluminum alloy. The material properties of 2024 aluminum alloy are shown in Table 1. The total length and width of the integration panel are \(L=160\) mm and \(W=100\) mm, and the thickness of the skin is \(t_{m}=5\) mm. The rib spacing, rib height and rib thickness of the integral panel are \(d=80\) mm, \(h=30\) mm and \(t=4\) mm, respectively. The main internal forces on the wing are vertical shear, vertical bending moment and torque. In the analysis of the opening crack in the integral lower panel of the wing, the shear stress on the crack surface plays a small role, while the tensile stress on the crack surface caused by bending moment is the main force for the initiation and propagation of the crack. Thus, in this paper, the stress field at the  
Figure 2: ABAQUS-FRANC3D co-modeling process. crack tip of the wing under bending load was taken as the focus of analysis. The finite element model of integral panel under bending load is shown in Figure 3. One side of the panel, which is the parallel plane of YOZ at the farthest direction along X, was limited by three degrees of freedom. On the other side the bending moment M which is around the \(Y\)-axis was loaded. The through crack is directly related to the damage tolerance of the component, so in this paper, the through crack is taken as the object to study the influence of the structural parameters of the integral panel on the stress intensity factor at the crack tip [17]. In the model, the integral panel model is a three-dimensional solid unit, and the material is 2024. Before dividing the grid, the whole model is divided into crack propagation region and other parts.