PSI - Issue 75

Aijia Li et al. / Procedia Structural Integrity 75 (2025) 318–333 Aijia Li, Christian Garnier, Marie-Laetitia Pastor, Xiaojing Gong, Clément Keller/ Structural Integrity Procedia (2025) 7

324

3.1. Initial simulation procedure

The initial stage of simulation, designated as "Initial simulation procedure," is for the purpose of determining the shape of the gauge and transition region, so it adopts a simplified model, thereby avoiding excessive computation time. Fig. 4 illustrates three types of gauge regions and two types of transitions, thus their combination gives six configurations in total for the geometric model in the simulation. Moreover, the dimensions of the gauge and transition region can be varied in a proper range during the design (Table 2). The material properties are chosen to be isotropic to reduce computation volume. Then, a 1/8 finite element simulation model was established using the symmetric boundary conditions of XY-plane, YZ-plane, and XZ-plane, and the element type of the whole model is uniformly assigned to “C3D4” with four nodes. Last, all geometries are tested under a tension-tension biaxial static load with a biaxiality of 1 and a maximum stress of 200 MPa to achieve an adequate stress concentration related to a failure in the specimen. Because the material is considered isotropic, its failure can be located by the maximum Von-Mises stress.

Table 2. six types of geometries in the initial simulation procedure No Gauge region Transition

Constant

Single circular curve (10 mm < R < 20 mm) Double circular curve (3 mm < R < 6 mm) Single circular curve (10 mm < R < 20 mm) Double circular curve (3 mm < R < 6 mm) Single circular curve (10 mm < R < 20 mm) Double circular curve (3 mm < R < 6 mm)

1

Reduced area (10 mm < d gauge < 20 mm)

2

Total length = 197 mm Arm’s width = 25 mm Total thickness = 3 mm

3

Circular hole (6 mm < d < 12 mm)

Mechanical behavior type = isotropic Equivalent elastic modulus = 2890 MPa Equivalent Poisson’s ratio = 0.3

4

5

Protrusion (16 mm < d < 26 mm)

6

3.2. Final simulation procedure

Once the shape is determined, a final simulation procedure with detailed parameters is carried out to find a suitable dimension. First of all, a series of anisotropic material properties mentioned in Table 1 is employed to precisely characterize the mechanical response of the matrix and reinforcement within the composite structures. To ensure the continuity of the reinforced fibers, the geometric model is changed to a 1/2 model that is symmetric about the XY plane in the thickness direction and has a more specific feature of the gauge region, as shown in Fig. 5. The loading condition is a tension-tension biaxial static load with a biaxiality of 1 and a displacement of 0.5 mm on each arm, and the boundary condition is a symmetry about the XY-plane. For the element type, the continuum shell element called “ SC8R ” with reduced integration is employed for the composite layers, the resin part is assigned to the 3D stress element “ C3D4 ” due to its isotropic material properties, and the cohesive element “ COH3D8 ” with the traction separation law (see Table 3) is introduced between two neighboring composite layers to reflect the laminar behavior and improve calculation accuracy. Considering the element generation strategy, the global size of the element is set as 0.8 mm, and the node density of some complex features, like the reduction, is manually adjusted to optimize the element quality, so the total number of the three types of elements is 353582. After each simulation, the stress and strain data are utilized to calculate the Tsai-Hill failure factor of each element, and then the maximum failure factor on the transition and gauge region is found to calculate the failure parameter B mentioned in the first design criterion. Meanwhile, the distribution of different stress components is visualized by the cloud diagram, for analyzing the uniformity of the stress field. As a consequence, the computational time and workload increase significantly, but results like the failure location and stress field become more reliable for the final design.

Table 3. mechanical properties of the cohesive layer in the final simulation procedure Property Symbol Value

Unit

Material behavior type

Traction

-

-