## 2 Experimental Methods and Simulations
### Simulation Methods  
#### 2.2.1 Crystal Plasticity Models  
The deformation of crystalline materials is a complicated process, which is not only related to macro factors, such as loading direction, rates, deformation amount, etc., but also to some micro factors, such as crystal orientations, microstructure and deformation mechanism. The mechanical behaviors of materials are closely related to the loading direction due to the anisotropy of elastic tensor of the material. Besides, the microstructure of materials has crystallographic orientation, which results in the different properties of polycrystalline materials under different loading direction during the elastoplastic transformation process. In the numerical simulation research based on the phase structure of alloy materials, the mechanical constitutive phase of each constituent phase can be simplified into an isotropic constitutive model. In the CPFEM, the anisotropic constitutive parameters used for different crystal orientations and the factors such as the crystal structure type, slip deformation, hardening effect, and the change of crystal orientation are considered, which make the simulation calculations more accurate. The model was developed from an EBSD image. The local area selected was 16.5 \(\upmu\)m \(\times\) 10.1 \(\upmu\)m (see Figure 2a). The area consisted of 12 grains, including seven \(\upalpha\)-phase grains and five \(\upbeta\)-phase grains. The grains were numbered (i.e., 1, 2, 3, and so on) and the excel file including crystal structure, centroid position, Euler angles (\(\varphi_{1}\), \(\phi\), \(\varphi_{2}\)) was output by channel5 software. Based on the RGB values of the image pixels, a 2D finite element model was developed. However, the 2D model used the plane strain or plane stress assumption, which may affect the accuracy of the simulation. Therefore, a unit thickness finite element model was established with 8-node 3D hexahedron solid elements, using the microstructure-based finite element model construction software developed by our group [27] (see Figure 2b), so it is called a 2.5D finite element model [19, 28], which can reduce the calculation time and well reflect the actual situation. Each grain was considered as a single crystal, with a uniform crystallographic orientation, and its Euler angle was determined by centroid result. The model was meshed into \(165\times 101\times 1\) elements, with each element having dimensions of 0.1 \(\upmu\)m \(\times\) 0.1 \(\upmu\)m \(\times\) 0.1 \(\upmu\)m. To simulate the quasi-static tensile experiment, boundary conditions were defined to obtain a uniaxial average stress state while upside and downside were a traction-free surface. Then, homogeneous normal displacement, i.e., in the loading direction X, was prescribed on left side in order to correspond to strains imposed during the experiments described in Figure 2d, which produced a displacement of 2.56 \(\upmu\)m at \(1.55\times 10^{5}\) ms. Constraints on right side are defined in order to keep the face in stationary state. Finally, a total of 155 steps of loading were performed while the total deformation was 15.5%, and the commercial software Ansys/LS-Dyna was used to simulate the deformation process. Besides, we expanded the functions of Ansys/LS-Dyna [29] and the specific process is as follow:(1) Read the parameter file containing the slip systems, elastic constants, critical resolved shear stress (CRSS), hardening coefficient, crystal orientation information, and stress-strain information in the sample coordinate system. (2) Through the rotation matrix \(g\), the mapping relationship between the sample coordinate system and the crystal coordinate system is established, so that the input constitutive parameters can be converted during the calculation. \[