# Effect of Residual Stress in Surface Layer on Plastic Yield Inception
## 2 Methods  
A contact model between a rigid hemisphere and a plane consisting of a surface layer and substrate was developed, as shown in Figure 1. An evenly distributed load P was applied to the top of the hemisphere to create an interaction between the two contact bodies. The following main assumptions are adopted:  
1. Both the material of substrate and the surface layer are homogeneous. 2. The surface layer and the substrate are perfectly bonded. 3. Residual stress in the surface layer is homogeneous along the thickness. This assumption is often adopted in the study of residual stress of films/coatings [6,24,26], especially for the films/coatings with small thickness. The contact was simulated using the finite element software ANSYS Workbench 16.0 (ANSYS Inc., Canonsburg, PA, USA). Considering the symmetry of the model, an axisymmetric 2D model was established. The boundary conditions are shown in Figure 2. Roller boundary conditions were applied on the axis of symmetry, bottom surface, and outer surface. For a practical surface layer and substrate system, the in-plane size is much larger than the surface layer thickness. The roller boundary condition on the outer surface is used to simulate the acting force of material out of the outer surface. It has been verified that free of the outer surface only led to stress concentration near the outer edge and had no significant effect on the stress field of the contact zone (see Appendix A). The friction coefficient between the contact pairs is set to be 0.15. The rigid hemisphere is modeled by setting the Young's modulus to be significantly larger (1000 times) than that of the surface layer and substrate. Figure 1: Contact between rigid hemisphere and plane consisting of surface layer and substrate. The geometric parameters of the finite element model are listed in Table 1. The radius of the rigid hemisphere is in the range of \(0.1\leq\ R\ \leq 10\) mm. To cover a relatively wide thickness range, the thickness of the surface layer relative to the radius of the rigid halfsphere (\(t/R\)) is basically a geometric sequence, as presented in Table 1. When \(R=0.1\) mm and \(t/R=0.0005\), the thickness of the surface layer is the smallest (50 nm), and when \(R=10\) mm and \(t/R=1.28\) mm, the thickness of the surface layer is the largest (1.28 mm). This range covers the thickness of the surface layer, which is commonly used in engineering applications. The dimensions of the substrate in relative to the radius of the rigid halfsphere (\(R\)) are presented in Figure 2. It has been verified that a further increase of the dimension of the substrate had no effect on the results. To obtain reasonable meshing, the computational domain was divided into layered subdomains along the depth, as shown in Figure 3, and distinguished by different colors. This method has two advantages. Firstly, the mesh density of each layer (subdomain) can be set independently, whereas the nodes on the boundary are shared. Compared with the more distant subdomain, a smaller layer thickness and finer mesh can be adopted close to the contact zone. Secondly, the material parameters of each layer (subdomain) can be set independently by changing the number of layers (subdomains) which possess the material parameters of surface layer, and the thickness of the surface layer can be changed without re-meshing the computational domain. The model contains approximately 120,000 eight-node axisymmetric quadratic quadrilateral elements and 1500 six-node axisymmetric quadratic triangular elements, totaling approximately 400,000 nodes. \begin{table}
\begin{tabular}{c c c c c c c c c c c c} \hline \hline
**Parameter** & & & & & & & & & & & & & \\ \hline \(R\) & & & & & & & 0.1 mm \(\leq R\leq 10\) mm & & & & & & \\ \(t/R\) & 0.0005 & 0.001 & 0.002 & 0.004 & 0.006 & 0.008 & 0.01 & 0.012 & 0.016 & 0.032 & 0.064 & 0.128 \\ \(t\) & & & & & & & 50 nm \(\leq t\leq 1.28\) mm & & & & & & \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Geometry parameter of the finite element model. Figure 2: Finite element model.