## 2 Materials and Methods
### Mathematical and Finite Element Models
With the insertion depth \(h_{in}=5\) um and the diameter of the cylindrical indenter \(d=9\) mm, it is possible to estimate the width of the contact zone along the direction perpendicular to the plane of simulation as follows  
\[L_{c}=2\sqrt{h_{in}\cdot d-h_{in}^{2}}\approx\sqrt{h_{in}\cdot d}\approx 0.424 \text{ mm}=4.24\cdot 10^{-4}\text{ m}. \tag{6}\]  
This estimate is from above (maximum), since it is assumed that the cylinder contacts the entire depressed surface. In fact, due to the elasticity of the real metal material, contact does not occur on the entire surface. If we calculate \(S_{\text{3D}}\) more precisely through the circular segment area and the corresponding area of the cone plane section, then we can get the value for the coefficient \(k=1.334\). Thus, to match the forces, we have the values given in Table 2.  
The values of density, elastic modules, and other thermophysical parameters as well as their dependences on the temperature used in the calculations were taken from [24; 25] and are presented in Appendix A. The developed mathematical model formed the basis of the FEM model. The ABAQUS computer code was used for the numerical calculation of stress, strain, and temperature fields. The simulation was performed in two steps. In the first step, the quasi-static task of indenter penetration into the sample surface under the action of a constant burnishing force was analyzed using ABAQUS/Standard. Using the distribution of stresses and deformations from the first step, the subsequent analysis of the indenter movement with a sliding speed and under the action of the burnishing force was carried out in the second step. To solve a quasi-static problem, the ABAQUS/Explicit code was used. As known, the use of ABAQUS/Explicit (explicit solver) allows one to quickly perform quasi-static simulations using explicit dynamics in the case of complex constitutive relations and contact conditions if certain approaches are used [26; 27]. The mesh density was determined by the applied loads and boundary conditions. Since a burnishing process leads to high deformations, stresses, and temperatures in the near-surface zone, a very fine mesh is required precisely at the contact zones of the indenter with the material being processed. Away from this zone, stresses and temperature gradients become low, small-scale, and a coarser mesh can be used there. In this two-dimensional study, the workpiece had the shape of a rectangle with a length of 22 mm and a thickness of 9 mm. The FEM mesh consisted of 60,200 linear quadrilateral elements of CPE4 RT type (4-node plane strain thermally coupled bilinear displacement and temperature). The grid contained 1721 nodes in length and 35 nodes in thickness (Figure 3). The smallest element of the mesh was square with a size of 10 um. These dimensions were chosen based on a preliminary study on the mesh convergence of the resulting solution. The indenter was considered a rigid body with its shape defined by an analytical surface in the form of a set of linear segments. To account for the heat sink in the indenter, its point heat capacitance was set in the calculations. To simulate the contact with Coulomb friction between the indenter and the treated surface, a 'Surface to surface' type contact was adopted. \begin{table}
\begin{tabular}{c c} \hline \(\mathbf{P_{\text{3D}}}\), \(\mathbf{N}\) & \(\mathbf{P_{\text{2D}}}\), \(\mathbf{k}\mathbf{N}\) \\ \hline
100 & 354 \\
150 & 531 \\
200 & 708 \\
250 & 885 \\ \hline \end{tabular}
\end{table} 
Table 2: Correspondence of forces in three-dimensional and two-dimensional cases.