# Analysis of Interference-Fit Joints
## 3 Results of Numerical Calculations and Experimental Studies  
### Numerical Simulation of the Pressing Process  
For each of the above joints, the pressing process was modeled using the Finite Element Method (FEM) and the Ansys v. 19.1 calculation system. The discussed set has an axis of symmetry, therefore it seems advantageous to use an axisymmetric model in the analysis. Initially, the authors prepared such a model, however, it was found that ANSYS simulation of interference using axial-symmetry led to errors that prevented effective completion of the analysis. Therefore, an axisymmetric model was abandoned in the numerical analysis. Figure 3 shows the discrete model of the shaft and the hub in the initial configuration. The model was divided with the use of solid hexagonal finite elements SOLID 186 [18]. The mesh of nodes was densified towards the contact surface. The model has 61,440 elements and 262,161 nodes. The FEM model used a bi-linear material model, with a tangent modulus of 1450 MPa. The outer surface of the shaft and the inner surface of the hub were assumed as contact surfaces. The contact was modeled with CONTA 174 and TARGE 170 elements [18]. The contact model is based on the Lagrange function with an exterior penalty function (aug \begin{table}
\begin{tabular}{c c c c c} \hline \hline
**Joint** & **Surface Pressure** & **Breaking Force** & **Surface Pressure** & **Breaking Force** \\
**Symbol** & **acc. (I)**, MPa** & **acc. (Z)**, N** & **acc. (J)**, MPa** & **acc. (Z)**, N** \\ \hline J1 & 44.10 & 1663 & 15.88 & 599 \\ J2 & 66.15 & 2494 & 37.93 & 1430 \\ J3 & 88.20 & 3325 & 59.98 & 2261 \\ J4 & 110.25 & 4156 & 82.03 & 3092 \\ J5 & 132.30 & 4988 & 104.08 & 3924 \\ J6 & 154.35 & 5819 & 126.13 & 4755 \\ J7 & 176.40 & 6650 & 148.18 & 5586 \\ J8 & 198.45 & 7481 & 170.23 & 6417 \\ J9 & 220.50 & 8313 & 192.28 & 7249 \\ J10 & 242.55 & 9144 & 214.33 & 8080 \\ J11 & 264.60 & 9975 & 236.38 & 8911 \\ J12 & 286.65 & 10,806 & 258.43 & 9742 \\ J13 & 308.70 & 11,638 & 280.48 & 10,574 \\ J14 & 330.75 & 12,469 & 302.53 & 11,405 \\ J15 & 352.80 & 13,300 & 324.58 & 12,236 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Results of calculations of surface pressures and breaking forces based on classic and modified Lame’s formulas. Figure 3: A discrete model. mented Lagrange formulation) described in [19]. It is worth noting here that the authors of this study also consider the use of another contact model for modeling interference, e.g., B-Spline surface for contact surface smoothing described in [20]. The front outer surface of the hub shown in Figure 4 was fixed. Displacement of the shaft front face of 15 mm was assumed opposite to the Z-axis direction of the coordinate system. In the pressing process simulation, the shaft moves in the hub in 30 steps of 0.5 mm each. The maximum force determined in the pressing analysis corresponds to the force required to assemble the joint. After pressing, a simulation of the shaft withdrawal was carried out. It was assumed that the force which causes the shaft to withdraw from the hub by the value of 0.1 mm is the force that destroys the joint. Figure 5 shows the distribution of the maximum principal stresses in the hub and shaft after pressing, for the J5 joint. Figure 6 shows the same stress distribution separately for the hub and the shaft. Figure 4: Fixed area. Figure 5: Principal stresses contour-assembly view. Table 3 summarizes the maximum values of surface pressure and plastic strain obtained for individual joints. Figure 9 shows the distribution of total strains. The diagram of assembly forces at each pressing step and the value of the force breaking the joint are shown in Figure 10.  
Column 4 in Table 4 presents values of the joint breaking forces obtained as a result of numerical simulations, compared to the values of the breaking forces obtained from analytical formulas (columns 5 and 6). To verify the correctness of the numerical model, experimental tests were carried out to determine the breaking force for the J5 joint.