# Finite Element Simulation of HELICOIL(r) Inserts
## 6 Simulation Model for the HELICOIL(r) Insert
### Boundary Conditions  
The upper surface of the screw (marked \(T1\) or RCB) was loaded with increasing displacement. The lower surface of the sample model was fixed in the vertical direction (\(z\)-axis for the FE model). The nodes in the symmetry planes were fixed in a direction perpendicular to the plane (i.e., the \(x\)-direction was fixed for the nodes in the \(yz\)-plane, and the \(y\)-direction was fixed for nodes in the \(xz\)-plane for the coordinate system of the FE model). The contact between the screw and the specimen (a contact area) started 2 [mm] from the upper edge of the specimen hole and ended after 7 [mm] (HELICOIL\({}^{\text{\textregistered}}\) insert length). The situation is depicted in Figure 9.  
\begin{table}
\begin{tabular}{c c c} \hline Displacement [mm] & 0 & 1 \\ Normal stress [MPa] & 0 & 10 \\ \hline \end{tabular}
\end{table}
Table 4: Table of values in a normal direction for the cohesive contact.  
Figure 8: Experimental scheme and comparison of the real model with the simulation model.  
Figure 9: Boundary conditions for the model.  
The lower surface of the FE model was fixed; this area corresponded to the actual specimen at the point where the radius of curvature began. It can be assumed that the displacement at this point would not be zero during loading. The point \(T\)2 was used to correct for this deviation. For the FE model, the following conditions were met: The point \(T\)2 was sufficiently far from the interface (threads), such that we could assume that the displacement of point \(T\)2 would increase linearly with increasing loading force. This condition also results from the material model used (linear elastic). The vertical displacement (z-axis for the FE model) of the \(T\)2 point could be calculated from the FE model. The interface between the screw and the specimen was formed by merging the nodes in the contact area. The displacement values of point \(T\)2 and the loading force for a fixed connection of the screw and the sample are provided in Table 5.  
By interpolation, we obtained a relationship to estimate the displacement \(T\)2 depending on the applied force. From the values of the forces measured at individual time points (Table 3), it was possible to calculate the displacement of the \(T\)2 point \(u_{j}^{T_2}\) (see Table 6). The actual displacement of point \(T\)1 \(u_{j}^{C}\) was then the sum of both values, which was applied to the simulation model.  
\[u^{T2}\approx\frac{F}{77,881}. \tag{43}\]  
The actual value of the displacement at point \(T\)2 will change during the solution, depending on the current value of the forces. We assumed that the course of forces for the resulting parameters would gradually approach the course of forces determined experimentally. Therefore, the displacement values (FEA) at \(T\)2 would finally correspond to the values of the experiment. The simulation would stop at the time of 20 [s], which includes the maximum force load (key, in terms of use) and some of the descending part of the curve. With increasing time, the threaded insert was pulled out, even with the threads cut (see Figure 3).