## 2 Finite Element Model Verification
### Building Up Finite Element Model  
Material properties required for finite element analysis were extracted through an experimental method. Density was measured using a digital balance, and [PERSON]'s modulus was estimated through the modal test, as shown in Figure 6. The natural frequencies and the corresponding mode shapes were obtained through the modal test. [PERSON]'s modulus was corrected so that the modal frequency calculated from the finite element analysis had the same natural frequency obtained by the modal test. Table 4 shows the corrected material properties used in the finite element analysis model. The material properties of wafer, pad, and platen were used by the manufacturer-provided values since no further experiments for material property estimation such as modal tests could be performed. The finite element analysis was conducted using ABAQUS. The finite element model consists of a pad, retainer ring, wafer, and platen, as shown in Figure 7. Since the rebound phenomenon mainly occurs due to the static interaction between the pad, wafer, and retainer ring, it is attempted to explain this phenomenon only with static analysis. The boundary conditions and load conditions of the analysis model are as follows. A fix boundary condition is applied to the lower part of the platen, and a contact \begin{table}
\begin{tabular}{c c c c} \hline \hline  & **Elastic Modulus** & **Density** & **Poisson’s Ratio** \\  & **(MPa)** & **(kg/m\({}^{3}\))** & **Poisson’s Ratio** \\ \hline Wafer & 10,000 & 2329 & 0.22 \\ Retainer ring (Polyether ether ketone) & 2935 & 1174 & 0.39 \\ Retainer ring (Inner metal ring) & 70,080 & 6020 & 0.32 \\ Pad & 20 & 35 & 0.1 \\ Platen & 190,000 & 7850 & 0.3 \\ \hline \hline \end{tabular}
\end{table} 
Table 4: Material properties. Figure 6: Modal experimental setup. \begin{table}
\begin{tabular}{c c c c c} \hline \hline \multicolumn{1}{c}{**P\({}_{1}\) [psi]**} & **9.3** & **8.5** & **7.65** & **6.0** \\ \hline Maximum relative MRR & 1148/1027 & 572/606 & \(-\)1244/\(-\)1215 & \(-\)2175/\(-\)2121 \\
[averaged] & [1107] & [589] & [\(-\)1230] & [\(-\)2148] \\ Relative MRR@7 mm & 881/810 & 502/514 & 106/85 & \(-\)779/\(-\)631 \\
[averaged] & 966/892 & [508] & [96] & [\(-\)705] \\
[887] & & & & \\ \hline \hline \end{tabular}
\end{table} 
Table 3: MRR result of model #4 for each load condition (R/P\({}_{2}\)/P\({}_{3}\)/P\({}_{4}\)/P\({}_{4}\) = 11.9/4.4/4.5/4.5/4.7 psi). condition is considered between the polishing pad and the wafer and between the polishing pad and the retainer ring with a friction coefficient of 0.1 [17] by referring to the Stribeck Curve. Tie constraint conditions are used between the platen and the polishing pad and between the retainer ring and the inner metal. Each pressure is applied to the wafer through the multi-zone carrier head, and each applied area is shown in Table 1. The load applied from the multi-zone carrier head to the wafer and the retainer ring is considered only for the vertical load. There are several uncertainties of the finite element model. First, since the real retainer ring rotates in the CMP process, there may be some discrepancy between the actual response and the result from the finite element analysis. In addition, the pressure applied to the wafer in the finite element model may be slightly different from the actual pressure applied to the wafer through the membrane from the multi-zone carrier head. Therefore, through the finite element analysis, it is mainly observed whether the trend of the MRR results is consistent or not. As shown in Figure 2, the actual model of the retainer ring is not completely an axisymmetric shape because there is a groove. However, when analyzing with a full 3D model, the displacement value of the wafer at the same distance from the center of the wafer is not constant, as shown in Figure 8. Therefore, in order to obtain meaningful data, it is required to extract the data in a circumferential direction, as show in Figure 8, and perform an arithmetic mean.