## 3 Results  
### Formation Analysis  
To verify the molding performance of this successive partial rubber-bulging method, an FEM analysis model was used for a formation simulation, as shown in Figure 8. The model comprised three parts: a cylindrical rubber piece, the cylindrical material, and the mold. The rigid body model was applied to the mold, the Mooney-Rivlin material model [20] was applied to the cylindrical rubber tube, and the elastoplastic material model was applied to the cylindrical tube. The explicit finite element code Abaqus was used to simulate the experimental process. In the simulation, the cylindrical rubber piece was placed into the cylindrical tube and the mold was placed on the outside of the tube. The tube wall was meshed using four-node curved S4R shell elements. The relationship between the tube and the rubber and mold was defined using'surface-to-surface' contact. A hard contact was applied to the column wall to avoid interpenetration of the folding generated during axial compression. The dynamic and static coefficients of the friction coefficients of the contact surface of each part were set to 0.2 and 0.15. The load condition for molding was referenced with respect to that read from the pressure gauge of the manual hydraulic jacket during the actual processing, as shown in Figure 6; a load of 100 kN was uniformly applied from both ends of the cylindrical rubber tube. Several simulations were first run to conduct a convergence test, and finally an element size of 2 mm was determined due to its acceptable accuracy and computational cost. The total number of nodes in the analysis model was 141,368 and the total number of elements was 54,477.  
The true stress-plastic strain curve of the STKM11A was obtained by processing data from the experiment, as shown in Figure 9. The properties of the CAP are as follows: density \(\rho\) = 7800 kg/m\({}^{3}\), [PERSON]'s modulus E = 213 GPa, [PERSON]'s ratio \(\
u\) = 0.3, yield stress 270 MPa, and ultimate stress 295.8 MPa.  
\begin{table}
\begin{tabular}{c c c} \hline
**Lock Load** & **Compression Load** & **Rubber Height** \\ \hline
20 KN & 100 KN & \(\omega\) 50 \(\pm\) 0.2 mm \\ \hline Rubber diameter & Rough bar height & Rough bar diameter \\ \hline \(\omega\) 48 \(\pm\) 0.2 mm & \(\omega\) 55 \(\pm\) 0.1 mm & \(\omega\) 48.2 \(\pm\) 0.1 mm \\ \hline \end{tabular}
\end{table}
Table 1: Technological Parameters of Manufacture.  
Figure 8: Model used for finite-element simulation of the CAP.  
The thickness distribution of the formed tube along the axial direction of the CAP is shown in Figure 10. The red line represents the simulation results, and the blue line denotes the experimental results; the \(\odot\) and \(\Delta\) symbols represent the respective thickness measurement points. In the rubber-bulging method, five samples were manufactured to measure the thickness using an outer dial caliper gauge (BO type) with an accuracy of 0.025 mm, and the average of these tests was taken. The numerical simulation values were very consistent with actual measured values: for the smallest wall thickness, which occurred in the center of a protrusion, the numerical simulation gave a value of 1.083 mm, and the actual measured value was 1.090 mm. Relative to the wall thickness of 1.20 mm before forming, the calculated maximum thinning rate was \((1.20-1.09)/1.20=10.1\%\). This result proved that this successive partial rubber-bulging method is reliable for the processing of the CAP [32; 33].  
Figure 10: Modelled and measured thickness distributions of the formed CAP.  
Figure 9: Model used for finite-element simulation of the CAP. (**a**) geometry of specimen (**b**) geometry of specimen for test.