## 4 Fatigue Life Estimation
### Elastic/Plastic Analysis and Verification  
The FE model of welded A-type frame was generated using HYPERMESH software to estimate the lifetime under its force time history. The frame structure made up of front plates and back plates was meshed with 83,648 solid elements, including 81,907 C3D8 and 1741 C3D6. The average length of the meshed elements was 2 mm. The cracked region of the weld seam was endowed with gradual meshing, as shown in Figure 19. The connection site between A-type frame and suspension (marked as A5 in Figure 19) was constrained with all degrees of freedom. The connection sites between A-type frame and frame (marked as A1 in Figure 19), right and left steering cylinder (marked as A3 and A2 in Figure 19), and front stabilizer bar (marked as A4 in Figure 19) were applied with the simulated force obtained from the multi-body dynamics analysis, respectively. The material properties for elastic/plastic finite element analysis were based on the cyclic characteristics, according to the parameters listed in Table 3. The Von-Mises stress contour of the welded A-type frame under the downhill and turning road surface condition is shown in Figure 20. The maximum stress was at the bottom corner between right front plate and back plate, which was close to the actual failure position. The critical regions at the bottom and top corner between front plate and back plate all had high stress levels as well.  
Figure 17: Multi-body dynamics model for downhill and turning condition.  
Figure 18: Force time history of welded A-type frame: (**a**) connection site between A-type frame and front stabilizer bar; (**b**) connection site between A-type frame and frame.  
To verify the finite element model, the strain measurements were conducted by using strain gauge rosettes under the downhill and turning road surface condition. The measuring points were considered as potential high stress ones, shown in Figure 21; the local strain gauge layout at measuring point A1-2 is displayed in Figure 22. Then, the tested principal stresses were compared with the simulated results, which were calculated from the measured strain values as the following equation:  
\[\sigma_{1,2}=\frac{E}{2(1-\mu)}(\varepsilon_{0^{{}^{\circ}}}+\varepsilon_{90^{{} ^{\circ}}})\pm\frac{E}{\sqrt{2}(1+\mu)}\cdot\sqrt{\left(\varepsilon_{0^{{}^{ \circ}}}-\varepsilon_{45^{{}^{\circ}}}\right)^{2}+\left(\varepsilon_{45^{{}^{ \circ}}}-\varepsilon_{90^{{}^{\circ}}}\right)^{2}} \tag{3}\]  
where \(\sigma_{1,2}\) are the principal stress, \(E\) and \(\mu\) are Yong's modulus and Poisson's ratio, and \(\varepsilon_{0^{{}^{\circ}}}\), \(\varepsilon_{45^{{}^{\circ}}}\), \(\varepsilon_{90^{{}^{\circ}}}\) are the strain components along the three directions of the strain rosette.  
Figure 19: Finite element model of welded A-type frame.  
Figure 20: Von-Mises stress contour of welded A-type frame, units in Pa.  
The simulated principal stresses could then be obtained from finite element analysis, which were compared with the experimental results, listed in Table 4. From the comparison, it was clearly seen that the finite element analysis results agreed well with the tested ones. Most of the relative errors were less than 10%, which is acceptable in engineering structure simulation.