- About this Journal ·
- Abstracting and Indexing ·
- Aims and Scope ·
- Annual Issues ·
- Article Processing Charges ·
- Articles in Press ·
- Author Guidelines ·
- Bibliographic Information ·
- Citations to this Journal ·
- Contact Information ·
- Editorial Board ·
- Editorial Workflow ·
- Free eTOC Alerts ·
- Publication Ethics ·
- Reviewers Acknowledgment ·
- Submit a Manuscript ·
- Subscription Information ·
- Table of Contents

Advances in Mechanical Engineering

Volume 2013 (2013), Article ID 428416, 8 pages

http://dx.doi.org/10.1155/2013/428416

## Finite Element Analysis Design of a Split Rotor Bracket for a Bulb Turbine Generator

^{1}State Key Laboratory of Hydroscience and Engineering, Department of Thermal Engineering, Tsinghua University, Beijing 100084, China^{2}Toshiba Hydro Power (Hangzhou) Co., Ltd, Hangzhou 310016, China

Received 16 February 2013; Revised 27 April 2013; Accepted 18 May 2013

Academic Editor: Tinh Q. Bui

Copyright © 2013 Yongyao Luo et al. This is an open access article distributed under the Creative Commons Attribution License, which permits unrestricted use, distribution, and reproduction in any medium, provided the original work is properly cited.

#### Abstract

The rotor bracket is a key component of the generator rotor with cracks in the rotor bracket leading to rubbing between the rotor and stator, which threatens safe operation of the unit. The rotor rim is so complicated that the equivalent radial stiffness of rim was determined by numerical simulation other than engineering experience. A comprehensive numerical method including finite element analyses and the contact method for multibody dynamics has been used to design the split rotor bracket. The com-putational results showed that cracks would occur in the initial design of the bracket when the turbine operated at the runaway speed, and the bracket design should be improved. The improved design of the bracket was strong enough to avoid cracks and rub between the rotor and stator. This design experience will help improve the design of split rotor brackets for bulb turbine generators.

#### 1. Introduction

Bulb turbines are widely used in low-head (less than 20 m) hydropower stations since they can operate over a wide range of heads with high efficiencies. Unlike the Kaplan or Francis turbines, a bulb turbine has a horizontal shaft, as shown in Figure 1. The runner is driven by water flow, and the main shaft as well as the rotor rotates with the runner. Then electricity is generated by cutting magnetic field lines. The rotor bracket is a key component of the generator rotor which is loaded with electromagnetic, centrifugal, and gravitational forces during operation. Cracks in the rotor bracket can lead to rub between the rotor and stator which will threaten safe operation of the unit as shown in Figure 2. Bulb turbine generator unit has more possibility to rub between the rotor and stator because of horizontal shaft. Rotor bracket cracks have attracted limited attention. Based on the cracks in rotor bracket, Shen et al. [1] performed stress analyses of a single bulb turbine rotor bracket with cracks to improve the original design. The dynamic stresses in a rotor bracket of a bulb turbine were measured by Wen et al. [2] with the results compared with simulation results. Chen studied the causes of a bulb turbine rotor bracket crack [3]. Li et al. found the reason of a rotor bracket cracks by finite element analysis and improved the initial design [4].

With the increasing unit output and turbine size in recent years, split rotor brackets are being widely used to facilitate manufacturing and transport, so the rotor bracket strength has become more of a concern. The generator rotor system is a complex multibody system including the main shaft, rotor bracket, rim, rim key, magnetic poles, radial sausage pin, and bolts as shown in Figure 3. The rim connects to the bracket through an interference fit with the rim keys. So it is very hard to simulate such a complex multibody system using traditional method. With the development of finite element analysis technology, it is possible to perform the design in ANSYS using the contact methodology [5]. Luo et al. [6] optimized the upper bracket of extremely high-head Francis hydrogenerator to successfully eliminate the resonance due to rotational vibrations using ANSYS. Hyder and Asif [7] optimized the location and size of the opening in a pressure vessel cylinder with ANSYS with good results. Peng et al. [8] optimized the design of a large dredge pump case using a finite element analysis with the predicted pump case distortion in the axial direction agreeing well with test results. But few studies have analyzed the stresses for the complex multibody system of a generator rotor. Contact methodology is an advanced function in ANSYS software, through which we can establish the finite element model for the multibody mechanism of the generator rotor to perform the calculation. In this paper, a bulb turbine generator rotor system was modeled using the contact methodology, and the equivalent Young’s modulus of the rim was obtained by simulation other than engineering experience. A preliminary design of the rotor bracket was improved to avoid cracks and rub between the rotor and stator.

#### 2. Determination of the Equivalent Young's Modulus for the Rim

The rim is made up of layers of 4 mm thick laminated rim-sheets, as shown in Figure 4. Each layer has 13 rim-sheets to go around the entire circumference with four poles in each rim-sheet. There are a total of 428 layers with each four layers of rim-sheets staggered such that they form a complete cycle in each of the 13 sections. Thus, there are a total of 5564 rim-sheets in the rim with 260 drag bolts to pull them together. The rim is so complicated that the model must be simplified with an equivalent radial stiffness. In this paper, the equivalent radial stiffness of rim was determined by numerical simulation other than engineering experience, which was rarely reported in the previous literature. The numerical theory was as follows.

The stresses were calculated using the finite element analysis based on the displacement method. The force equilibrium equation is where is the stiffness matrix, is the nodal displacement vector, and is the load vector on the nodes. The displacements, , found by solving (1) are then used to calculate all stresses by (2): where is the elastic matrix based on Young’s modulus and Poisson’s ratio for the material and is the strain-displacement matrix based on the element shape functions.

Many experimental results showed that the fourth-order strength theory could suitably describe yielding of plastic materials such as steel, copper, and aluminum. Therefore, it is applied universally in engineering analyses such as to analyze the stress characteristics of a rotor bracket. The Misses stresses can then be calculated from the fourth-order strength result as follows [9]:

Four layers of rim-sheets for 1/13 of the circumference as shown in Figure 5 were modeled to determine the equivalent radial stiffness with the four layers of rim-sheets held together by drag bolts that were modeled using the contact method to generate the simplified model as shown in Figure 6.

The material of the rotor is steel with the properties listed in Table 1. Application of the equivalent centrifugal force generated at the same rotational speed gave the radial displacement distributions shown in Figures 7 and 8.

The radial displacements at the rim key fitting face were used to calculate equivalent Young's modulus. The radial displacement at the rim key fitting face was 10.86 mm before simplification as shown in Figure 7 and 6.89 mm after simplification as shown in Figure 8. Thus, equivalent Young's modulus of the rim after simplification can be determined by (Pa) with the simplified rim shown in Figure 9 and equivalent Young’s modulus of the rim reduced by 37% compared with general steel. In general engineering experience, a reduction of 25% for equivalent Young’s modulus of the rim is adopted because it is hard to measure the actual value in field test.

#### 3. Strength Analysis of the Initial Rotor Bracket Design

The computational model included the main shaft, rotor bracket, rim, rim key, radial sausage pin, and bolts, as shown in Figure 10. The two splits in the bracket are tightened together with pretensioned bolts. Radial sausage pins and pretensioned bolts are used to connect the main shaft with the bracket. The rim connects with the bracket through the interference fit with the rim keys, with an initial interference fit of 1.2 mm, which is large enough to avoid a clearance between the rim and rim key at the runaway speed.

The rated speed of the turbine is 115.4 rpm and the runaway speed is 380 rpm. The radius of the magnetic pole centroid is 2.8 m, so the ratio of the gravitational and centrifugal forces on the magnetic pole is 1 : 41.7 at the rated speed and 1 : 458 at the runaway speed. Thus, the gravitational force is so small compared with the centrifugal force that the gravitational force on the magnetic pole was ignored in the computations. The model was loaded with centrifugal force, gravitational force, radial magnetic pull, and magnetic torque at rated speed, with only centrifugal force and gravitational force at runaway speed because of zero output of the generator, as shown in Figure 10. Young's modulus of the simplified rim was 1.332e11 Pa, while Young's modulus of the other parts was 2.1e11 Pa. The computational model was meshed with hexahedral elements as shown in Figure 11.

The stress distribution in the bracket at rated speed shown in Figure 12 shows the stress concentration at the inner corner of the vent with a maximum stress of 171 MPa, which is lower than the yield strength of the material (230 MPa). The stress distribution in the bracket at runaway speed shown in Figure 13 has three stress concentration locations. The first stress concentration location is at the inner corner of the vent with a maximum stress of 387 MPa, which is close to the ultimate strength of the material (400 MPa), as shown in Figure 13(a). The second occurs at the ribs near the joint surface with a maximum stress of 567 MPa, which greatly exceeds the ultimate strength of the material, as shown in Figure 13(a). The last occurs at the bolted hole on the joint surface with a maximum stress of 450 MPa, which also exceeds the ultimate strength of the material, as shown in Figure 13(b). Thus, cracks would occur in the bracket when the turbine operated at the runaway speed, and the bracket design should be improved.

#### 4. Improved Design

The bracket structure was modified to eliminate the three stress concentration locations at the runaway speed. An analysis showed that the height and thickness differences in the ribs caused the stress concentration, so the height and thickness of the ribs near the joint surface were increased, as shown in Figure 14(a). Reinforced plates were also added to strengthen the joint surface, as shown in Figure 14(b). The area of the vents near the joint surface was also reduced to avoid excessive stresses, as shown in Figure 15.

The stress distribution in the improved bracket is shown in Figure 15, where the maximum stress concentration occurs at the radial sausage pin hole with a maximum stress of 342 MPa, which is lower than the ultimate strength of the material (400 MPa), so the improved bracket is safe even when the turbine operates at the runaway speed. The maximum stress at the inner corner of the vent reduced from 387 MPa to 252 MPa, at the ribs near the joint surface reduced from 567 MPa to 261 MPa, and at the bolted hole on the joint surface reduced from 450 MPa to 324 MPa, as shown in Figure 16. Therefore, the improved rotor bracket is much stronger than the initial one at the runaway speed.

#### 5. Dynamic Stresses in the Bracket at the Rated Speed

The turbine is normally operated at the rated speed, so the fatigue life of the improved bracket at the rated speed is an important criterion. The dynamic stresses in the bracket were computed to evaluate the bracket’s fatigue life at the rated speed. The stress distribution in the bracket at the rated speed is shown in Figure 17, where the maximum stress is 162 MPa, which is less than the material yield strength. The stress concentrations were monitored at the radial sausage pin hole at node number 543136 and the inner corner of the vent at node number 17781 since these had the maximum dynamic stresses.

The dynamic stresses were calculated by rotating the computational model 15° each time step, with the full cycle divided into 24 time steps. The stresses at nodes 17781 and 543136 were recorded at each time step. Time histories of the dynamic stresses at nodes 17781 and 543136 at the rated speed are shown in Figure 18, and the dynamic stresses in one cycle are sinusoidal in nature.

The mean dynamic stresses at nodes 17781 and 543136 were 142 MPa and 144 MPa, with amplitudes of 10 MPa and 21 MPa. The equivalent stress amplitudes were computed according to the Goodman formula [10] as follows: where is the amplitude of the dynamic stress, is the mean value of the dynamic stress, is the ultimate strength of the material, and is the equivalent stress amplitude.

The equivalent amplitude of the dynamic stress at node 17781 is 15.5 MPa and the equivalent amplitude at node 543136 is 32.8 MPa, which are both far less than the fatigue strength of the material (160 MPa), so the bracket would not fatigue at the rated speed.

#### 6. Conclusions

A bulb turbine generator rotor multibody system was modeled using the contact methodology. Equivalent Young’s modulus of the rim was obtained by simulation other than engineering experience, and equivalent Young’s modulus of the rim reduced by 37% compared with general steel. A preliminary design of the rotor bracket was improved to reduce the maximum stress in the bracket at the runaway speed from 567 MPa to 342 MPa, which is less than the ultimate strength of the material (400 MPa). The maximum stress in the new bracket was 162 MPa at the rated speed, which is less than the material yield strength (230 MPa). The maximum equivalent dynamic stress amplitude was 32.8 MPa at the rated speed, which is far less than the material fatigue strength (160 MPa). Thus, the bracket design is strong enough to avoid cracks and rub between the rotor and stator.

#### Acknowledgments

The authors thank the National Natural Science Foundation of China (no. 50979044), State Key Laboratory of Hydroscience and Engineering (Grant no. 2009T3), and Toshiba Hydro Power (Hangzhou) Co., Ltd, for supporting the present work.

#### References

- W. L. Shen, W. Chen, L. J. Bian, F. Yan, and G. P. Zhao, “The research of static state intensity and dynamic characteristic about rotor bracket of hydro-generator,”
*Modern Manufacturing Engineering*, vol. 12, pp. 54–56, 2005. - J. M. Wen, J. Q. Chen, and W. L. Shen, “The research of FEA and dynamic stress testing about rotor bracket of hydro-generator,”
*Mechanical Engineer*, vol. 3, pp. 61–63, 2007. - T. Y. Chen, “Reasons and repair for cracks of tubular turbine generator rotor bracket,”
*Fujian Hydro Power*, vol. 1, pp. 25–27, 2003. - Z. G. Li, F. Y. Yang, X. X. Pu, J. H. Chen, and G. L. Si, “Application of ANSYS in the hydraulic generator rotor bracket crack,”
*Applied Mechanics and Materials*, vol. 148-149, pp. 1058–1061, 2012. View at Publisher · View at Google Scholar · View at Scopus - S. Reh, J. Beley, S. Mukherjee, and E. H. Khor, “Probabilistic finite element analysis using ANSYS,”
*Structural Safety*, vol. 28, no. 1-2, pp. 17–43, 2006. View at Publisher · View at Google Scholar · View at Scopus - Y. Y. Luo, Z. W. Wang, G. D. Chen, and Z. J. Lin, “Elimination of upper bracket resonance in extremely high head Francis hydro-generators,”
*Engineering Failure Analysis*, vol. 16, no. 1, pp. 119–127, 2009. View at Publisher · View at Google Scholar · View at Scopus - M. J. Hyder and M. Asif, “Optimization of location and size of opening in a pressure vessel cylinder using ANSYS,”
*Engineering Failure Analysis*, vol. 15, no. 1-2, pp. 1–19, 2008. View at Publisher · View at Google Scholar · View at Scopus - G. J. Peng, Z. W. Wang, Z. G. Yan, and R. X. Liu, “Strength analysis of a large centrifugal dredge pump case,”
*Engineering Failure Analysis*, vol. 16, no. 1, pp. 321–328, 2009. View at Publisher · View at Google Scholar · View at Scopus - M. H. Yu,
*Engineering Strength Theory*, Higher Education Press, Beijing, China, 1999. - J. Goodman,
*Mechanics Applied to Engineering*, Longmans Green, London, UK, 1899.