Journal of Mechanical Science and Technology 27 (6) (2013) 1597~1601 www.springerlink.com/content/1738-494x
DOI 10.1007/s12206-013-0405-3
Numerical simulation investigation on centrifugal compressor performance of turbocharger† Jie Li1,*, Yuting Yin2, Shuqi Li3 and Jizhong Zhang3 1
State Key Laboratory of Hybrid Process Industry Automation System and Equipment Technology, Automation Research and Design Institute of Metallurgical Industry, China Iron & Steel Research Institute Group, Beijing, 100081, China 2 China North Engine Research Institute, Datong, 037036, China 3 Science and Technology Diesel Engine Turbocharging Laboratory, Datong, 037036, China (Manuscript Received November 23, 2012; Revised February 27, 2013; Accepted March 4, 2013)
----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
Abstract In this paper, the mathematical model of the flow filed in centrifugal compressor of turbocharger was studied. Based on the theory of computational fluid dynamics (CFD), performance curves and parameter distributions of the compressor were obtained from the 3-D numerical simulation by using CFX. Meanwhile, the influences of grid number and distribution on compressor performance were investigated, and numerical calculation method was analyzed and validated, through combining with test data. The results obtained show the increase of the grid number has little influence on compressor performance while the grid number of single-passage is above 300,000. The results also show that the numerical calculation mass flow rate of compressor choke situation has a good consistent with test results, and the maximum difference of the diffuser exit pressure between simulation and experiment decrease to 3.5% with the assumption of 6 kPa additional total pressure loss at compressor inlet. The numerical simulation method in this paper can be used to predict compressor performance, and the difference of total pressure ratio between calculation and test is less than 7%, and the total-to-total efficiency also have a good consistent with test. Keywords: CFD; Compressor; Turbocharger; Performance ---------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------Table 1. Parameters of the compressor in this paper.
1. Introduction Centrifugal compressor as the main components of turbochargers has indirectly influences to engines performances. Thus the simulation on centrifugal compressors performance is becoming increasingly important. It is difficult to obtain the flow detail in compressor from 1 D performance forecast, and many other forecast methods have been studied before [1-4]. Those methods used in 20 century 1960s~1970s were build base on the test data, and classify the impeller losing factor like impeller load losing, circumfluence losing and surface friction losing etc. In present year, due to the development of computer and numerical method, impeller machine internal flow field numerical simulation has make a great progress, and make a great contribution to improve the design level and design periods; It is complexity and difficulty to measure the impeller internal flow fields, so the CFD revise case is very little in the published paper. Therefore, 3-D numerical simulation on centrifugal
Size
Name
Size
Dia.of impeller inlet flange
Name
100/mm
Backswept angle of impeller outlet
-30°
Blade angle of impeller inlet
-68°
Dia.of diffuser outlet
225/mm
Dia.of impeller outlet
140/mm
Width of diffuser outlet
7.5/mm
Width of impeller outlet
8.4/mm
compressor performance of turbocharger is investigation base on existence research. Inter-stage pressure measurement investigation of transonic centrifugal compressor was studied before [5]. Combined with the test data, gridding sensibility of a compressor was studied firstly; then forecast method was validated and mass-flow, pressure ratio of characteristic parameter revised method was formed.
*
Corresponding author. Tel.: +86 01062185820, Fax.: +82 01062185710 E-mail address:
[email protected] This paper was presented at the ISFMFE 2012, Jeju, Korea, October 2012. Recommended by Guest Editor Hyung Hee Cho © KSME & Springer 2013
†
2. Model, computational grid, boundary conditions and settings Table 1 is parameters of the compressor in this paper. Be-
1598
J. Li et al. / Journal of Mechanical Science and Technology 27 (6) (2013) 1597~1601
Table 2. Settings and boundary conditions. Settings
Boundary conditions Pressure and temperature
Fluid
Air ideal gas
Inlet
Turbulence
K-epsilon
Outlet
Pressure
Advection scheme
High resolution
Wall
Adiabatic and no slip
Heat transfer
Total energy
Rotating domain
Turbocharger speed
Fig. 2. Comparison of CFD results with experimental results.
and inlet boundary condition of inlet air sub-velocity of sound was presented. Outlet average-static pressure was presented and mass-flow was presented when approach to surge [6-10]. 2.1 Model validation and analysis As shown in Fig. 2, a comparison between experimental results and the results obtained from 3D CFD computations. As a result of the CFD simulations are based on theoretical CAD data with low grid numbers and conditions that does not necessarily perfectly match the real component produced, the curves of calculation results are higher than the experimental results. The differences between simulation and experiment are occurred, but in the error range the model can be used to forecast the compressor performance.
3. Results and discussions 3.1 Gridding sensibility study Fig. 1. Single passage model.
cause of the impersonally conditions, we cannot simulate the whole stage including impeller, diffuser and volute to forecast compressor performances. In this regard, main blade and splitter blade passage that is single-passage was selected as calculation region. As shown in Fig. 1 there are 3 parts including inlet of 2 times impeller width, rotating impeller and outlet diffuser. The grid in Fig. 1 was generated by using turbo-grid, and the grid number is 50000. The compressor mathematical model is based on the following simplifying assumptions. Take no account of the heat transfer between gas and solid. The boundary conditions are smooth wall with no slip and adiabatic. The inlet air is idea gas and periodicity flow in the impeller and gas density changes comply with ideal gas equation of state. Inlet total temperature (298 K), total pressure (1 standard atmosphere)
As known to all, in simulation fields, grid numbers and distribution have a great influence to the results. Irrationality of grid distribution and number may lead to bad results, and too many grids may need a long time to get results. Thus, to obtain a suitable grid number grade, we study the influences of grid number to the numerical calculation results. To generate the mesh using the ANSYS Turbo-GridTM element count and size method is used by author. Three different girds are plotted to analyze the influence of grid to compressor as shown in Table 3. As shown in Fig. 3, while the total grid number is 300000 above, there is little difference in pressure ratio and efficiency between different grid numbers, the compressor characteristic of pressure ratio and efficiency almost keep invariableness. The maximum difference of pressure ratio between different grid numbers is 8‰, the mass flow is12‰ and the efficiency is 7‰. Thus, to save the calculation time and effective using the computer resources, the total grid number is 300000 above of a single passage can meet the calculation requirement.
J. Li et al. / Journal of Mechanical Science and Technology 27 (6) (2013) 1597~1601
1599
Table 3. Grid numbers and distribution. HJG-I
HJG-II
HJG-III
Sort
Main blade
Splitter blade
Main blade
Splitter blade
Main blade
Splitter blade
Circumference
12
12
24
24
24
24
Radial
25
--
25
--
50
--
Impeller front
9
12
18
24
18
24
Impeller back
5
5
10
10
10
10
Impeller
24
21
48
42
48
42
O grid
10
--
10
--
20
--
Clearance
8
--
8
--
16
--
Upstream
--
13
--
26
--
26
Downstream
--
24
--
48
--
48
Total grid number
92562
306316
740832
Fig. 4. Comparison of CFD results with experimental results by increasing the grid number to 320000.
Fig. 5. Comparison of CFD results and experimental results by using the assumption.
3.2 Revising of numerical method
Fig. 3. Comparison of CFD results with different gird number.
Compared with Fig. 2 the grid number of Fig. 4 is increased to 320000, and the CFD results are better than the results in Fig. 2, the curves are more close to the experimental results.
Fig. 4 shows a comparison between experimental results and the numerical results obtained from CFD computations. In Fig. 4 it is obvious that pressure ratio and mass flow from numerical results are different from test bench data. Thus we make the following assumption, the adiabatic and no slip boundary settings lead to the efficiency, pressure ratio and mass flow is higher than test results. We can decrease the inlet total pressure to minimize the difference, based on the assumption. We recalculate the model, at the condition of 70000 r/min with the total pressure loss of 6 kPa. As shown in Fig. 5, the mass flow near choke line is consisting well with the test results, the maximum difference of the impeller inlet static pressure is 10%, the outlet static pressure is 9% and the diffuser outlet is 3.5%. Thus, from the compare, author in this paper modified the numerical calculation pressure ratio expression as follows,
1600
J. Li et al. / Journal of Mechanical Science and Technology 27 (6) (2013) 1597~1601
Fig. 7. Comparison of CFD results and experimental results by using the new method for a new mode.
Fig. 6. Comparison of CFD results and experimental results by using the new method for the compressor.
PRcor
PRcal = ζ pr
Fig. 8. Comparison of CFD results and experimental results by using the new method for a new mode.
(1)
4. Conclusions
ζ pr = 5.1×10−9 U 23 − 4.8 ×10−6 U 22 + 1.7 ×10−3U 2 + 0.836
(2) where PRcal is total-to-total pressure ratio of diffuser outlet from calculation, PRcor is total pressure ratio of the compressor form forecast; ζPr is pressure revision coefficient, U2 is velocity of the impeller outlet. As shown in Fig. 6, by using the pressure ratio revision expression, the numerical results are consisting well with the test bench data. The maximum difference of the numerical pressure ration compared with test data is 7%, and near the surge zone. Mostly the difference is less than 3%. The numerical efficiency is consisting well with the test bench data. 3.3 Verification of the numerical calculation revision method In this paper the verification model is a new compressor, by using the pressure ratio revision expression and 6 kPa loss of the impeller inlet. As shown in Figs. 7 and 8. The difference of the presser ratio between the test bench data and the calculation results of the new compressor is less than 3%. The difference of the efficiency is less than 1%.
In the present work, CFD model was build and validated. Base on the simulation results, it can be concluded that: (1) While the grid number of single-passage is 300000 above, the increasing of the grid number has little influences on the numerical results of the compressor performance. (2) Supposing that 6 kPa additional total pressure loss at compressor inlet, the numerical calculation mass flow rate of compressor choke situation has a good consistent with test results. The maximum difference of the diffuser exit staticpressure between simulation and experiment decrease 3.5%. (3) Based on CFX, the simulation method and calculation rule in this paper can be used to calculate the designed compressor performance. The difference of pressure ratio be-
tween calculation and test is 3%~7%. The calculation efficiency has a good consistent with test results. Acknowledgment This work supported by National Key Basic Research and Development Program (“973” Plan) of China (NO. 2012CB724304). The authors show their gratitude to Science and Technology Diesel Engine Turbocharging Laboratory for
J. Li et al. / Journal of Mechanical Science and Technology 27 (6) (2013) 1597~1601
investigation assistance.
References [1] L. Shu-qi and Z. Jun-yue, Two-zone modeling method for performance prediction of centrifugal compressor, Chinese Internal Combustion Engine Engineering, 30 (3) (2009) 7579. [2] L. Rui-tao and X. Zhong. The research development of internal flow in centrifugal turbomachinery, Advances in Mechanics, 33 (4) (2003) 518-532. [3] L. Xiao-yu and B. Yu-hua, CFD analysis on air compressor interior flow field of turbo supercharger, Small Internal Combustion Engine and Motorcycle, 36 (5) (2007) 12-14. [4] M. Chao-chen and Z. chen, Alculation and analysis of the outflow field of the adjustable inlet equipment on a compressor, Transactions of Beijng Institute of Technology, 23 (2004) 97-99. [5] L. Shu-qi and Z. Jun-yue, Inter-stage pressure measurement investigation of transonic centrifugal compressor, Chinese Internal Combustion Engine Engineering, 31 (2) (2010) 5358. [6] Y. Wang and Z. Luo, Simulation and performance analysis
1601
on centrifugal compressors of different dimensions and variable operation speed, IEEE 978-1-61284-459-6/11/ (2011). [7] R. A. tog and A. M. Tousi, Design and CFD analysis of centrifugal compressor for a microgasturbine, Aircraft Engineering and Aerospace Technology, 79/2 (2007) 137-143. [8] D. Japikse, Centrifugal compressor design and performance, Vermont USA: Concepts ETI, Inc. (1996). [9] M. V. Herbert, Method for performance prediction of centrifugal compressor. NGTE memorandum, 78029 (1978). [10] S. Ibaraki, T. Masuo and H. Kuma et al., Aerodynamics of a transonic centrifugal compressor impeller, Trans ASME Journal of Turbomachinery, 125 (2003) 346-351.
Jie Li is an engineer at state key laboratory of hybrid process industry automation system and equipment technology. He received his Master Degree in Refrigeration and Cryogenic Engineering (CFD analysis) from Northeastern University in China and has worked for CNEI as a staff engineer to design impeller with CFD analysis. His research interests include thermodynamics, system energy conversion model and CFD analysis.
