34-76 The hydrodynamic performance prediction of ship hull with propeller and rudder
The hydrodynamic performance prediction of ship
hull with propeller and rudder
SHEN Hai-long，GOMRI Abdelhak，QIN Zai-bai，SU Yu-min，PANG Yong-jie （National Key Laboratory of Science and Technology on Autonomous Underwater Vehicle, Harbin
Engineering University, Harbin 150001, China）
Abstract：In the present study, we conducted ship’s resistance and propulsion performance, using computational fluid dynamics techniques, where a Reynolds-averaged-Navier-Stokes equations (RANSEs) solver was employed. The principal aim of the study is to verify the ability of a CFD method, to predict the hydrodynamic performances of a ship hull appended by propeller and rudder. The complexity in the mesh generation is one of the main obstacles for CFD. For convenience of mesh generation, unstructured meshes were used in the region around ship hull, propeller, and rudder, where the domain's shape is formed of delicate curved surfaces. On the other hand, structured meshes were generated for the rest of the domain. Following a hybrid mesh generation approach, prismatic cells have been generated in the boundary layer, where viscous phenomena are dominant，and tetrahedral cells in the remaining regions. The SST k-w model has been employed for turbulence closure using the steady-rotating reference frame source terms. Thrust and torque forces, pressure and velocity distributions were used to analyze the computed flow field. The hydrodynamic performance prediction method was gotten and was validated. The computational results were validated by comparing with the existing experimental data.
Key words: computational fluid dynamics; turbulence model; mesh; interaction of ship with propeller and rudder; resistance oefficient
1 Introduction
The flow past a ship hull with propeller and rudder is one of the most challenging problems in the computational fluid dynamics. Various numerical simulation approaches (boundary elements, panel methods, etc.) for studying ship, propeller, and rudder geometries, have been used for decades, but only recently, due to the rapid advances in computer power and in the parallelization capabilities, different CFD methods, and in particular RANS equation solvers, are increasingly applied to simulate the full three-dimensional viscous and turbulent flow for various ship geometries [1, 2].
In the last few years, computational analysis of ship resistance and propulsion using CFD is being widely adopted. The results are being applied to actual design of ships [3-6]. In those applications, however, the difficulty in mesh generation is the most serious obstacle for non-expert users for utilizing CFD with maximum efficiency. In case of mesh generation around a ship hull, the bow and stern regions require special care and experience because of the delicate and rapidly changing surfaces. Therefore, a hybrid meshing approach using unstructured meshing near the complex geometry and structured meshing in the remaining simple geometry domain was suggested[7]. The use of unstructured mesh is suitable for improvement of accuracy and for future extension to complex flows, and for investigation of the hull-propeller-rudder interaction [8-10].
In the present study, we have focused on the hydrodynamic performance prediction of the interaction hull-propeller-rudder using hybrid meshing. The present computational results were investigated through comparison with the experimental data from Shanghai Merchant Ship Design & Research Institute [11].
2 Computational Model and Numerical Techniques
The ship model test for the 57 000 t bulk-cargo ship, named SM0637-1, was carried out in China Ship Scientific Research Center. The design propeller model is named TM0782. The principal particulars for the ship and propeller are described in reference[11]. The shapes of the propeller and stern of ship hull shows in Fig. 1.
The commercial CFD software FLUENT version 6.3 is utilized for the computations in the present study. FLUENT solves the RANS equations with a finite-volume approach on hybrid unstructured grids. A variety of pressure-based algorithms are available in FLUENT. For the present steady-state computations, the SIMPLE algorithm is adopted. The difference schemes of convection terms in the momentum transport and pressure-velocity coupling used for discretizing the equations are discussed. The SST k-w model with wall functions is used for turbulence modeling. The resulting system of equations is solved using an algebraic multigrid method for faster convergence.
Fig.1 The shapes of the propeller and stern of ship hull Fig.2 Calculation mesh
3 Computational Meshes
The computational domain for the whole model includes two parts. One part is stationary which include ship hull and rudder. The other part rotates around the propeller axis which includes the propeller. The interfaces of the two parts are dealt with sliding mesh technique. The computational mesh generation method is presented in reference [12].
Fig.2 represents the calculation mesh of hull with propeller and rudder. The propeller is located in the blue volume and the volume itself rotates with non-conformal interfaces placed between the rotational and stationary sub-domains. Fig. 2 also illustrates the partition of the structured and unstructured mesh around the whole model. The green mesh is the surface mesh of hull and rudder in figure 2. The hybrid grid generation process of stationary part is as follows. First, the surface of the ship and rudder is triangulated, and then a boundary layer mesh is fitted all around it. The spacing of the nearest grid cells are such that it is consistent with the wall function formulation. The computational domain is then meshed with tetrahedral shaped cells in the core, which is surrounded by hexahedral cells in the rest of the domain. Finally, a local grid refinement is applied around the stern and propeller disc to provide reasonable resolution of the most complex part of the fluid field. The hybrid grid generation process of revolving part is same as the stationary part. The total number of the cells for the computation was 5.07 million.
4 Numerical Prediction based on CFD Techniques
In this paper, the thrust and torque of propeller behind the ships are predicted by the method presented in reference [13]. The resistance coefficient of ship and pressure distribution is also predicted .The ship speed considered in this work is 14 knot, while the scantling draught is 12.8 meter.
4.1 Results of forces and torque
To predict thrust and torque forces of the propeller working behind ship hull in the upstream of the rudder, and to get more accurate resistance coefficient, we have done different calculations by changing the following parameters: under-relaxation factors, pressure-velocity coupling, discretization types, and turbulence specification methods. Table 1 summarizes some case's specifications.
Tab.1 Some specifications of different calculation cases
specifications Case Some
1 2nd order descritization, simple pressure-velocity coupling, intensity and length scale turbulence method
2 Standard pressure dscritization,1st order for others, simple pressure-velocity coupling, intensity and length scale turbulence method
3 Standard pressure dscritization,2nd order for others, coupled pressure-velocity coupling, intensity and length scale turbulence method
4 2nd order descritization, simple pressure-velocity coupling, intensity and viscosity ratio turbulence method
5 2nd order descritization, simple pressure-velocity coupling, intensity and viscosity ratio turbulence method, different under-relaxation factors
6 2nd order descritization, simple pressure-velocity coupling, intensity and viscosity ratio turbulence method, different under-relaxation factors
The experimental values of thrust, torque, and resistance coefficient are 830399.046 N, 571471.47N, 0.0025657 respectively. Table 2 represents the computational results for each case. From the table, it can be pointed out that the results are changing with the change of the parameters. The result of case 2 for thrust and torque is more accurate, while the error for the resistance coefficient is so big. In other hand, resistance coefficient for case 5 and 6 is more accurate. Thrust and torque for case 5 and 6 is also acceptable comparing with other cases. As a result, next steps of performance prediction will just concern the last case.
Tab.2 Results for different calculation cases
Error/% Resistance
coefficient Error/%
Torque/N.m
Case
Thrust/N Error/%
1 75
2 670.61 -9.
3 518 856.77 -9.2 0.003 229 861 7 20.65
2 780 740.58 -5.27 55
3 982.61 -2.5 0.00
4 813 308 2 46.69
3 751 996.88 -9.
4 519 888.32 -9.03 0.003 223 299 20.40
4 753 702.84 -9.23 519 044.73 -9.17 0.003 357 340 23.57
5 751 704.14 -9.48 498 217.23 -12.82 0.002 885 11.06
6 75
7 751.61 -8.7 499 380.14 -12.6 0.002 844 971 9.82
4.2 Prediction of pressure distribution
The pressure distribution on the ship hull and rudder with propeller is shown in Fig. 3. In order to comparing
the influence of the propeller on the pressure distribution , the pressure distribution on the ship hull and rudder without propeller is also shown in Fig. 4. As can be seen from the figure, the influence of the propeller on pressure distribution is obvious. The pressure distribution on the hull and rudder has changed. The rudder pressure distribution changes greatly because of the propeller suction disturbing the flow field. Two zones of high pressure
are observed close to the leading edge of the rudder. The high-pressure regions were caused by the swirl of the slipstream which hit the leading edge part and tip part of rudder. In these figure, the unit of the pressure is Pascal.
Fig. 3 Pressure distribution on the ship hull and rudder Fig. 4 Pressure distribution on the ship hull and rudder
with propeller without propeller Fig.5 and Figure 6 illustrate the pressure distribution on the face side and back side of the propeller. In Fig. 5
and Fig. 6, there is one zone of high pressure on every blade of the propeller which is observed close to the trailing edge of the blade. This high pressure zone is propitious to avoid blade cavitations. In these figure, the unit
of the pressure is Pascal.
Fig.5 Pressure distribution on the face side of propeller Fig.6 Pressure distribution on the back side of propeller
5 Summary
This paper discussed the applicability of CFD techniques to predict the hydrodynamic performance of the whole hull-propeller-rudder model. The results showed that though the complexity of the model and the difficulty
of the prediction, a good and efficient result can be gotten. With he help of CFD post-process software, which
have powerful display technique of the flow field around ship hull with propeller and rudder, the details of pressure distribution of ship with rudder and propeller are explored. The details could be used for studying the cavitations and erosion of blades and rudder.
The interaction mechanism and the matching performance will be the future work that can be explored from
the flow details of flow field using CFD post-process software. These could provide the theoretic basis and technique instructor for low resistance ship design and high efficiency propeller design which have well matching performance.
Acknowledgements:This paper is supported by National Natural Science Foundation of China (51009038).
References:
1 M Abdel-Maksoud, F Menter, H, Wuttke. Viscous flow simulations for conventional and high-skew marine
propellers. Ship Technology Research,45,1998:64–71.
2 M, Stanier. The Application of ‘RANS’ Code to Investigate Propeller Scale Effects. 22nd Symposium on
Naval
Hydrodynamics, 1999 : 222–238.
3 Jasak H.. OpenFOAM: Open Source CFD Research and Industry. International Journal of Naval Architecture
and Ocean Engineering, 2009,1(2):89-94.
4 Kim M-C, Park W-G, Chun H.-H, Jung U.-H. Comparative Study on the Performance of POD Type Waterjet
by Experiment and Computation. International Journal of Naval Architecture and Ocean Engineering, 2010, 2(1):1-13.
5 Seo D W, Lee S.-H, Kim H, Oh J K. A Numerical Study for the Efficacy of Flow Injection on the Diminution
of Rudder Cavitation. International Journal of Naval Architecture and Ocean Engineering, 2010, 2
(2):104-111.
6 Yang J, Rhee S H, Kim H.. Propulsive Performance of a Tanker Hull Form in Damaged Conditions. Ocean
Engineering, 2009,36( 2):133-144.
7 Lee J H, Park B J, Seol D M, Rhee S H, Jun D S, Chi H R, Ryu M C.. Hybrid Meshing Approach for
Resistance Performance Prediction of a POD Propulsion Cruise Ship. Proc. of ASCHT09, 2nd Asian Computational Heat Transfer and Fluid Flow,2009.
8 S H Rhee, and S Joshi. CFD Validation For A Marine Propeller Using An Unstructured Mesh Based Rans
Method. Proceedings of FEDSM’03, 4th ASME-JSME Joint Fluids Engineering, Summer Conference.2003.
9 S H Rhee, E Koutsavdis. Two-dimensional simulation of unsteady marine propulsor blade flow using dynamic
meshing techniques. Computers Fluids 34, 2005 :1152–1172.
10 T Watanabe, T Kawamura, Y Takekoshi, M Maeda, S H Rhee. Simulation of Steady and Unsteady Cavitation
on a Marine Propeller Using a RANS CFD Code. 5th Int. Symposium on Cavitation. paper GS-12-004.
11 Y liang-mei, C chang-yi, L xi-wu, X chang-sheng. Model test report for the 57000t bulk-cargo ship No:
07307 CSSRC,2007.10.30
12 SHEN Hai-long, SU Yu-min. Study of mesh partition methods for numerical simulation of flow field of full
form ships.Journal of Harbin Engineering University, 2008, 29(11):1190-1198.
13 SHEN Hai-long,SU Yu-min.Study on the interaction between ship hull and propeller based on sliding mesh
technique. Journal of Harbin Engineering University, 2010,31(1)：1-7.