Scholarly article on topic 'Simulation of Propeller - Hull Interaction Using Ranse Solver'

Simulation of Propeller - Hull Interaction Using Ranse Solver Academic research paper on "Mechanical engineering"

Share paper

Academic research paper on topic "Simulation of Propeller - Hull Interaction Using Ranse Solver"

Simulation of Propeller - Hull Interaction Using Ranse Solver

M.N. Senthil Prakash1 and V. Anantha Subramanian2

1Research scholar, email: 2Professor, email: Department of Ocean Engineering Indian Institute of Technology, Madras INDIA-600 036


This work simulates propeller-hull interaction effects by a novel method namely, coupling a Vortex Lattice Method (VLM) with a RANSE solver. The VLM generates the propeller forces based on the inputs of blade geometry, wake at propeller inlet, the required thrust and the propeller revolutions. The propeller forces thus obtained are distributed in the fluid domain at the propeller disk region at specific cells. These cells lie close to the blade coordinates and the forces are assigned to the centroids of cells by means of a user-defined function (UDF). The introduction of the body forces into the fluid domain, emulates the propeller action in the field of flow with consequent influences on the flow kinematics. Therefore the interaction effect between propeller and ship hull is simulated successfully by coupling the two methods. Thereby the kinematical aspects such as effective wake conditions are obtained. The results based on the methodology have been verified by comparison with data from the KCS ship available in recent published literature. The method establishes a successful numerical tank approach in understanding the ship hull-propeller interaction problem.

Keywords: Vortex Lattice Method; RANSE solver; User Defined Function (UDF) Propeller-hull interaction.


The assessment of performance of a propeller working near the ship hull is important in the design process. The well known interactive effects, mainly in the form of wake and thrust deduction fraction, are required to obtain the best geometry and to adapt the propeller to the actual working conditions. Traditionally physical modeling in towing tanks by means of self-propulsion tests has helped in establishing these characteristics for practical design purposes. In recent years, there has been steady progress in the use of numerical hydrodynamic tools (CFD) to simulate the flow past ships without and with the influence of propellers. The phenomenal growth in the speed of computational capability has brought this otherwise complex problem within the realm of numerical modeling and solution. The complexity arises due to the requirement of representing the rotating propeller with its continuous 3-D complex geometry near the ship hull. Recent research efforts have attempted the method of approach of directly modeling the propeller in the field of flow along with the ship hull in the computational domain. A rotating reference frame is used to simulate the action of the propeller. The iterative solution converges after several runs in order to stabilize the flow since the speed of the ship combined with the action of the propeller modifies the flow in the computational domain. Hence the simulation process tends to be computationally intensive. Dhinesh et al (2009).

The design and analysis of propellers is also performed by the vortex lattice method, which is a subclass of the lifting surface method. In this method (Kerwin & Lee 1978, Kerwin 1984), the continuous distribution of vortices and sources are replaced by a finite set of straight-line elements of constant strength whose ends lie on the blade camber surface. The method essentially gives the optimum distribution of pitch, camber and mean line offset at various radii. The above method can be combined

with the RANSE solver based inflow conditions to generate the body forces characteristic of the propeller. Therefore, the second approach combines the body forces associated with the propeller into the RANSE solver, thereby simulating the propeller action. This alternative method is useful as it combines design and analysis to describe the complex flow field.

By simulating the flow past the ship hull using the RANSE solver, the velocity distribution at the aft of the hull at the propeller inlet section can be estimated. This gives the inflow velocity field, which is also the wake field upstream of the propeller. Combining this wake field with the Vortex Lattice Method gives the necessary propeller body forces, which are used in the subsequent stage of RANSE simulation to represent the rotating propeller at the aft hull. To account for the transient effects created by the rotating propeller, the sub-domain representing the propeller swept volume is rotated at the propeller rpm, after applying propeller body forces at the blade coordinates, by using the rotating reference frame application of the RANSE solver. The introduction of the body force in RANSE results in modification of the velocity field and the updated body forces need to be determined and re-allocated in the fluid domain to continue the iterative procedure until there is no change in the velocity field. The simulation at this stage will give conditions ideal to the working propeller at the prescribed rpm and giving the required thrust behind the ship. This is the propeller - hull interaction. The coupling between the VLM and RANSE is therefore mutual viz., the propeller body force links VLM to RANSE and the velocity distribution from RANSE links it with VLM.


Application of the method here is demonstrated by the analysis of an existing propeller to simulate the propeller-hull interaction. The scheme involves the coupling of VLM with a commercial RANSE solver package, FLUENT. The methodology of implementation is described with reference to Fig. 1. There are two domains in the RANSE solver, the main domain around the hull and a sub-domain in the main domain for the swept volume of the propeller. The scheme is initiated by simulating the motion of bare hull in FLUENT to obtain the nominal wake distribution. The wake distribution is used to find the radial circulation distribution for a given thrust, rpm and geometry of the propeller. This radial distribution of circulation is applied in the VLM programme along with the wake distribution, advance coefficient, and the propeller geometry for deriving the thrust distribution over the blade geometry with the details of coordinates of the thrust distribution over the blade and induced velocity. The blade coordinates are now transformed to suit the coordinates in the main domain coordinate system. A User Defined Function (UDF) is now used to input the thrust values, modified as propeller body forces, into the sub-domain representing the propeller swept volume at the corresponding cell centroids close to the above coordinates. The UDF has in-built sub-routines to determine the centroid of the domain cell closest to the transformed blade coordinate, extract the volume of this cell, calculate propeller body force which is the ratio of the thrust to the volume of the cell, and put this body force back in to the corresponding cell centroid. To account for the transient effects created by the rotating propeller, the sub-domain is rotated at the propeller rpm using the rotating reference frame application of the RANSE solver. The RANSE solver is run with the UDF hooked and the modified velocity distribution at the propeller inlet section extracted, which will represent the updated wake in the presence of the working propeller (total wake). The effective wake at the propeller inlet for updating the propeller body force is found by subtracting the induced velocity from the total velocity. The updated body force is calculated by the VLM, and the RANSE is run iteratively until there is convergence in the circulation distribution. At this stage, the RANSE simulation will give the true working condition with realistic propeller rpm and thrust behind the ship, simulating the propeller-hull interaction. The example chosen is the KP505 propeller and the Korean Container Ship (KCS) (CFD Workshop Tokyo 2005).


Fig. 1 presents the flow chart of the algorithm in a block diagram. The upper part of the block diagram defines the method of obtaining the propeller thrust and torque invoking the design process of a wake aligned propeller blade. Based on the wake, the radial circulation distribution is obtained. By the

Figure 1. Flow chart for obtaining propeller-hull interaction

principles of the lifting surface method, the blade grid and the wake grid are generated and the velocities induced by the blade singularities and wake singularities are computed. Once wake alignment is achieved, the propeller related torque absorption and thrust delivered can be calculated. At this stage the results are coupled to the RANSE solver. Invoking the user-defined function subroutine, the cell specific thrust density values are allocated into the propeller swept volume sub-domain. Running the RANSE solver, gives the updated flow velocities under the influence of the propeller as represented through the body forces. The resulting updated wake distribution now enables to recalculate the circulation distribution as done in the first step. The propeller is thus iteratively improved for optimum performance.

Blade geometry

The parameters for blade geometry are given in Fig. 2. They are propeller diameter, number of blades, pitch, camber distribution, skew, rake and thickness distribution of the blade surface as mean line offset. The face and back of the propeller are obtained by adding half the thickness to the mean camber line on either side. The mean camber line for different radii will describe the blade mean surface.

The mid-chord line initiates the blade formation. The mean blade shape is a space curve defined parametrically by the radial distribution of skew, d (r), and rake, x (r). By advancing a distance ± c(r)/2 along a helix of pitch angle 0(r) passing through the mid chord line, one obtains the blade leading and trailing edge respectively. The blade mean surface may then be defined in terms of camber distribution f(r, s), where s is a non-dimensional curvilinear coordinate along the nose-tail helix which is zero at the leading edge and unity at the trailing edge.

The camberf, is measured in the plane of a cylinder of radius r at right angles to the nose-tail helix. Finally thickness t(r, s), is added symmetrically with respect to the mean line at each radius, again in a cylinder of radius r, and at right angles to f. The maximum values of f and t at a given radius are f0(r)

Mid chord line

t(s) \ /


Figure 2. Blade geometry description

and t0(r) and upon non-dimensionalization with respect to the chord c(r), are defined as the section camber and thickness ratios. The Cartesian coordinates of any point on the mean blade surface or on the actual blade surface are easily related to these functions.

Here cublic spline functions are used to represent the above-mentioned geometrical quantities. The coordinates are based on specified or computed values at a set of radial and chord wise stations. The number of radial stations as well as their spacing is chosen conveniently at say every 10% interval of radius with additional half stations at both ends. A fixed set of 17 chord-wise stations are used, as per NACA guidelines for section data interpolation.

Wake parameter

The presence of the hull upstream of the propeller affects the inflow to the propeller. The tangential, radial and axial components of the inflow velocity are obtained from the RANSE solver by simulating the flow past the hull. Application of the Biot - Savart law gives the induced velocity component Vinduced. To obtain the velocity input for the VLM, subtract the induced velocity Vinduced from the total velocity Vtotal ^^ V

' mflow = Vtotal - Vinduced. The inflow velocity is used to update the body force.

Circulation and the resulting forces

The radial distribution of circulation generates forces which contribute to the absorbed torque and generated thrust characteristics of the propeller blades. The radial circulation distribution is spread on to the surface lattice of the mean blade surface by proper interpolation in both span wise and chord wise directions.

The total propeller thrust and torque are obtained by integration of local forces over the blades. The approach used here is to derive the total fluid velocity at the midpoint of each span wise and chord wise vortex element by interpolation based on the velocities computed at the control points. Application of the Kutta - Jowkowski law will then yield a concentrated force on each vortex element normal to the blade surface and the force on each side of the element F side is given by

Fside = pU(x) X rside = Prside (U() X lside )

Where U(x) total velocity calculated at the midpoint of the panel side, lsue is the vector for each side rsde and is the total circulation on one side of the panel. Each blade having Msp number of panels in the span wise direction and Nch number of panels in the chord wise direction is replaced by vortex elements and the force calculation is done by adding the forces derived by individual elements in each panel by Eqn. 1. The contribution from all panels is given by Eqn. 2. Refer Fig. 3

T = F x =pZ £r

1+( m-1) Nch

" ch ^

I Kn I

n=1 k=1

z.n+(m-1)Nch .k y

Ly.n+(m-1 )Nch .kuz Uy ( X

Uy (xn+( m-1)Nch . k ) -

L „+^1 w . Uz (Xn+( m-1)Nch . k )


Uz (x1+(m-1)Nch.4)

lZ.1+(m-1)Nch.4Uy ( X 1+( m-1) Nch. 4 ) +

Where xi k is the coordinate of the mid point of side k of the panel i,Ux ( x ) x,y,z components of the velocity, ri is the circulation of the ith panel, Kn is the weight function and lxyzik is the x,y,z components of the vector lk on the mean blade surface. These forces, and their corresponding moment about the axis of rotation, may then be summed to obtain the total inviscid thrust and torque.

Q = -Mx = -zFy )i (3)

Tangential forces associated with viscous drag may be added to the existing force on each span wise vortex, with a magnitude proportional to an assumed drag coefficient, the elementary blade area and the square of the total velocity.

Coupling of VLM with RANSE solver

The Body forces representative of propeller action are introduced into the fluid domain to achieve the VLM - RANSE solver coupling. The User Defined Function (UDF) helps to achieve this coupling. The UDF enables to calculate the cell specific body force and identify the cell closest to the body force specific co-ordinate on the blade region in the sub-domain. See Fig. 8. The algorithm conducts search restricted to the swept volume in the disk area indicated below.

The UDF thread stores the coordinates of all the cell centroids belonging to the sub-domain at a temporary location. Similarly, it stores the coordinates of the panels on the blade shape and corresponding propeller forces at a temporary location. The cell centroids in the domain are matched to the closest panel blade coordinates, by comparing their distances between the panel coordinates and the coordinates of the cell centroids around it. If more than one panel corresponds to the same cell centroids, then the forces are added and assigned to these cells. The forces are assigned as density so that the cells have forces corresponding to their cell volume. These force terms are used during the solution of the momentum equation. Once the cell centroid coordinates and the body forces are finalized the same is stored in User Defined Memory in FLUENT to avoid running a centroid search algorithm at each step of the iteration. Inputting the body forces is achieved by reading the UDF in the momentum source panel in FLUENT. Finally the body force loaded sub-domain is rotated about the

axis of the propeller at its rated rpm to simulate the realistic rotating propeller. Fig. 4 shows the subdomain on application of propeller body forces.

The moving reference frame (Rotation)

The objective of assigning the moving reference frame is to achieve the rotation of the propeller domain with body forces at its rated rpm. By default, the solver deals with the equations of fluid flow in a stationary (or inertial) reference frame. In the case of ship hull with a rotating propeller at the aft, either the radial average of body force should be applied at the propeller swept volume or a rotating reference frame which incorporates the real rotation effect should be used. It is advantageous to solve the equations in a moving (or non-inertial) reference frame. The input is given as rotational velocity in radians/s about the propeller rotational axis in appropriate direction. Refer Fig. 5

-0.15 -0.1 -0.05 0 0.05 0.1

Figure 4. Application of body forces at the cell centers and rotation of the domain to obtain the effect of unsteady rotation

Figure 5. Stationary and rotating reference frames in FLUENT

In this case, the moving propeller renders the problem unsteady when viewed from the stationary frame. With a moving reference frame however, the flow around the moving part can be modeled as a steady-state problem with respect to the moving frame.

The moving reference frame modeling capability allows in activating the moving reference frame in selected cell zones. With this activation, the equations of motion are modified to incorporate the additional acceleration terms which occur due to the transformation from the stationary to the moving reference frame. By solving these equations in a steady-state manner, the flow around the moving parts can be modeled.


The principal particulars of the ship hull are given in Table 1, and propeller details are given in Table 2. The hull form is given in Fig. 6, and the propeller geometry in Fig. 7. Blade geometry characteristics are given in Table 3.

Table 1. Particulars of ship Particulars of the ship_Dimension

Length between perpendiculars Lpp 48.14 m

Breadth B 11.00 m

Draught d 2.90 m

Wetted surface area S0/Lpp2 0.1793

Block Coefficient CB 0.6508

No. of propellers 1

Table 2. Propeller details Item Value

Diameter 0.250 m

Hub/Diameter ratio 0.18

Number of blades 5

RPM 573

J 0.925

Thrust 90 N

Table 3. Particulars of propeller geometry - KP 505

Chord Max. Camber Max thickness

to dia to dia to dia

r/R P/D Rake Skew ratio C/D ratio fo/C ratio to/D lr/r

0.2 0.8347 0 —4.72 0.2313 0.0284 0.0459 0.4630

0.25 0.8912 0 —6.98 0.2618 0.0296 0.0407 0.5240

0.3 0.9269 0 —7.82 0.2809 0.0295 0.0371 0.5620

0.4 0.9783 0 —7.74 0.3138 0.0268 0.0305 0.6280

0.5 1.0079 0 —5.56 0.3403 0.0220 0.0246 0.6810

0.6 1.013 0 —1.5 0.3573 0.0173 0.0195 0.7150

0.7 0.9967 0 4.11 0.3590 0.0140 0.0149 0.7180

0.8 0.9566 0 10.48 0.3376 0.0120 0.0107 0.6750

0.9 0.9006 0 17.17 0.2797 0.0104 0.0069 0.5590

0.95 0.8683 0 20.63 0.2225 0.0101 0.0053 0.4450

1 0.8331 0 24.18 0.0001 0.0000 0.0037 0.0000

The sequences in the running are as follows: Step 1

At the first step the bare hull is run and the velocity distribution obtained at the propeller inlet section is shown in Table 4. For turbulence modeling, the Shear Stress Transport (SST) k — œ model was used. This model combines effectively the k — œ model in the near-wall region with the k — s model in the far field free-stream domain. The definition of the turbulent viscosity is modified to account for the transport of the turbulent shear stress. The settings in FLUENT are given later in Table 9.

Table 4. Velocity distribution at propeller disk obtained from RANSE simulation

Averaged axial Averaged radial Averaged tangential

R/r_velocity ratio_velocity ratio_velocity ratio

0.2-0.25 0.508271 -0.07203 0.002928

0.25-0.3 0.670154 -0.06797 -0.00078

0.3-0.4 0.738887 -0.08624 0.000465

0.4-0.5 0.775077 -0.09047 0.001273

0.5-0.6 0.782136 -0.08168 0.001388

0.6-0.7 0.787718 -0.07579 0.001369

0.7-0.8 0.795662 -0.07126 0.0013

0.8-0.9 0.802577 -0.06582 0.001156

0.9-0.95 0.807169 -0.05922 0.000935

0.95-1 0.810337 -0.05411 0.000752

Step 2

The circulation distribution corresponding to the above axial velocity distribution, for the required thrust and advance coefficient, is obtained.

Step 3

The radial velocity distribution obtained in Table 4, and the circulation computed in Step 2 above, is applied in VLM to obtain the body forces. The VLM, basically a blade design code, is modified to obtain as outputs the X, Y and Z components of non-dimensionalised thrust offered by span wise and chord wise singularities. At this stage a thrust correction is also applied to account for viscous effects. The typical listing of the non-dimensionalised thrust values and their location co-ordinates, as applied on the candidate hull (KCS container ship) are shown in Table 5-7. The co-ordinates are with reference to the propeller shaft centre line. The points are then transferred to the co-ordinates with reference to the fluid domain, as shown in Table 8.

Step 4

The body force density functions are input into the propeller swept volume through the UDF link to the RANSE solver to obtain the updated wake distribution. Steps 2 to 4 are iteratively run till there is no change in the circulation distribution in the successive step, within tolerance.

Table 5. Typical thrust distribution for chord wise singularities Thrust (non dimensionalised) offered by

Chord wise singularities__Coordinates of point of application

Fx chord Fy chord Fz chord X Y Z

3.04E-08 -1.62E-08 -2.27E-08 -0.1842 0.143 -0.1399

2.16E-07 -2.54E-07 -6.86E-08 -0.1794 0.1466 -0.136

6.77E-07 -1.10E-06 -6.19E-08 -0.1695 0.1531 -0.1287

1.49E-06 -3.21E-06 1.26E-07 -0.1547 0.1616 -0.1179

2.64E-06 -7.40E-06 4.81E-07 -0.1352 0.1711 -0.1035

3.97E-06 -1.45E-05 7.40E-07 -0.1117 0.1807 -0.0858

5.19E-06 -2.50E-05 2.63E-07 -0.0848 0.1891 -0.0651

5.94E-06 -3.86E-05 -1.80E-06 -0.0552 0.1955 -0.0423

5.84E-06 -5.39E-05 -6.10E-06 -0.0239 0.1992 -0.0182

Table 6. Typical thrust distribution for span wise singularities

Thrust (non dimensionalised) offered by

_Span wise singularities__Coordinates of point of application

Fx span Fy span Fz span X Y Z

-5.41E-06 2.94E-06 3.49E-06 -0.1842 0.143 -0.1399

-1.56E-05 9.10E-06 1.09E-05 -0.1794 0.1466 -0.136

-2.48E-05 1.47E-05 1.87E-05 -0.1695 0.1531 -0.1287

-3.30E-05 1.90E-05 2.65E-05 -0.1547 0.1616 -0.1179

-4.00E-05 2.16E-05 3.42E-05 -0.1352 0.1711 -0.1035

-4.54E-05 2.23E-05 4.13E-05 -0.1117 0.1807 -0.0858

-4.93E-05 2.09E-05 4.73E-05 -0.0848 0.1891 -0.0651

-5.15E-05 1.80E-05 5.18E-05 -0.0552 0.1955 -0.0423

-5.21E-05 1.38E-05 5.45E-05 -0.0239 0.1992 -0.0182

Table 7. Typical thrust compensation (non dimensionalised) for viscosity

Thrust compensation (non dimensionalised)

_for viscous correction_ _Coordinates of point of application

Fvisc X Y Z

2.53E-04 -0.1842 0.143 -0.1399

7.90E-04 -0.1794 0.1466 -0.136

1.32E-03 -0.1695 0.1531 -0.1287

1.80E-03 -0.1547 0.1616 -0.1179

2.21E-03 -0.1352 0.1711 -0.1035

2.53E-03 -0.1117 0.1807 -0.0858

2.75E-03 -0.0848 0.1891 -0.0651

2.86E-03 -0.0552 0.1955 -0.0423

2.88E-03 -0.0239 0.1992 -0.0182

Table 8. Combined resultant thrust distribution

Coordinates of point of application Thrust distribution in the domain (N) in the domain

Fx Fy Fz X Y Z

-0.00252125 0.00141746 0.00168494 0.1045 0.0178 0.1122

-0.00717463 0.00429184 0.00526566 0.1025 0.0261 0.1034

-0.01126174 0.00660840 0.00903369 0.1033 0.0360 0.0962

-0.01468324 0.00768601 0.01294061 0.1050 0.0477 0.0912

-0.01734707 0.00691375 0.01684287 0.1070 0.0619 0.0902

-0.01924604 0.00376411 0.02040634 0.1097 0.0781 0.0947

-0.02046080 -0.00197040 0.02309086 0.1128 0.0948 0.1058

-0.02113396 -0.00999957 0.02427156 0.1165 0.1097 0.1248

-0.02143012 -0.01947713 0.02348317 0.1061 0.0186 0.1131

-0.02146252 -0.02915713 0.02064533 0.1041 0.0274 0.1047

Table 9. Solver parameters used for simulations


Solver 3D Segregated, Unsteady, Implicit

Velocity formulation Absolute

Viscous model SST k - (0 (barehull), Realizable k - s (with propeller)

pressure-velocity coupling PISO (Pressure Implicit with Splitting of Operators)

pressure discretization Body force weighted

Momentum discretization Quick

Volume fraction Modified HRIC

Turbulent kinetic energy and energy

dissipation rate discretization Second order upwind scheme

Hull and, top and bottom

boundary conditions Wall (no slip), Wall (allows slip)

Free surface model Volume of Fluid

Air and water Inlet boundary conditions Velocity Inlet: Free stream velocity

Air and water outlet boundary conditions Out flow

Settings for FLUENT

Computational Domain and Grid System

Based on ITTC 1999 recommendation, the computational domain was chosen with length of the domain upstream of the hull being 1.9 Lpp, downstream being 2.5 Lpp, width of Lpp on both sides and depth being 0.7 Lpp, Lpp refers to the ship length between perpendiculars. Block structured hexahedral grid was used for the domain descretization.

For initialization in general, all the flow variables are set to zero values and the simulation converges towards the steady state. The gridded domain was marked and separated in order to demarcate water and air regions as separate entities, and the regions patched and allocated appropriate volume fraction values. In order to initialize, the X-component (along the length) velocity at air and water inlet were set to free stream velocity corresponding to the model speed of 2.196 m/s, at the start of computations and all other variables set to zero. The UDF was interpreted and the source terms added.

The boundary conditions were set with the same velocity inlet at the domain inlet, out flow at the domain outlet, wall with slip and zero shear (at free surface and at the bottom and side wall) and wall with no slip (over the hull surface) conditions (Fig. 8).

Block structured multi-block grids in ANSYS ICEM CFD was used to generate numeric grids in the domain. The region near hull was meshed with O-grid to capture the fictional resistance. The difficulty of gridding the sub domain with in presence of complicated blade geometry is avoided in this method. Fine mesh was used to represent the cylinder representing the propeller swept volume by O grids, see Fig. 3.


The numerical results based on simulation of the self propulsion condition in the KCS container ship are given in Fig. 10 to 22. The comparisons from literature are included in Fig. 9, 10, 19 and 20. The cross flow vectors have been well captured in the present simulation as seen in Fig. 10. The axial, radial and tangential velocity components at both the inlet and outlet of the propeller have been realistically captured and are depicted in Fig. 11 to 16. The wave elevation contours are compared in Fig. 19. The kinematics are presented for the ship speed corresponding to Fn = 0.26. By coupling the propeller into the ship flow simulation using the UDF, the augmented resistance and self propulsion point has been successfully obtained. The thrust deduction fraction has been obtained as 0.14. This is quite realistic for the hull form considered.

In conclusion, a computationally efficient method is presented for obtaining the dynamics and associated kinematics of the propeller-ship interaction.

Domain extends -1.9<x/Lpp<2.5 -1 <y/Lpp<1 -0.7<z/Lpp<0

Gridded propeller domain (magnified)

Figure 8. Computational domain with boundary conditions for RANSE solver

Cross flow vectors at D/4 downstream (CFD)

-0.01 -0.02 -0.03 -0.04 -0.05

/ / Jf / S S s Jf * .'K-K't.W W /////A

///// ////J ffffl fftjl fftjl f'fti



-0.04 -0.02

Cross flow vectors at D/4 downstream (Experimental - CFD workshop Tokyo 200

Figure 9. Cross flow vectors down stream of the propeller plane

Ratio of axial velocity contour (CFD) at D/4 downstream

Ratio of axial velocity contour (Experimental - CFD workshop Tokyo 2005 at D/4 downstream

Figure 10. Comparison of ratio of axial velocity contours down stream of the propeller plane

-0.1 -0.05

0.05 0.1

Figure 12. Ratio of axial velocity at propeller outlet

Figure 13. Ratio of radial velocity contours at Propeller inlet

Figure 14. Ratio of radial velocity at propeller outlet

Figure 15. Ratio of tangential velocity at propeller inlet

0.15 -

0.05 -

-0.1 -0.05 0

0.05 0.1

Figure 16. Ratio of Tangential velocity at propeller outlet

-0.1 -0.05 0 0.05 0.1

Figure 17. Ratio of tangential velocity contours at D/4 down stream

Figure 18. Ratio of radial velocity contours at D/4 downstream

Figure 19. Wave elevation contours compared with the experimental results (CFD workshop Tokyo 2005)

Figure 21. Dynamic pressure contours on the Bare hull surface


Simonsen, C. D. and Stern, F. (2005), RANS "Maneuvering Simulation of Esso Osaka with Rudder and a Body-Force Propeller". Journal Ship Research, Vol. 49, No. 2, pp. 98-120.

Tahara, Y., Wilson, R., and Carrica, P. 2005. "Comparison of free-surface capturing and tracking approaches to modern container ship and prognosis for extension to self-propulsion simulator", Proc CFD workshop Tokyo 2005, 548-555.

Karl, Y., Chao. and Carrica, P. (2005). "Numeric propulsion for the KCS container ship, Proc CFD workshop Tokyo (2005), 483-489.

FLUENT 6.2 User's Guide (2006), Copyright Fluent Incorporate.

Kerwin, J. E. (1984). "A vortex lattice method for propeller blade design", MIT PBD-10 users manual, Massachusetts institute of technology.

Olsen, A. (2001). "Optimization of propellers using Vortex lattice method", PhD thesis, Denmark technical university.

Kerwin, J. E., Lee, C.S. (1978). "Prediction of steady and unsteady marine propeller performance by numerical lifting surface theory" SNAME Transactions, Vol.86, 1978, pp. 218-253.

Dhinesh, G., K. Murali, V.A. Suramanian, (2009) "Estimation of hull-propeller performance by numerical lifting surface model hull using RANSE solver" Ships and Offshore Structures, Vol. 2(2), 1-15.

Hino, T. (2005) Preprints of CFD Workshop Tokyo 2005, National Maritime Research Institute, Tokyo, Japan.