Computational Fluid Dynamics Modelling
of the Yamaha Personal Watercraft
Motivation for CFD Modelling
The purpose of the CFD analysis is to provide a general overview of the complex flow
created by the planing surfaces of the hull. The motivation for the modelling with a CFD
program was, that given the alternatives such as tow tank testing or full scale testing of
the actual craft provided to us, this was deemed to be the easiest method to obtain
potentially useful information for our client. This is taking into consideration that the
winter conditions make it nearly impossible to test the craft on a lake (ice) or on a river
(dangerous). Scaled model testing in a tow tank also requires considerable time and is
relatively expensive when compared to a CFD model. In a CFD model numerous
simulations can be performed by changing a few parameters of the geometry of the
problem provided the validity of the model can be verified.
Some challenges in CFD modelling applied to modeling of boats are presented in the
following excerpt from Beck:
Some important information which could potentially be obtained by CFD included; the
pressure distribution on the planing surfaces of the hull, the streamlines and the
recirculation zone as the fluid separates at the transom edge. The pressure distribution on
these planing surfaces at various angles of attack would be beneficial in determining the
lateral components of the resulting pressure force acting normal to these surfaces. Thus
far the roll is not yet being considered.
Preliminaries to the Problem
Modelling of the flow around the hull alone would be required before any appendages
either in the form of flaps or rudders could be included with the hull shape. Inspection of
the Yamaha Waverunner hull reveals that it has primarily two flat surfaces that make up a
‘V’ shape. These surfaces are at approximately 20 degrees from the horizontal as
illustrated in Figure D1.
Figure D1 - 'V' Angle of Yamaha Hull
Since we are interested in turning behaviour when the hull is planing, we’ve begun with
the assumption that the hull is nearly planing and pitched backward as shown in Figure
Figure D2 - Wetted Surface of the Hull
To make modeling easier, the hull geometry was simplified. The apparent wetted surface
was approximated by the triangular shape shown in Figure D3. The blue surface is at the
surface of the water, the red surface is at the stern, and the dark surface is the starboard
part of the hull that’s in contact with the water.
Figure D3 - Simplified Geometry of Wetted Surface
After a search of available software was performed, it was initially determined that
ANSYS would be suitable for the problem, however the specification of proper boundary
conditions was later found to be problematic and thus CFX 5.6 was rechosen as an
alternative. Initially ANSYS was used to model the flow of the apparent wetted portion
of the planing hull at a planing speed of 13.4 m/s. The automatic meshing of the fluid
element was achieved with grid refinement on the two planing surfaces. CFX 5.6 and
Gambit/Fluent were also used to model the fluid element initially, but the meshing
methods were a problem at the tip of the fluid model where the surface of the water is
pierced in CFX 5.6 and on the hard edges (location of spray) for Gambit/Fluent. For a
planing hull, the pitch angle is approximately 3-4 degrees according to Cohen . This
also agrees with the video footage from summer runs of the Yamaha craft. With this
assumption, the apparent wetted portion of the hull is much like a triangular prism of
dimensions 1.85m, 0.1258m and 0.6916m for the length, depth and width, respectively.
Using the ANSYS 7.1 program the fluid portion modelled is shown below (Figure D4).
Figure D4 - Fluid Volume in ANSYS Model
At an angle of attack of 5 degrees with a freestream component of 1.168 m/s in the y-dir
and an x-component of 13.35 m/s the following pressure distribution was obtained for the
modelled fluid (figure D5):
Figure D5 - Pressure Distribution on Surfaces of ANSYS Model (5 deg of Yaw)
The method used included a refined mesh on the 2 planing surfaces of the fluid model
and an ordinary mesh for the rest of the fluid. The element type used was of the
tetrahedral type (fluid 142). The boundary conditions on the faces of the fluid volume
were set by specifying the condition of no slip on the planing surfaces and no velocity in
the z direction for the free surface. The pressure along the back wall was set as the
reference pressure P=0 (outlet condition). The Inlet velocity was also specified in terms
of its components (u,v,w) in vector form. This solution showed a perculiar result for the
pressure field and irregular patterns on the surfaces as shown in figure D5. Changing the
boundary conditions and relaxing parameters yielded no better data. After further
discussion with Professor Szyszkouski, the ANSYS/Flotran program was abandoned and
the CFX 5.6 program was reconsidered.
CFX 5.6 Program Structure
The CFX program is comprised of four sections
3) CFX-Solver Manager
Adjustment of Previous Build Model
In CFX Build, the geometry of the prism, previously determined in the ANSYS model,
was used to create an Autocad model with 3D solids editing features. The Autocad
model was used in order to obtain the coordinates of the truncated point, which was now
a sufficiently small, 3-point triangular face at the tip of the prism. This was required
mathematically to enable the solid to be meshed properly. The CFX GUI was used and
from the keypoints, edges were created, after which surfaces were defined using the
edges. The surfaces were then used to define a solid shown in figure D6 (next page)
along with the bounding box surfaces. For the model at an angle of yaw, the prism
surfaces were selected and rotated about the Z-axis by 5 degrees, after which the solid
was recreated and later re-meshed.
Figure D6 - Geometry of the Fluid Model with zero Yaw Angle
The bounding box was also created for both models, extending 2 times the width, 2 times
the length and 5 times the height of the prism dimensions. The Solid region for both
cases, were then each given a name and later the 2-dimensional regions (faces) of each
solid were assigned domain names. Meshing was easily performed for this attempt and
mesh refinement was specified at the transom surface. Mesh refinement wasn’t required
for the small face at the front of the prism due to its small area. Meshing of the fluid
volume produced 76000 volume elements. The meshed volume is shown in figure D7.
Figure D7 – The Meshed Fluid Volume with zero Yaw Angle
The CFX Build geometry and mesh were then written to *.db files which were opened in
the CFX-Pre program. The db file consists of the *.CFX (geometry) and the *.gtm
In CFX-Pre, the physics of the model fluid domain are specified. The faces of the model
are defined and domains named. In this section, the inlet was specified in terms of the
fluid velocity components. The freestream at the inlet was set to 13.4 m/s (30mph). The
outlet condition was set at the rear face of the bounding box, where the pressure was set
to zero. The other four walls of the bounding box were called freewall 1-4. The boundary
condition placed on them was the slip condition with no shear stress along the surface.
The remaining walls were those of the hull which were assigned a no-slip condition. The
CFX–pre model is shown in Figure D8.
Figure D8 – Model Domain Specification in CFX-pre
The fluid properties were set to water from the library provided and the simulation type
was set to steady-state. The initialisation was automatically set by the program. For
solver control, the advection scheme was specified as high resolution, convergence
control was set to the physical timescale with the max number of iterations set to 200 and
with a time scale of 5 seconds. The convergence criterion was set as the root mean
square residual convergence target of 1e-6. The definition file (*.def) was then written.
The CFX Solver Manager plots the residuals for the velocity, residuals and the pressure
and for the k-and epsilon equations , using a convergence criterion of 10^-6 for residuals
Figure D10 - CFX Solver Manager Output (zero yaw)
Figure D11 - CFX Solver Manager Output with Yaw
CFX-post was used to analyze the results output from the CFX solver manager (*.res
file). Visual graphing of the streamlines and the pressure distributions were displayed.
These results can give an insight to the flow on the underside of the hull using
streamlines and pressure distributions. The results are shown in figures D12-17 for the
streamlines and the pressure distribution obtained in both models. The pressure variation
between surfaces for the yaw model is readily shown in figure D15. The results of the
model indicate a general high pressure towards the front of the model prism. This shows
agreement with the empirical models mentioned ealier.
Figure D12 - Pressure Contours on the Hull Surfaces (no Yaw)
Figure D13 - Pressure Contours on the Model Wall Surfaces (no yaw)
Figure D14 - Streamlines in the Entire Flow Domain (no yaw)
Figure D15 - Contour Plot of for Full Range of Values of Pressure on Yaw Model
Figure D14a - Streamlines in the Entire Flow Domain on Yaw model
Figure D14b - Streamlines and vortex in the Entire Flow Domain on Yaw model.
The CFX files to construct these streamline plots are CFX results files which are
appended with the cd.
Significance of Modelling in CFX
The pressure distributions along the planing surfaces obtained when integrated would
then give the total hydrodynamic force and the directions this force acts in. As for the
roll, the fluid element needs to be changed for every degree as it goes through the roll
since the wetted shape also changes. The validity of the data obtained thus far should be
investigated further and verified before modelling the roll of the watercraft in a turn.
After further investigation of the tests performed by Savistky it was concluded that
the wetted area assumption we had made previously was invalid for a planing hull with
chines, such as for our particular Yamaha PWC. The flow could actually drop below the
plane of the undisturbed surface as it follows along the chine. This is believed to be the
case by observing the following photos in figures D16-17 for a Sea-Doo craft.
Figure D16 – Sea-Doo Watercraft 
Figure D17 - Sea-Doo watercraft at high speed (planing) 
Special attention should be placed at the tip of the surface piercing point where the spray
root is shown to rise up the sides of the craft as it deflects off of the first chine. The
underside of the Yamaha hull is shown in figure D18.
Figure D18 - Actual Yamaha Hull underside
To make things visually easier, an illustration made in Autocad 2004 of the Yamaha hull
is shown in figure D19 (next page). The red line shows a more probable path for the
wetted surface for a planing trim angle of 4 degrees.
Figure D19 Wetted hull predictions (Yamaha)
Considering the above figure D19, the model represents only a rough approximation for
the flow, in general characteristics that should still hold true include the location of the
spray tip with respect to the planning surfaces and the free surface. This is corroborated
in High-Speed Small Crafts  which shows that there is no significant pressure wave
created at the front of the advancing tip unlike a flat plate which shows considerable
change in wetted length with increase in speed. Thus the actual area of wetted surface
would be in error due to the chines. It is also probable that the chines affect the flow
along the hull constraining the streamlines near the hull surface. Possible future
modelling should include the actual complete geometry of the hull with chines and
software specifically designed for planing hulls.