Guy A

Document Sample
Guy A Powered By Docstoc
					            Appendix D
Computational Fluid Dynamics Modelling
  of the Yamaha Personal Watercraft
                                        Appendix D

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[21]:

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

                                            Appendix D

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


                                         Appendix D

                             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

                                       Appendix D

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 [22]. 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):

                                       Appendix D

         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.

                                        Appendix D

CFX 5.6 Program Structure

The CFX program is comprised of four sections

       1) CFX-Build

       2) CFX-Pre

       3) CFX-Solver Manager

       4) CFX-Post

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.

                                        Appendix D

                 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.

                                        Appendix D

                   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

(meshing) files.

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.

                                       Appendix D

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.

                                       Appendix D

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 D10-11).

                     Figure D10 - CFX Solver Manager Output (zero yaw)

                     Figure D11 - CFX Solver Manager Output with Yaw

                                       Appendix D

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.

                       Appendix D

Figure D12 - Pressure Contours on the Hull Surfaces (no Yaw)

                          Appendix D

Figure D13 - Pressure Contours on the Model Wall Surfaces (no yaw)

   Figure D14 - Streamlines in the Entire Flow Domain (no yaw)

                                Appendix D

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

                                        Appendix D

         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.

                                        Appendix D

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[18] 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 [3]

                                         Appendix D

                   Figure D17 - Sea-Doo watercraft at high speed (planing) [3]

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.

                                         Appendix D

                       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 [11] 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.


Shared By: