P.Bull (Defence Research Agency, United Kingdom)

Good propulsor design requires knowledge of the flow entering the region just upstream of a propulsor. For both submarine and surface ships, it is desirable that the hull provides as uniform a nominal wake as possible in this region. In this context, the wake can be defined to be the fluid velocity distribution. Detailed knowledge of the velocity distribution will result in the propulsor designer being able to produce an efficient and effective propulsion system.

Whilst the fluid velocity distribution can be measured by using a scale model in a towing tank or wind tunnel, there are difficulties in applying results obtained at model scale to the full scale hull. Furthermore, experiments of this type require many detailed measurements to be taken in the region of interest. These can be both costly and time consuming.

An alternative approach is to use Computational Fluid Dynamics (CFD) to predict the fluid velocity distribution by solving the fundamental equations of motion using numerical methods. An advantage of this approach is that it has the potential to remove the difficulties associated with the traditional methods, since predictions can be made at both model and full scale. The fundamental equations for fluid flow, which describe the conservation of fluid mass and momentum, are the equation of continuity and the Navier-Stokes equations. In practice, it is impossible to solve these equations directly since the fastest supercomputer with the largest memory available falls short of the required performance by many orders of magnitude. However, if the fundamental equations are averaged over a period of time, the computer requirements for the resolution of the flow features are eased enormously. These time-averaged equations are known as the Reynolds-Averaged Navier Stokes Equations (RANS) equations. The time-averaging process introduces new variables into the equations that are known as the Reynolds stresses. Turbulence models are introduced which require assumptions to be made on the relationships between the Reynolds stresses and the mean flow parameters. The numerical methods used to solve these equations and the turbulence models introduce errors into the prediction of the flow parameters.

Therefore, both experiments and CFD computations have degrees of uncertainty with the accuracy of the predictions of the flow parameters for full scale flows. This gives rise to the need for validation of both the measurements and computations for the prediction of such flows, in order to quantify the uncertainty levels. This can be achieved by comparison between high quality experiments, where the uncertainty is carefully evaluated and quoted, and computations, where a systematic approach is used to quantify the uncertainty in the various stages of the numerical methods [1].

One such high quality experiment data set is the DARPA SUBOFF [2,3,4] set of measurements which provide a comprehensive set of data for a number of different geometry configurations. This paper describes a comprehensive validation exercise which has been carried out at the Defence Research Agency (DRA) at Haslar for one of the SUBOFF configurations. This configuration was chosen as

© British Crown copyright 1996. Reproduced with the permission of the Controller of Her Majesty's Stationery Office. The views expressed are those of the author and do not necessarily reflect the views or policy of The Ministry of Defence, Her Majesty's Stationery Office or any other British government department. |

Below are the first 10 and last 10 pages of uncorrected machine-read text (when available) of this chapter, followed by the top 30 algorithmically extracted key phrases from the chapter as a whole.

Intended to provide our own search engines and external engines with highly rich, chapter-representative searchable text on the opening pages of each chapter.
Because it is UNCORRECTED material, please consider the following text as a useful but insufficient proxy for the authoritative book pages.

Do not use for reproduction, copying, pasting, or reading; exclusively for search engines.

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
The Validation of CFD Predictions of Nominal Wake for the SUBOFF Fully Appended Geometry
P.Bull (Defence Research Agency, United Kingdom)
Introduction
Good propulsor design requires knowledge of the flow entering the region just upstream of a propulsor. For both submarine and surface ships, it is desirable that the hull provides as uniform a nominal wake as possible in this region. In this context, the wake can be defined to be the fluid velocity distribution. Detailed knowledge of the velocity distribution will result in the propulsor designer being able to produce an efficient and effective propulsion system.
Whilst the fluid velocity distribution can be measured by using a scale model in a towing tank or wind tunnel, there are difficulties in applying results obtained at model scale to the full scale hull. Furthermore, experiments of this type require many detailed measurements to be taken in the region of interest. These can be both costly and time consuming.
An alternative approach is to use Computational Fluid Dynamics (CFD) to predict the fluid velocity distribution by solving the fundamental equations of motion using numerical methods. An advantage of this approach is that it has the potential to remove the difficulties associated with the traditional methods, since predictions can be made at both model and full scale. The fundamental equations for fluid flow, which describe the conservation of fluid mass and momentum, are the equation of continuity and the Navier-Stokes equations. In practice, it is impossible to solve these equations directly since the fastest supercomputer with the largest memory available falls short of the required performance by many orders of magnitude. However, if the fundamental equations are averaged over a period of time, the computer requirements for the resolution of the flow features are eased enormously. These time-averaged equations are known as the Reynolds-Averaged Navier Stokes Equations (RANS) equations. The time-averaging process introduces new variables into the equations that are known as the Reynolds stresses. Turbulence models are introduced which require assumptions to be made on the relationships between the Reynolds stresses and the mean flow parameters. The numerical methods used to solve these equations and the turbulence models introduce errors into the prediction of the flow parameters.
Therefore, both experiments and CFD computations have degrees of uncertainty with the accuracy of the predictions of the flow parameters for full scale flows. This gives rise to the need for validation of both the measurements and computations for the prediction of such flows, in order to quantify the uncertainty levels. This can be achieved by comparison between high quality experiments, where the uncertainty is carefully evaluated and quoted, and computations, where a systematic approach is used to quantify the uncertainty in the various stages of the numerical methods [1].
One such high quality experiment data set is the DARPA SUBOFF [2,3,4] set of measurements which provide a comprehensive set of data for a number of different geometry configurations. This paper describes a comprehensive validation exercise which has been carried out at the Defence Research Agency (DRA) at Haslar for one of the SUBOFF configurations. This configuration was chosen as
© British Crown copyright 1996. Reproduced with the permission of the Controller of Her Majesty's Stationery Office. The views expressed are those of the author and do not necessarily reflect the views or policy of The Ministry of Defence, Her Majesty's Stationery Office or any other British government department.

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
representative of the other configurations at zero angle of attack.
The SUBOFF experiments
The SUBOFF experiments were funded by DARPA and conducted at the David Taylor Model Basin during 1988 and 1989. A number of submarine configurations, ranging from an axisymmetric body to a fully appended submarine were constructed in order to provide flow measurements for CFD validation. Each of the models was placed in the Anechoic Flow Facility (AFF) wind tunnel. The dimensions of the wind tunnel and layout of the model are shown in figure 1. The flow was measured at a Reynolds number of 1.2×107. This paper considers the flow past configuration AFF-1-, the axisymmetric body of revolution and configuration AFF-8-, the fully appended geometry at zero angle of attack.
Figure 1 The wind tunnel
For each configuration, pressure taps on the hull surface connected to rotary pressure scanners provided measurements for surface pressure. The wall shear stress was also measured at the location of selected pressure taps. A traversing mechanism was used to position hot film probes in order to measure mean and fluctuating components of the velocity. The uncertainty of the measurements, with 95% confidence, was 2.5% of U∞ for the mean flow components and 0.2% for the Reynolds stresses, where U∞ is the free stream inlet velocity. The uncertainty of the absolute values of the pressure and wall shear stress was within ±0.015 and ±0.0002 of their measured values respectively. A complete description of the measurement system and their uncertainty is given in reference 1.
For the axisymmetric naked hull case, AFF-1-, measurements were taken at non-dimensionalised positions of x/L=0.875, 0.904, 0.927, 0.956 and at the propulsor plane x/L=0.978 where x is the position along the hull and L is the total length of the hull. For the fully appended case, AFF-8-, measurements were taken at positions x/L=0.978, 1.040, 1.096 and 1.200. For the AFF-8- case, the flow was measured at two degree intervals for radii between r/Rmax=0.25 and 2.00 where r is the distance of the probe from the axis of the hull and Rmax is the maximum radius of the hull. The quantities obtained at each location of these wake surveys were
and the static pressure. The non-dimensional quantities Cp and Cτ are then defined by
where u=mean axial velocity component
vr=mean radial velocity component
vθ=mean tangential velocity component
u′,v′,w′=fluctuating components
p=static pressure
p∞=free stream static pressure
ρ=fluid density
and τw=wall shear stress
Grid generation
In order to perform a validation exercise of this type, it is necessary to have a fast, efficient grid generation system which is capable of producing high quality grids with sufficient grid density to resolve the flow features. The system chosen was the SAUNA [5,6] system produced for the DRA by the Aircraft Research Association Ltd. The system uses the elliptic multiblock method to generate grids around fully appended geometries. This system is currently being developed to generate hybrid structured and unstructured grids with hexahedral, pyramidal, prismatic and tetrahedral cells. The SAUNA system takes separate geometry component definitions and combines them together into the required configuration, calculating intersections, as required.

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
For the SUBOFF configurations, the geometry of the hull, sail and aft appendages were analytically defined, although the aft appendage fin tips were modified to have elliptical caps.
A background grid topology is used to form the basis of a grid and individual topologies, associated with each geometry component, are automatically embedded with this. A local topology is applied in each of the two parametric directions of a geometry component. For aerofoil-like components, such as a sail or an aft appendage, these directions are equivalent to the chord and the span. Three different topologies, H,C and O can be combined to give a choice of 6 topologies for appendage and 3 for hulls. Illustrations of the topologies chosen around a sail are shown in the figure 2. The full volume topology is created automatically.
Figure 2 Types of topology around the sail
Surface grids are generated for each geometry component and for the bounding surfaces of the domain, using the appropriate block faces from the full volume topology. These grids are generated as solutions of a two dimensional set of partial differential equations. For geometry components, the surface grids are generated in parametric co-ordinates. Internal grid control surfaces are also generated which extend from certain components. These are used to control grid quality. Initial surface grid distributions are automatically defined by the SAUNA system around key contours of the components. The volume grid is formed in two stages. Initially a coarse grid is generated as a solution of a three-dimensional set of elliptic partial differential equations. This grid is refined algebraically with the blocks abutting the geometry in order to provide cells of aspect ratio suitable for capturing the viscous boundary layer around the geometry. The algebraic refinement is propagated into additional adjoining blocks to satisfy continuity of cell distribution. This provides extra refinement to help capture viscous wakes when C and H topologies are used. An example of the type of grid produced by SAUNA for the SUBOFF AFF-8-configuration using an O-O topology around the hull and C-C topology around the appendages is shown in figure 3.
Figure 3 Typical SUBOFF grid
A number of grids were generated with cell numbers ranging from 250,000 cells to 1,000,000 cells and for four topologies, H-H, C-H, C-C and O-O around the appendages. Additional grids were also generated using a preliminary version of the hybrid system with prismatic cells surrounding the geometry and tetrahedral cells elsewhere. The same domain size was used for all grids. In addition, care was taken to

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
ensure that the first cell spacing, which controls the accuracy and applicability of a wall function approach, was consistent for all the grids. This cell spacing was chosen to give an approximate value of 50 for the non-dimension parameter y+, along the length of the hull and appendages.
Table 1 defines a grid identifier for each of these grids and outlines the number of cells and topology for each.
Table 1 Grid Properties
Grid Identifier
Hull Topology
Appendage Topology
Number of Geometry Cells
Number of Fluid Cells
Grid A
O-O
N/A
72
2,496
Grid B
O-O
N/A
120
4,096
Grid C
O-O
N/A
176
5,472
Grid D
Unstr
N/A
7,458
309,162
Grid E
O-O
H-H
5,568
271,104
Grid F
O-O
H-H
7,745
526,720
Grid G
O-O
H-H
18,496
1,042,048
Grid H
O-O
C-H
6,032
271,448
Grid I
O-O
C-H
7,168
476,928
Grid J
O-O
C-H
17,616
1,023,232
Grid K
O-O
C-C
10,048
511,744
Grid L
O-O
C-C
19,792
1,032,192
Grid M
O-O
O-O
11,792
476,096
Grid N
O-O
O-O
22,224
997,376
Grid O
Unstr
Unstr
14,434
432,180
Grid P
Unstr
Unstr
32,208
1,243,689
Brief description of flow solution algorithms
Several distinct types of flow solution algorithms are potentially applicable to the prediction of the nominal wake. These algorithms use different methods for discretising the RANS equations which fall into three broad categories: finite difference, finite volume and finite element. Each method has different advantages, depending on the complexity and nature of the application. In addition, a number of different turbulence models can be used to estimate the Reynolds stresses with varying degree of sophistication and accuracy. Some of the important turbulence models are given below:
a.
Zero equation Baldwin-Lomax
b.
Two equation k–ε
c.
Renormalisation Group two equation k-ε
d.
Differential Reynolds Stress transport model
The differences in discretisation approaches, in numerical techniques used to segregate and linearise the equations; in turbulence models and in boundary condition and wall functions lead to many distinct CFD algorithms. These algorithms govern the behaviour of individual RANS flow codes when applied to the prediction of nominal wakes.
The RANS flow codes used in this validation exercise are outlined briefly below:
CFDS-FLOW3D [7] is a multi-block structured, control volume based finite difference flow code. The governing equations are discretised, based on a curvilinear grid to enable computations on complex and irregular geometries. Interpolation is accomplished via a wide range of different advection schemes. CFDS-FLOW3D offers a choice of k-ε, RNG k-ε and the Reynolds Stress turbulence models which can be used in conjunction with standard near-wall modelling methods.
FLUENT/UNS [8] is an unstructured control volume flow code which is based on solution adaptive, fully unstructured grids with cell centred discretisation schemes. A pressure based segregated solution scheme is used for the velocity-pressure coupling and algebraic multigrid methods are used to accelerate convergence. A first or second order upwind scheme is used for convection terms and a second order reconstruction scheme is used for diffusion terms. FLUENT/UNS offers a choice of k-ε or the RNG k-ε turbulence models which can be used in conjunction with two different near wall modelling methods.
FIDAP [9] is an unstructured finite element flow code based on the iterative solution of the discretised equations using the Petrov-Galerkin method. The equations are solved in a segregated form, using pressure correction to ensure mass conservation. FIDAP offers a choice of k-ε or extended k-ε with different models for the eddy viscosity and near- wall modelling based on a Reichart wall element.
Although this list of flow codes is not exhaustive, the flow solution methods were chosen to be representative of the types commercially available. Each of these flow codes is a general purpose fluid dynamics package which can be used for a wide range of problems. This paper is only concerned with their application to high Reynolds' number flows around the SUBOFF geometry.

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
Measures for validation
For any validation exercise of this type, it is important to decide on suitable measures for comparing the computed flow results with the measured data.
Comparison between the axial variation of the non-dimensional static pressure coefficient Cp and the skin friction coefficient Cf is appropriate for the naked hull configuration AFF-1-. Boundary layer profiles of the axial velocity component and turbulent kinetic energy at stations along the hull are also compared.
It is more difficult to define suitable measures of the accuracy of the flow computations for the fully appended configuration AFF-8-due to the three-dimensional nature of the flow features. For this paper the following measures were used:
Contours of the Taylor wake fraction in the propulsor plane.
Wake survey of flow parameters at various radii in the propulsor plane
The averaged circumferential Taylor wake fraction at various radii in the propulsor plane.
Harmonics of the Taylor wake fraction.
The Taylor wake fraction and the averaged Taylor wake fraction are defined as
W(r,θ)=u(r,θ)/U∞
and
respectively, where
u(r,θ)=axial velocity component in the propulsor plane
r=radial distance from the axis
and θ=circumferential angle
The angle θ is measured from θ=0 at the upper symmetry plane and θ=π at the lower symmetry plane.
The wake harmonics are defined to be the amplitude coefficients, An(r) of the Fourier series representation of the Taylor wake fraction as given by:
where
This definition gives W1(r) as the zeroth order harmonic of the Taylor wake fraction.
Results for the AFF-1- Configuration
Preliminary computations for the AFF-1-configuration were made using the flow code FIDAP. These computations were used to investigate the sensitivity of such flows to changes in the initial and input parameters. The chosen parameters were checked using FLUENT/UNS to ensure that consistent results could be obtained using a different flow solution algorithm.
Computations using the FLUENT/UNS flow code were performed for grids A, B and C using k-ε and RNG k-ε turbulence models. Figure 4 shows comparison between the measured data and the computations, for the pressure and skin friction coefficients respectively, for each of these models. The measured data are given as symbols and the

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
predictions for each grid are given by solid, dashed and dotted lines for grids A, B and C respectively.
Figure 4 Pressure and skin coefficients for the AFF-1-configuration
Comparisons of the boundary layer profiles at the axial stations x/L=0.875, 0.904, 0.956 and 0.978 are shown in figure 5. The measured data are given as symbols and the predicted data for grid A, B and C using solid, dashed and dotted lines repsectively.
Figure 5 Axial velocity profiles for the AFF-1- configuration

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
A later computation, using the hybrid unstructured grid E, was also carried out for the AFF-1-configuration. The pressure coefficient for this prediction and the equivalent prediction for grid B are shown in figure 6 with boundary layer profiles in figure 7.
Figure 6 Pressure coefficient for structured and unstructured grids
Figure 7 Boundary layer profiles for structured and unstructured grids
Results for the AFF-8- Configuration
Computations were made for the AFF-8-configuration for the grids described above using the flow codes FLUENT/UNS, FIDAP and CFDS-FLOW3D. Care was taken to ensure that the same inlet and initial conditions were used for each computation by using non-dimensional parameters. The initial and inlet conditions were defined as:
U∞=1.0
L=12.926
ρ=1.0
µ=1.191×10–6
k=1.332×10–4
ε=4.47×10–5
These parameters give a Reynolds number of
Re=1.2×107
where
The chosen parameters for the turbulence were based on the sensitivity study carried out using FIDAP for the AFF-1- configuration. The turbulent dissipation rate, ε, was chosen by prescribing the ratio of molecular to turbulent viscosity. The value chosen for this ratio was
where
Initial computations were made with grids E,F and H,I; the H-H and C-H topology grids with 250,000 and 500,000 cells respectively. Contour plots of the Taylor wake fraction, W, in the plane of the propulsor at x/L=0.978 are shown in figures 8 to 14, for the measured experiment values and for each of the flow codes. All the contours are plotted to the same scale and range from a minimum value of 0.4 to a maximum of 0.9 with an increment of 0.05. The predictions for the grids E and H are shown on the left with grids F and I on the right of each figure.

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
Figure 8 Taylor wake contours for measured experiment data
Figure 9 Taylor wake contours for FLUENT/UNS C-H topology grids
Figure 10 Taylor wake contours for FLUENT/UNS H-H topology grids
Figure 11 Taylor wake contours for FIDAP C-H topology grids

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
Figure 12 Taylor wake contours for FIDAP H-H topology grids
Figure 13 Taylor wake contours for FLOW3D C-H topology grids
Figure 14 Taylor wake contours for FLOW3D H-H topology grids
It is clear that the predictions obtained by FLOW3D failed to converge for the C-H topology grids. This was due to grid singularities in the C-H topology grids due to the embedding of C grids around the leading edges of the appendages in SAUNA. This causes degenerate cells to be generated above the fin tips. These degenerate cells were not present in the H-H topology grids.
It is also evident that the development of the hull boundary layer was unstable in the predictions obtained by FIDAP. This was because the hull surface grid density was insufficient for the Reichard wall function model implemented in FIDAP.
Comparison between the predicted and experiment velocity components and turbulent kinetic energy are given in figures 15 and 16 for the FLUENT/UNS computations. The figures show the variation of the flow parameters u,v,w and k at a radius of r/Rmax= 0.25. Data are plotted at 2° from the upper centreline of the hull, in the plane of the propulsor at x/L= 0.978. The computational predictions were linearly interpolated from values at cell vertices to the locations of the measured data. The predictions are shown as dotted lines and the measured experiment values as a solid line.

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
Figure 15 Wake survey for grids E and F
Figure 16 Wake survey for grids H and I

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
The averaged circumferential Taylor wake fractions, W1, in the plane of the propulsor, are given in Table 2 for these computations. The table gives values of W1 for each flow computation for a number of radii, namely r/Rmax=0.25, 0.35 and 0.45. The values of W1, derived from the measured experiment data, are 0.474, 0.597 and 0.746 for each of the respective radii.
Table 2 Averaged circumferential Taylor wake fractions for each flow code
r/Rmax
Grid
FLUENT
FIDAP
FLOW3D
0.25
E
0.519
0.241
0.517
F
0.528
0.229
0.519
H
0.523
0.288
1.747
I
0.512
0.304
0.617
0.35
E
0.634
0.311
0.637
F
0.631
0.296
0.640
H
0.635
0.344
1.407
I
0.619
0.367
0.657
0.45
E
0.743
0.409
0.738
F
0.740
0.398
0.740
H
0.742
0.422
1.089
I
0.736
0.451
0.735
The FLUENT/UNS results indicated that further computations with alternative topologies and higher grid resolutions could lead to more accurate predictions of the flow parameters.
Further computations were carried out using FLUENT/UNS for grid G and for grids J to P, the H-H, C-H, C-C and O-O topology grids with 500,000 cells or 1,000,000 cells and the unstructured grids. All of these computations were carried out with identical initial parameters for the inlet conditions and boundary conditions. The same number of iterations were used for every computation; namely 250 iterations, which gave, on average, a reduction of residuals by four orders of magnitude. It was observed that the residuals for earlier FLUENT/UNS predictions for grids F and I had been reduced by only three orders of magnitude. Therefore the computations for grids F and I were repeated.
Contours of the Taylor wake fraction for these predictions are given in figures 17 to 21. These figures show the predicted nominal wake for each of the structured grid topologies and for the unstructured hybrid grids. The smaller grids are shown on the left and the larger grids on the right. Comparison between these prediction and the measured data can be made by comparing these figures with figure 8.
Figure 17 Taylor wake contours for H-H topology grids
Figure 18 Taylor wake contours for C-H topology grids

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
Figure 19 Taylor wake contours for C-C topology grids
Figure 20 Taylor wake contours for O-O topology grids
Figure 21 Taylor wake contours for unstructured grids
The averaged circumferential Taylor wake fractions W1, are shown in Table 3 for each of the grids. These indicate that there is little variation in the predictions for changes in the topology or for increases in grid resolution.
Table 3 Averaged circumferential Taylor wake fractions for each grid
r/Rmax
Resolution
H-H
C-H
C-C
O-O
Unstr
0.25
500,000
0.522
0.527
0.536
0.539
0.573
1,000,000
0.533
0.540
0.538
0.541
0.595
0.35
500,000
0.634
0.638
0.645
0.646
0.685
1,000,000
0.646
0.654
0.649
0.649
0.743
0.45
500,000
0.743
0.744
0.750
0.745
0.779
1,000,000
0.751
0.760
0.752
0.752
0.817
Comparisons of the wake surveys for the predicted and measured velocity components and the turbulent kinetic energy for each of the C-H topology grids are shown in figure 22. This figure indicates the dependency of the predictions on the grid resolution. Comparison between the predicted and measured data for each of the topologies are shown in figures 23 and 24 which indicate the dependency of the predictions on the grid topology.

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
Figure 22 Wake survey comparison between grids H, I and J
Figure 23 Wake survey comparison between grids G and J

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
Figure 24 Wake survey comparison between grids L and N
In addition to the study on grid topology and resolution using FLUENT/UNS, a further study was carried out using CFDS-FLOW3D on variations in the discretisation schemes and turbulence models. Since FLOW3D failed to converge for the C-H topology grids, grid F was used for this study. Six computations were carried out using the k-ε, RNG k-ε and the differential Reynolds Stress turbulence models for first order ‘hybrid' and third order ‘curvature corrected quadratic upwind' discretisation schemes. The third order scheme is guaranteed to preserve the positivity of the turbulence parameters, unlike a standard quadratic upwind scheme.
Taylor wake contours for each of the turbulence models and for each discretisation scheme are given in figures 25 to 27. The ‘hybrid' first order discretisation scheme is shown on the left and the ‘curvature corrected' third order scheme on the right.
Figure 25 Taylor wake contours for k-ε turbulence model

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
Figure 26 Taylor wake contours for RNG k-ε turbulence model
Figure 27 Taylor wake contours for Reynolds Stress model
Figure 28 shows the wake survey data for each of the third order predictions
Figure 28 Wake survey data for third order scheme

OCR for page 1061

Twenty-First Symposium on NAVAL HYDRODYNAMICS
Finally, it is useful to compare the amplitude coefficients of the harmonics of the wake survey data. These amplitude coefficients provide useful information when designing the propulsion system.
Comparison between the coefficients derived from the measured data and the predictions are given below in table 4.
Table 4 Amplitude coefficient of the wake harmonics (×1000)
Harmonic Number
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
Experiment
4.28
12.58
6.51
102.36
10.74
5.66
8.63
50.00
9.48
4.48
2.61
10.72
2.10
0.58
0.80
1.65
H-H grid
2.11
8.85
10.70
63.09
12.73
3.40
1.23
26.86
2.45
0.21
0.17
6.21
0.67
0.01
0.21
2.03
C-H grid
7.17
16.00
14.27
66.18
12.32
4.18
1.73
26.63
1.56
1.10
0.10
5.61
0.16
0.12
0.32
2.64
C-O grid
6.32
30.45
16.00
71.50
12.12
2.73
1.59
26.12
1.08
1.15
0.05
5.58
0.28
0.57
0.37
1.03
O-O grid
0.03
34.90
13.06
74.88
13.57
2.37
2.75
21.87
1.96
0.52
0.44
4.52
0.24
0.61
0.07
1.09
k-ε
0.40
2.44
7.22
39.41
7.42
5.93
2.80
14.25
1.18
1.89
0.38
4.18
0.27
0.19
0.17
0.25
RNG k-ε
1.31
1.32
9.13
51.65
8.38
5.51
2.79
15.41
1.52
1.49
0.67
4.87
0.49
0.32
0.25
0.12
DSM
2.50
1.38
7.61
42.60
7.01
4.84
3.60
24.87
1.52
1.66
0.50
12.06
0.08
0.07
0.04
2.28
Conclusions
The capability of the CFD approach to the prediction of nominal wake has been quantified by comparison with high quality experiment data. In the region of the propulsor, the predictions are qualitatively correct in that the flow features are captured. The predictions have an overall error of around 5% of the reference velocity in the fluid velocity distribution. This compares with an error of 2.5% associated with the measured data. The predictions also fail to capture adequately the harmonics of the measured velocity distribution.
However, the predictions obtained appear to be independent of grid resolution and topology for a given flow solution algorithm. Changing from the isotropic two-equation turbulence models to the anisotropic Reynold Stress model requires further evaluation.
The author wishes to acknowledge the invaluable help and assistance in the preparation of these predictions and this paper by the Computational Hydrodynamics Team at DRA Haslar.
References
1. Report of the 20th ITTC Resistance and Flow Committee. Proceedings of the 20th ITTC. Volume 1. San Francisco, California, September 1993.
2. Huang TT, Liu H-L, Groves NC, Forlini TJ, Blanton JN and Gowing S. “Measurements of Flows Over an Axisymmetric Body with Various Appendages (DARPA SUBOFF Experiments).” Proceedings of the 19th Symposium on Naval Hydrodynamics. Seoul, Korea. August 1992.
3. Groves NC, Huang TT, Chang MS. “Geometrical Characteristics of DARPA SUBOFF Hulls (DTRC Models Nos. 5470 and 5471)”. DTRC/SHD-1298–01 March 1989. David Taylor Research Center, Bethesda, Maryland 20084–5000
4. Lin CW, Smith GD, Fisher SC. “Numerical Flow Simultations on the DARPA SUBOFF Configurations”. DTRC/SHD-1298–09 July 1990. David Taylor Research Center, Bethesda, Maryland 20084–5000
5. Shaw JA, Georgala JM, May NE, Pocock MF. “Application of Three-Dimensional Hybrid Structured /Unstructured Grids to Land, Sea and Air Vehicles”. Proceedings of Numerical Grid Generation in Computational Fluid Dynamics and Related Fields. Swansea, UK. 1994, pp 687–695
6. Patis CCP, Bull PW. “The Generation of Viscous Grids for Hydrodynamic Vehicles”. Mississiippi State University, Starkville, April 1996.
7. “CFDS-FLOW3D Users' Guide”. CFDS. Building 8.19, Harwell Laboratory, Oxfordshire, OX11 0RA. United Kingdom
8. “FLUENT/UNS Users' Guide”. Fluent Inc., Centerra Resource Park, 10 Cavendish Court, Lebanon. USA. NH 03766
9. “FIDAP 7.5 Users' Guide” FDI Inc., 500 Davis Street, Suite 600, Evanston, USA. Illinois 60201 .