^{1}

^{*}

^{1}

^{2}

^{3}

^{4}

^{1}

^{1}

Autonomous Underwater Vehicles (AUV’s) are considered as advanced classes of vehicles, capable of performing pre-established missions without physical communication with the ground or human assistance. The research and development of this type of vehicles have been motivated, due to its excellent characteristics, ideal to the military, scientific and industrial sectors. Thus, the objective of this paper is to study fluid flow behavior past over AUV’s, without and with control surfaces (rudders), by Computational Fluid-Dynamics (CFD), aiming to obtain information about the impact of the operating depth and control surfaces on the vehicle's hydrodynamics, in order to help researchers and designers of this class of vehicles. Results of the drag coefficient, pressure, velocity and streamlines distribution around the vehicles are presented and analyzed.

An Autonomous Underwater Vehicle, or AUV, can be defined as a vehicle that travels submerged, without physical communication with the ground and without the need of a human operator. The AUV’s are included in Unmanned Underwater Vehicles group, well better known as UUV’s.

During the last years research and development of AUV’s have increased significantly because of the extremely favorable characteristics they have, such as the ability to operate autonomously in hostile environments [

The application of AUV’s has been growing by the constants technological advances, mainly in electronics and robotics, allowing the execution of high precision missions, the reduction in the costs of design and operation, and the increase in embedded equipments quality, as well as for new technologies of batteries and power management, enabling the increase in autonomy, maintenance and safety in operations with this class of vehicles [

The use of numerical techniques to solve engineering problems is nowadays a reality due to the development of high processing capacity computers. These techniques have many advantages, being able to solve complex problems (which exact solutions can’t be obtained and often can’t be reproduced by experiments), in less time and with a lower cost compared to experimental techniques.

Actually tools of Computational Fluid-Dynamics (CFD), which is an area of science that study, through numerical simulation, fluid flow, heat transfer, and related transport phenomena, are integrated with others numerical tools, creating a complete design environment, allowing that experiments are done only for final configurations, validations and tests. Many recently researches uses CFD techniques to study AUV problems [

Most existing AUV’s uses batteries as power supply for their propulsion systems. However, large drag during the vehicle navigation results in more energy consumption and, consequently, reduction in the vehicle autonomy, which is undesirable by any designer. In this context, this paper aims to evaluate numerically the influence of operation depth, which is operational basic parameter, in the AUV drag coefficient, without and with control surfaces, by CFD. The intention is to obtain data to assist researchers and designers in future projects related to this class of vehicles.

The hull of the AUV studied is torpedo type (cylindrical body with a large ratio between the length and the diameter), due to their good characteristics, like low hydrodynamic drag, good internal volume, simplified access to all equipment and reduction of manufacture cost, making this type of hull the most used by the main commercial manufacturers of this class of vehicles.

To model the profiles of the bow and stern of the vehicle it was used the Myring Equations (Equations (1) and (2)). These theoretical equations describe the shape of the torpedo bodies which generate low drag coefficient [

a) Bow:

r 1 ( x 1 ) = 1 2 D [ 1 − ( x 1 − a a ) 2 ] 1 / n (1)

b) Stern:

r 2 ( x 2 ) = 1 2 D [ 3 D 2 c 2 − tg θ c ] x 2 2 + [ D c 3 − tg θ c 2 ] x 2 3 , (2)

where the parameters of these equations are shown in

In this paper the geometric parameters of AUV’s hull considered are shown in

Geometric details of the AUV rudders (NACA0015 profiles) are shown in _{t}⁄D = 7.44, similar the ratio of AUV analyzed in this paper (L_{t}⁄D = 10.00).

For simplification of the analysis, the effect of the propellant over the flow around the AUV was not considered.

For the solution of flow problems using CFD tools is necessary to define continuous fluid domain around the body studied. The continuous domain is then subdivided

Parameter | Value |
---|---|

L_{t} = a + b + c (mm) | 1400 |

a (mm) | 250 |

b (mm) | 700 |

c (mm) | 450 |

D (mm) | 140 |

n (-) | 2 |

θ (˚) | 20 |

into small control volumes, becoming it a discrete domain. The set of these control volumes is commonly referred to as the “numerical mesh”.

In this paper were create two semi-cylindrical fluid domains (one for AUV with rudders and another for AUV without rudders), aiming to obtain meshes with smaller numbers of control volumes, thus reducing the computational cost. The dimensions of these domains (_{t}⁄D = 9.00, and are shown in

For generation of the geometries and numerical meshes that represent the studied domains was used the commercial software ICEM-CFD 15.0.

Initially it was procedure the mesh convergence study, aiming to obtaining independence of simulations results, due to the increment of mesh elements. The numerical meshes used are hybrids (tetrahedral and prisms control volumes), with 454,950 elements (medium y^{+} = 11) for the situation of AUV without rudders

(mesh 1) and 1,012,855 elements (medium y^{+} = 8) for the situation of AUV with rudders (mesh 2), and are showed in

y^{+} is a dimensionless distance that is a relevant parameter in the modeling of external flow. This parameter, which is commonly used to define the ideal mesh refinement in the wall regions, is calculated by the following equation:

y + = Δ n μ / ρ τ w , (3)

where Δn is the height of the first layer of control volumes, measured vertically to the wall, µ is the fluid dynamic viscosity, ρ is the fluid density and τ_{w} is the shear stress in the wall.

Parameter | Value |
---|---|

A (mm) | 0.5L_{t} = 700 |

B (mm) | 3L_{t} = 5200 |

R (mm) | 3D = 420 |

Much care must be taken when constructing numerical meshes aimed at solving problems of flow around immersed bodies. Here, many factors were taken into account [

δ = 0.035 L t R e − 1 / 7 , (4)

where Re is Reynolds number of the flow, calculated as follow:

R e = ρ | U | L t μ , (5)

where | U | is the norm of flow velocity vector and µ is the fluid dynamic viscosity. The meshes were built with great refinement near the surface of the AUV (boundary layer region), in order to encompass precisely the viscous effects of the flow around the AUV.

The Reynolds number can be defined in volumetric basis, as follows:

R e V = ρ | U | V 1 / 3 μ , (6)

where Re_{v} is the volumetric Reynolds number of the flow, and V is the volume of AUV hull.

To investigate the single-phase flow around the AUV, it was considered a three-dimensional, steady-state, incompressible, isothermal and turbulent flow.

The general equations used in this work are:

a) Mass conservation equation:

∂ ρ ∂ t + ∇ ⋅ ( ρ U ) = 0 , (7)

b) Momentum conservation equation:

∂ ( ρ U ) ∂ t + ∇ ⋅ ( ρ U ⊗ U ) − ∇ ⋅ ( μ e f f ∇ U ) = − ∇ p ′ + ∇ ⋅ ( μ e f f ∇ U ) T + ρ g , (8)

where p' is the corrected pressure, which depends of turbulent model to be used, g is the local gravity acceleration vector (adopted value 9.81 m/s^{2}) and µ_{eff} is the effective viscosity, calculated as follows:

μ e f f = μ + μ t , (9)

where µ_{t} is the turbulent viscosity.

c) Turbulence model equations:

It is necessary to add in the model new equations to predict the phenomenon of turbulence that is present in the flow. The turbulence consists of fluctuations in the flow field in time and space (time-dependent velocity and pressure fields).

It is a complex process and can have a significant effect on the flow characteristics. Turbulence occurs when the inertial forces acting on the fluid becomes significantly higher than the viscous forces and is characterized by a high Reynolds Number of the flow. Turbulence can also be caused by surface roughness, which induces secondary flow (i.e. vortices) [

The turbulence model adopted in this work is the Shear Stress Transport model (SST model), with the kinetic boundary layer fully turbulent. This model is based on the k-ω turbulence model. This model was used because of its good treatment of external flow with high Reynolds numbers.

The SST model introduces two new variables in the problem, which is the turbulent kinetic energy (k) and the turbulent frequency (ω). These variables are calculated, respectively, by:

∂ ( ρ k ) ∂ t + ∇ ⋅ ( ρ U k ) = ∇ ⋅ [ ( μ + μ t C k 1 ) ∇ k ] + P k − C k 2 ρ k ω , (10)

where P_{k} is the turbulence production, C_{k}_{1} = 2.000 and C_{k}_{2} = 0.090. And:

∂ ( ρ ω ) ∂ t + ∇ ⋅ ( ρ U ω ) = ∇ ⋅ [ ( μ + μ t C ω 1 ) ∇ ω ] + C ω 2 P k ω k − C ω 3 ρ ω 2 , (11)

where C_{ω}_{1} = 2.000, C_{ω}_{2} = 0.556 and C_{ω}_{3} = 0.075. In the SST model the parameters µ_{t}, p' and P_{k} are given as follows:

μ t = ρ k ω , (12)

p ′ = p d + 2 3 ρ k and (13)

P k = μ t ∇ U ⋅ ( ∇ U + ∇ U T ) − 2 3 ∇ ⋅ U ( 3 μ t ∇ ⋅ U + ρ k ) , (14)

where p_{d} is the dynamic pressure, calculated by the equation:

p d = 1 2 ρ | U | 2 . (15)

Total pressure, p_{t}, is calculated by:

p t = p s + p d , (16)

where p_{s} is static pressure.

According to [

The friction drag is due to the boundary layer surface shear stress, while pressure drag is due to pressure difference in the flow direction resulting from formation of the wake in the downstream region.

The drag on a body is usually expressed in terms of a dimensionless drag coefficient. The total drag coefficient in volumetric basis is calculated by:

C d v = C d p v + C d f v = F d p 1 2 ρ U ∗ 2 V 2 / 3 + F d f 1 2 ρ U ∗ 2 V 2 / 3 , (17)

where C_{dv} is the volumetric drag coefficient, C_{dpv} is the volumetric pressure drag coefficient, C_{dfv} is the volumetric friction drag coefficient, F_{dp} is the pressure drag force, F_{df} is the friction drag force and U_{*} is the free stream parallel fluid velocity. The parameters F_{dp} and F_{df} are calculated by:

F d p = ( ∫ A p d d A ) i ^ , (18)

F d f = ( ∫ A τ w d A ) i ^ , (19)

where A is the AUV superficial area and i ^ is the unit vector in the parallel flow direction.

The fluid adopted in the validations simulations was pure water. The physical properties of this fluid are shown in

The fluid adopted in the simulations that evaluates the influence of operation depth in drag coefficient was sea water with 35 g/L of salinity. The physical properties of this fluid, for equatorial and tropical areas, are shown in

Boundary | Condition | Value |
---|---|---|

Inlet | Prescribed velocity | 0.4 i ^ - 1.4 i ^ m/s |

Wall | Prescribed pressure³ | 5.1 - 10.2 MPa |

AUV surfaces¹ | Prescribed velocity | 0 m/s |

Outlet^{2} | Prescribed pressure³ | 5.1 - 10.2 MPa |

Symmetry plane | Symmetry | - |

^{1}No slip and smooth wall; ^{2}Opening condition; ^{3}On the operation depth in the water.

Propertie | Value |
---|---|

Density (kg/m³) | 997 |

Dynamic viscosity (mPa∙s) | 0.8899 |

Depth (m) | Temperature (˚C) | Density (kg/m^{3}) | Dynamic viscosity (mPa∙s) |
---|---|---|---|

500 | 25 | 1023 | 0.9600 |

750 | 15 | 1026 | 1.2300 |

1000 | 3 | 1028 | 1.7200 |

In order to predict the drag coefficients at different situations, it was proposed the following linear model for these parameters as a function of the operation depth (Y):

C = A ¯ + B ¯ ⋅ Y , (20)

where A ¯ and B ¯ are coefficients of the equation and C is the dependent variable (C_{dv}, C_{dpv} or C_{dfv}).

This model was fitted by numerical simulations and the least square error technique. For all of the simulations was used the commercial software ANSYS-CFX 15.0, which makes use of the finite volumes method based on finite elements method to solve the problem under study.

Equation (20) is valid in the interval 500 ≤ Y (m) ≤ 1000.

To validate the methodology for constructing the numerical meshes and mathematical model used in this study, was done comparison between the predicted volumetric drag coefficient and the obtained experimentally by [

Parameter | Consideration |
---|---|

Primary convergence criterion | Root Main Square (RMS) equations error < 10^{−5} |

Secondary convergence criterion | Reached 300 iterations, with convergence of C_{dv} |

Advection scheme | High resolution |

Interpolation scheme for pressure | Trilinear |

Interpolation scheme for velocity | Trilinear |

U_{*} (m/s) | Re × 10^{−5} (-) | Re_{V} × 10^{−5} (-) | Experimental C_{dv}¹ (-) | Numerical C_{dv} (-) | Difference between numerical and experimental C_{dv}^{2} (%) |
---|---|---|---|---|---|

0.4 | 6.27 | 1.05 | 0.0489 | 0.0460 | 5.9 |

0.6 | 9.41 | 1.57 | 0.0451 | 0.0424 | 6.0 |

0.8 | 12.55 | 2.10 | 0.0434 | 0.0401 | 7.6 |

1.0 | 15.68 | 2.62 | 0.0419 | 0.0385 | 8.1 |

1.2 | 18.82 | 3.15 | 0.0407 | 0.0372 | 8.5 |

1.4 | 21.96 | 3.67 | 0.0389 | 0.0362 | 6.8 |

1 [^{2}Calculated by | C d v n u m e r i c a l − C d v e x p e r i m e n t a l | C d v e x p e r i m e n t a l × 100 % .

AUV without rudders. From the analysis of the results we can note that the maximum and the average difference between the predicted and experimental volumetric drag coefficients were small, 8.1% and 7.2%, respectively. These deviations can be attributed to the association of experimental errors, numerical errors and the small variation between the computationally simulated hull geometry and that used in the experiments. The low deviations between the results validate the methodology used in this work, showing that it describe well the studied physical phenomenon.

Figures 8-10 show the comparison between results of volumetric drag coefficients, volumetric pressure drag coefficient and volumetric friction drag coefficient, respectively, versus operating depth obtained for AUV without (

Y (m) | Re × 10^{−5} (-) | Re_{V} × 10^{−5} (-) | C_{dv} (-) | C_{dpv} (-) | C_{dpv}/C_{dv} (%) | C_{dfv} (-) | C_{dfv}/C_{dv} (%) |
---|---|---|---|---|---|---|---|

500 | 14.92 | 2.71 | 0.0399 | 0.0050 | 12.5 | 0.0349 | 87.5 |

750 | 11.68 | 2.12 | 0.0421 | 0.0053 | 12.6 | 0.0368 | 87.4 |

1000 | 8.37 | 1.52 | 0.0447 | 0.0057 | 12.8 | 0.0390 | 87.2 |

and with (

From analysis of these results it can be verified a linearly increasing behavior of the volumetric drag coefficient with the increase in the operation depth for both situations, AUV without and with rudders. This phenomenon can be explained,

Y (m) | Re × 10^{−5} (-) | Re_{V} × 10^{−5} (-) | C_{dv} (-) | C_{dpv} (-) | C_{dpv}/C_{dv} (%) | C_{dfv} (-) | C_{dfv}/C_{dv} (%) |
---|---|---|---|---|---|---|---|

500 | 14.92 | 2.71 | 0.0796 | 0.0341 | 42.8 | 0.0455 | 57.2 |

750 | 11.68 | 2.12 | 0.0830 | 0.0352 | 42.4 | 0.0477 | 57.6 |

1000 | 8.37 | 1.52 | 0.0885 | 0.0363 | 41.0 | 0.0522 | 59.0 |

basically, by the significant increase in sea water viscosity due to the considerable drop in temperature as AUV moves deeper into the ocean layers.

Further, it was observed that the average volumetric drag coefficient of AUV with rudders is approximately twice when compared with the situation of AUV without rudders, showing that the use of control surfaces has a strong impact on the total drag of the vehicle, for the simulated conditions. It was also verified an almost constant value of the volumetric pressure drag coefficient with the increase in the operation depth, for the AUV in both situations (without and with rudders), showing that the change in the operational depth parameter has little influence on the pressure drag of the vehicle. In the case of AUV with rudders it was observed a volumetric pressure drag coefficient almost 7 times higher than the situation of AUV without rudders, due to the 68% increase in the frontal area of the vehicle. This additional part in the vehicle generates an increase in the flow separation and consequent increase in the wake region. Furthermore, it was possible to verify that the average percentage of pressure drag in relation to the total drag of the vehicle increased from 12.6% to 42.4%, considering the AUV without and with rudders, respectively. As reported in the methodology, based on the simulations results it were obtained correlations between the parameters C_{dv}, C_{dpv} and C_{dfv} as a function of the operation depth, Y.

It was also found that volumetric friction drag coefficient for the AUV with rudders is approximately 30% higher than the obtained with the AUV without the rudders, due to the 29% increase in vehicle wetted area, thus increasing the area subjected to viscous shear stress generated by the fluid flow. In addition, it was possible to verify that the average percentage of frictional drag in relation to the total drag of the vehicle dropped from 87.4% to 57.6%, considering AUV with and without rudders, respectively.

In

Based on the high determination coefficient reported in ^{2} > 0.96), we can verify that a good agreement was obtained. Thus, we state that all drag coefficients present linear behavior with operation depth, in both AUV design.

AUV | Equation | Dependent variable (-) | Coefficient A ¯ (-) | Coefficient B ¯ × 10^{4} (m^{−1}) | R^{2} (-) |
---|---|---|---|---|---|

Without rudders | 21 | C_{dv} | 0.0351 | 0.0956 | 0.9961 |

23 | C_{dpv} | 0.0043 | 0.0137 | 0.9951 | |

25 | C_{dfv} | 0.0308 | 0.0820 | 0.9963 | |

With rudders | 22 | C_{dv} | 0.0703 | 0.0178 | 0.9802 |

24 | C_{dpv} | 0.0318 | 0.0452 | 0.9998 | |

26 | C_{dfv} | 0.0385 | 0.1327 | 0.9634 |

Further, it is verified high pressure values and low range of this parameter. This is due the high contribution of static pressure, p_{s}, in the total pressure, due the big depth in that the study was performed. For the case of AUV with rudders there are additional high pressure zones at the leading edges of the rudders, as well as additional low pressure zones at the rudder tips. The same pressure behavior was verified for simulations in operation depths of 500 and 1000 m.

figure we can see that there are low velocities zones on the leading edge and in the wake region of this rudder, as well as symmetrical high velocities zones on their both sides, a physically expected fact, due the characteristics already mentioned of NACA0015 profile and the null attack angle of vehicle. Similar behavior was verified for simulations in operation depths of 500 and 1000 m.

plane located 0.15 m from the AUV centerline (crossing one of the rudders), respectively, for operation depth 750 m. From the analysis of these figures we can verify that the streamlines were quite ordered around the AUV, which is due to the good hydrodynamic geometry of the hull and rudders of the vehicle. The same pattern was verified for simulations in operation depths of 500 and 1000 m.

This paper study the fluid flow behavior past over AUV’s, without and with control surfaces (rudders), by Computational Fluid-Dynamics (CFD). Results of the drag coefficient, pressure, velocity and streamlines distribution around the vehicles were presented and analyzed.

Based on the results it can be concluded that the numerical-mathematical model used in this paper represented well the phenomenon of the flow around the AUV studied and that the methodology used was satisfactory. It was also observed that the average total drag of the AUV with rudders was about twice higher than the AUV without rudders, and the contribution due to pressure and friction effects are practically constant and increasing, respectively, when the operation depth is increased, for both situations, with and without rudders. Additionally, it was obtained a linear model to predict the drag coefficients as a function of the operation depth. Finally, the study has proved that CFD tools have strong relevance in the development and improvement of naval projects, being essential in the current scenario of technological advances and cost reduction.

The authors would like to express their thanks to Brazilian Research Agencies CNPq, CAPES and FINEP for supporting this work, and are also grateful to the authors of the references that helped in the improvement of quality of this paper.

The authors declare no conflicts of interest regarding the publication of this paper.

de Sousa, J.V.N., de Lima, A.G.B., Batista, F.A., de Souza, E.C., de Macedo Cavalcante, D.C., de Morais Pessôa, P. and do Carmo, J.E.F. (2020) On the Study of Autonomous Underwater Vehicles by Computational Fluid-Dynamics. Open Journal of Fluid Dynamics, 10, 63-81. https://doi.org/10.4236/ojfd.2020.101005