On the Study of Autonomous Underwater Vehicles by Computational Fluid-Dynamics

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.


Introduction
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 [1] [2], such as unexplored or contaminated areas, enemy territorial seas or deep waters. All ways of using AUVs are very interesting for the military, scientific and industrial sectors.
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 [3].
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 [4]- [10].
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 Geometry
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 [11], and are given as follows: a) Bow: where the parameters of these equations are shown in Figure 1.
In this paper the geometric parameters of AUV's hull considered are shown in Table 1. These parameters were based on dimensions of Afterbody1 hull, studied by [12].
Geometric details of the AUV rudders (NACA0015 profiles) are shown in Figure 2, and are based on [13] and on the Pirajuba AUV studied by [3], which has ratio L 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.

The Physical Domains and the Numerical Meshes
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   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 ( Figure 3) were based in the work of [5], that studied the flow around AUV hull (torpedo type) with L t ⁄D = 9.00, and are shown in Table 2.
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 Figure 4. The refinement of both meshes are similar, but mesh 2 has more than twice the numbers of elements of mesh 1 due to rudders (27% additional surface area), which require a large quantity of additional prismatic elements near these control surfaces.
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: 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.  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 [14]. It was used an equation that provides the average thickness of the kinetic boundary layer (region where viscous flow effects are important) around immersed bodies, δ, as follows: where Re is Reynolds number of the flow, calculated as follow: 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: where Re v is the volumetric Reynolds number of the flow, and V is the volume of AUV hull. Figure 5 shows details of the mesh 2 around the region of bow, upper rudder and stern, respectively.

Mathematical Modeling
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: b) Momentum conservation equation: 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: where µ t is the turbulent viscosity.  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) [15].
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: where C ω1 = 2.000, C ω2 = 0.556 and C ω3 = 0.075. In the SST model the parameters µ t , p' and P k are given as follows: where p d is the dynamic pressure, calculated by the equation: Total pressure, p t , is calculated by: where p s is static pressure.
According to [16], the action of viscosity is diminish the fluid velocity past a surface and, thus, decreasing the fluid momentum within the boundary layer. It strongly affects the overall flow behavior past the surface. Since, fluid flow is governed by the pressure distribution on the boundary layer. We must analyze both the retarding action of viscosity and the imposed pressure distribution.
Thus, the drag coefficient in the flow was determined. The total drag force is generated by the friction and pressure forces acting on a body immersed in a flowing fluid.
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: 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: where A is the AUV superficial area and î is the unit vector in the parallel flow direction. Figure 6 shows the domain with indicative information related to boundary conditions and Table 3 shows specified values of these boundary conditions.

Boundary Conditions and Fluids Properties
The fluid adopted in the validations simulations was pure water. The physical properties of this fluid are shown in Table 4.
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 Table 5. Table 6 shows the considerations adopted for the numerical solver.   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): where A and B are coefficients of the equation and C is the dependent variable (C dv , C dpv or C dfv ).

AUV without Rudders (Validation)
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 [12], that studied similar AUV without rudders. Table 7 and Figure 7 show the comparison between the numerical and experimental volumetric drag coefficients versus volumetric Reynolds number for        and with (Table 9) rudders, and free stream fluid velocity equal to 1.0 m/s. 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, basically, by the significant increase in sea water viscosity due to the considerable drop in temperature as AUV moves deeper into the ocean layers. 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.

AUV without and with Rudders (Hydrodynamic Analysis)
In    Figure 11. Pressure field around the AUV without rudders. 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.        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.

Conclusions
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.