Computational fluid dynamic study on design and modification of underwater remotely operated vehicle

Remotely Operated Vehicle (ROV) has been widely used in numerous underwater exploration applications such as exploration of complex deep sea environment, pipeline detection, installation, maintenance, and repair. Thus, it is worthy to design, optimize, and performance evaluation of ROV systems for underwater exploration purposes. Computational Fluid Dynamic (CFD) is a computational approach that is very helpful and widely used to examine the flow characteristics of ROV systems. In this research work, CFD analyses of ROV bodies with different thruster blades were carried out in order to generate thrust forces by the thruster blades. For this purpose, ANSYS FLUENT was used to examine the flow characteristics over the ROV body. The analyses were performed at different flow velocities, such as 1 m/s, 1.5 m/s, 2 m/s, 2.5 m/s, 3 m/s and 3.5 m/s. The outcomes were in the form of thrust force, drag force, pressure distribution, and velocity distribution. The result shows that four-blade thruster generates maximum thrust force as compare to other ROV thruster models. The main reason behind this higher thrust force is due to the larger motion of the fluid. Similarly, drag force was also investigated and observed that the drag force is greater for thruster model 3, having four blades due to the large frontal area of the ROV body and thruster blades. The results obtained in this study are very helpful for engineers and researchers to design and optimize ROV models using numerical methods.


Introduction
The requirement for seabed surveys prompted the development of modern underwater technology.New methodologies have been developed since the 1950s, but even in the 1960s, when the offshore gas fields in the southern North Sea were established, knowledge of seabed stratigraphy was limited [1].In order to guarantee a stable seabed that can support the focused strain needed for subsea structure foundation, all prospective fixed platform locations must be examined with adequate accuracy.Due to incomplete information from early surveys, operators have been forced to relocate the location of a project at the last minute or remove rocks from a site quickly in the North Sea [2].The necessity for more accurate underwater surveys and better underwater positioning and navigation technologies is highlighted by these situations.The appropriateness of the seabed sediment for burying the pipeline is determined by a geophysical analysis of the underlying strata once a suitable path has been selected [3].After completion, annual side-scan sonar and sub-bottom profile surveys are required to verify the depth of burial.Offshore oil firms discovered the value of doing underwater surveys of the seafloor and sub-seabed conditions before undertaking any offshore engineering work, such as platform installation, pipeline laying, or semisubmersible anchoring, after a string of disasters that started in the 1970s [4].In general, the cost of such a survey is insignificant when compared to the potential hazard and expense of a seafloor collapse.As exploration has progressed deeper into the ocean, Under the Offshore Installations Regulations of 1975, a diving bell must be used below 50 meters.Saturation diving has become important as decompression times have increased [5].The offshore industry has created several atmospheric diving suits, manned and unmanned submersibles, and underwater surveying and inspection operations to get around the problems of decompression [6].Driverless techniques have become the favored solution in deep water.The usage of a ROV (Remote Operated Vehicle) as a main or backup working system is required for many underwater tasks.A range of data collection tools and contemporary manipulators for handling items are included in the general-purpose ROV kit [7].The market locks that human submersibles and saturation divers had on the market prevented these new invaders from gaining ground, despite the fact that their design goals were successfully achieved.These underwater robots are usually operated like video games by a person on a surface ship using a joystick [8].Determined the hydrodynamic forces and coefficient of an underwater vehicle using a numerical and experimental approach.They measured the hydrodynamic coefficient and flow properties across the vehicle body for the purposes of numerical study using Computational Fluid Dynamics (CFD) Fluent [9].With the significant growth of the computer hardware capability in the recent decades, the applications of Computational-Fluid Dynamics (CFD) in the hydrodynamics study tend to become prevailing [10][11][12][13].Skorpa [14] studied the drag, lift and moment history for the ROV model with different turbulent models in FLUENT.Numerical modelling was carried out to the ROV and validated by a free-decaying model testing [15,16].L. Hong, X. Wang.[17] evaluated two kinds of forced, in which both the steady-state and unsteady-state conditions were simulated considering the wall effects [18].Generally, the simulation of a six-DoF dynamics model of the ROV is more challenging than that of a torpedo-shaped streamlined autonomous underwater vehicle (AUV) which has an analytical solution [19].According to current literature, it was investigated that CFD can be utilized to evaluate the performance of ROV models.It was also examined from the current literature; many authors have worked on different parameters like control systems, navigation systems, etc., but still there are much potential is existed and need to work on geometrical parameters using CFD approach.CFD is particularly useful for understanding complex fluid phenomena such as turbulence, which is a fundamental aspect of many fluid systems.By using numerical methods to solve the Navier-Stokes equations, CFD simulations can provide insights into the behavior of fluids that are difficult to study experimentally [20].CFD has become a vital tool for engineers and scientists to design and optimize complex fluid systems, and it continues to be an active area of research and development.However, the tool of CFD still plays an important role considering the limitation of the model test in the cost, test model scale and facility capability [21].In this current research, performance analyses of ROV models with different blades thruster were carried out to find the lowest drag force and high-speed ROV structure model using a CFD approach.For this purpose, ANSYS FLUENT 2020 R2 was used to examine the flow behavior over the ROV body and determine the lowest drag force and highest thrust force at different water flow velocities such as 1 m/s, 1.5 m/s, 2 m/s, 2.5 m/s, 3 m/s, and 3.5 m/s.

Numerical methodology
Computational Fluid Dynamics (CFD) analyses of ROV models with two blades, three blades, and four blades thrusters were performed at different water flow velocities (1 m/s, 1.5 m/s, 2 m/s, 2.5 m/s, 3 m/s, 3.5 m/s) in order to determine the drag force and drag coefficient of the ROV models.The ANSYS Fluent was used for the performance analysis of ROV models.First of all, ROV models were made using Solidworks and then imported into ANSYS design modeler for further simulation.The complete description of the numerical methodology of ROV models is shown in Figure 1.      3. The units were used for modeling all ROV models millimeters.In this proposed structure model, two thrusters are installed on the both side of the model.In addition, the camera system and other control systems are inserted inside the ROV structure model.The curve surface of the ROV structure model helps to decrease the drag force and increase the velocity of the ROV body.Two thrusters are mounted on the both sides of the model.The diameter of the thruster blades is 240 mm.This ROV structure model total length of the ROV body is 454 mm and width is 200 mm.In addition, total vertical height of the ROV body is 105 mm.

Computational domain
The important part of CFD simulation is to make computational domain.The computational domain is generally defined as a region which surrounds the building model where basic governing equations such as the equation of continuity, the conservation of energy, and the equation of momentum are discredited and solved [22].To analyze the aerodynamic behavior of the ROV model, for instance, a rectangular box is generated and extracted a ROV body.The total length of rectangular box is 3 m; width and height are 1m and 2 m respectively.In the three-dimensional views presented in Figure 4, the complete description of the ROV model's computational domain is given [23].Moreover, the simulations were conducted at six different water flow velocities such as 1 m/s, 1.5 m/s, 2 m/s, 2.5 m/s, 3 m/s, 3.5 m/s.The main reason to choose these six different flow velocities is to examine the flow behavior at different flow conditions because ROV is subjected to different flow conditions.

Grid generation in ANSYS mechanical
Meshing is generally a sub-division of the computational domain.Meshing can be defined as the division of a computational part into finite sub-parts.Meshing plays an important role in numerical simulation.Thus, meshing quality is the most important factor in the accuracy of simulation results.After creating the computational domain in ANSYS Fluent design modeler, it is necessary to generate appropriate meshing to attain accurate results [24].The mesh elements are growing in a direction perpendicular to the surface of the ROV body into the fluid.The mesh was smoothed to ensure a continuous transition between elements.This is important for calculating the transition from laminar to turbulent flow.The mesh of the main domain around the ROV model is shown in Figure 5.In this work, unstructured and tetrahedron meshing is drawn due to the complexity of the ROV model.This computational body's total nodes and elements are 604620 and 3198744, respectively.Mesh of the three-dimensional flow domain or computational domain and cut section of mesh structure are shown in Figure 4.

Mesh independence study
A suitable mesh density plays an important role in order to obtain an accurate solution since the computational cost and precision of the solution are highly dependent on the number of elements.In this study, mesh independence is examined at different degrees of refinement until there is little to no significant quantitative variance in the answers.Table 1 is a list of the different mesh refinement levels.The relative errors were also calculated between the two results of drag and thrust force values.It was observed from Table 1 that the relative errors were less than 5% when rough mesh was drawn and the relative errors were reduced to less than 1% when mesh is too refine.It shows that there is no significant variation in the outcomes of drag and thrust force values.Drag and thrust forces on the ROV bodies are chosen as the variables to change with various mesh refinement levels in order to assess mesh independence.The selected mesh refinement level of 4 is employed for CFD analysis and includes 3198744 elements and 604620 nodes with average orthogonal quality, aspect ratio, and skewness, respectively, of 0.85, 1.82, and 0.22.According to the findings of the mesh independence research, refinement level 4 is regarded as the optimal mesh and falls within the acceptable range for CFD simulations in order to guarantee the accuracy of hydrodynamic coefficient calculation at a reasonable computational cost.For CFD analysis in HSHKT, a mesh independence test was conducted, and 181627 [25] with average aspect ratio, skewness, and orthogonal quality of 1.96, 0.25, and 0.84 respectively were nominated.The description of the computational domain's mesh research is presented in Table 1.It has been discovered that the computational findings and experimental results accord much more closely.Hence, the current computational findings fall within a reasonable range.In a similar manner, [26] performed a grid independence test for a CFD study of a propeller turbine runner and chose 4080993 total numbers of elements with skewness, aspect ratio, and average orthogonal quality of 0.23, 1.79, and 0.82, respectively.As a result, the mesh parameters that are supplied are acceptable.

Mathematical modeling of numerical simulation
The flowing fluid field near the ROV body region in the stream can be described by using Reynolds number.The Reynolds number can be expressed below [27]  Where Re is Reynolds number,  is the fluid density,  U is flow velocity, D is the diameter,  is the dynamic viscosity.A Reynolds number of 14.33x106, depending on the size of the computational domain, was used for the numerical calculations.The K-SST, the most practical turbulence model, is used for numerical simulation that resolves two separate transport equations for determining turbulent kinetic energy and dissipation rate.The numerical simulations for the ROV structure are conducted using the governing equations under the following assumptions: that the flow is three-dimensionally incompressible and steady-state [28].Based on these predictions, the equations that follow may be expressed as: Equation of conservation of mass Where u is the velocity vector, ρ is density, t is time, p is the pressure, τ is the stress tensor, S M is momentum source.
Equation of turbulence kinetic energy Equation of specific dissipation rate Where k turbulence kinetic energy,  is the specific dissipation rate,  is the closure coefficient, S is the mean rate-of-strain tensor 1 F is the blending functions.

Simulation boundary conditions
Through the fluid numerical simulation software ANSYS FLUENT 2020 R2, the water flow of a large ROV body under the condition of multi-degree-of-freedom motion was analyzed.The settings for the dynamic performance calculation for this numerical simulation of a three-dimensional steady-state flow are set to the following values [29].The ROV structure body is long the unidirectional flow model is used to move underwater during the period, when determining the hydrodynamic performance of ROVs; the turbulence model selects the k-w model which takes into account the effects of low Reynolds numbers compressibility and shear flow dispersion.In addition, the rotational speed of ROV propeller blades is 1450 rpm.However, for each the corresponding characteristic length and characteristic velocity need to be modified for the working condition.The pressure-velocity coupling approach is used to solve the turbulence equation and the momentum equation is discredited using the central difference format.In addition, Jacobi iterative method is used for iterations.The upper and lower computational domain limits are specified using hydrostatic pressure, and the inlet and outlet bounds, as well as the borders on both sides, are defined for far-field situations.The ROV body is set to a standard wall function.The fluid parameters are set to 20 degrees Celsius and the density to 1025kg/m3 of seawater, the dynamic viscosity coefficient is 8.90 × 10−4 Pa.s.

CFD reliability verification
The reliability of the CFD simulation is most important to compute accurate results.In validation, the assessment of CFD results was conducted at different parameters such as comparison of results with physical setup, comparison of results with current literature etc.In this work, for validation purpose, the comparison of computational fluid dynamics (CFD) results was carried out with current literature.The CFD simulations were performed at different flow velocities.The comparison of drag force at various flow velocities is shown in Figure 6.It was examined from the obtained results that there is no major difference between the present work and Ahmad Zarei et al. [30].The maximum drag force was observed at a flow velocity of 20 m/s, and the minimum drag force was noted at 5 m/s.The percentage error between the present work and from the current literature is observed less than 5%.Similarly, the variation of lift force at different flow velocities was also examined in Figure 5.It is evident from the obtained results that the maximum lift force was at a flow velocity of 25 m/s and the minimum at a flow velocity of 5 m/s.In addition, the percentage error between the present work and the current literature are less than 5%.

Results and discussions
Computational Fluid Dynamics (CFD) analyses of ROV designs with different thruster models are performed in order to determine the drag force and thrust force and examine the flow characteristics around the ROV walls.For this purpose, the water flow velocities of 1 m/s, 1.5 m/s, 2 m/s, 2.5 m/s, 3 m/s, and 3.5 m/s were used for CFD analyses.Variations of drag force with the variation water flow velocities for ROV designs with different thruster models were also described.Variations of drag force and thrust force with the variation water flow velocities for three different thruster blades attached to ROV model are listed in Tables 1 and 2. It can be seen from the computed results in Tables 2 and 3 that drag forces and thrust forces are increased with the increase of flow velocity on the ROV model.According to computed results, the maximum drag forces are observed with 2 blades thruster, and the minimum drag forces are observed with 3 blades thruster.Similarly, the maximum and minimum thrust force was also examined, which is 2.3 N and 1.3 N for 4 blades thruster and 3 blades thruster, respectively.The larger computed drag force values are due to the maximum contact area of water flowing around the ROV model.The maximum and minimum values of the drag forces for model 2 are 20 N and 1.7 N at water flow velocities of 3.5 m/s and 1 m/s, respectively.Similarly, it was also examined from the computed results that the maximum and minimum values of thrust force for model 2 was 12.5 N and 1.3 N at flow velocities of 3.5 m/s and 1 m/s, respectively.Moreover, a graphical representation of a comparison of drag force and thruster force for three different thruster models is shown in Figure 6.It can be seen from the comparison graph that maximum thrust force was observed for model 3, having four thruster blades.It is due to the maximum force is generated to move the ROV body to move forward.Similarly, drag force was also greater for thruster model 3, having four blades due to the large frontal area of the ROV body and thruster blades.According to the listed tables, it can be observed that the maximum thrust force for model 3 is 13 N, and the minimum thrust force for model 3 is 2.3 N at a flow velocity of 3.5 m/s and 1m/s, respectively.
Similarly, the maximum and minimum values of drag forces were observed 20 N and 2 N at flow velocities of 3.5 m/s and 1m/s, respectively.Moreover, the comparison of drag force and thrust force for different thruster blades was investigated.It is evident from Figure 7 that maximum drag force was observed for ROV structure model 1, having 2 blades of the thruster.The reason behind this higher value of drag force in model 1 is due to the availability of maximum contact area exposed to fluid.The maximum contact area enhances the hydraulic load on the ROV body, which causes to increase in drag force.Similarly, the minimum drag force observed in ROV model 2 which has 2 blades of the thruster.This is due to the minimum contact area exposed to fluid.Similarly, a comparison of thrust force for different thruster models was also investigated at different flow velocities.It was observed that ROV thruster model 3, having 4 blades, has higher thrust force.The reason behind this increment in thrust force is the number of blades installed in ROV body.Larger numbers of blades produce more thrust as compared to a lesser number of blades.Similarly, ROV model 1, having a number of blades 2 produces less thrust force to enhance the forward and backward motion of the thruster.At various flow velocities, Table 4 displays the pressure distribution for a ROV body with 4 blades thruster.According to the results, the most pressure is generated on the frontal area of the thruster models' blades.The largest pressure is generated at flow rates of 3.5 m/s, and the lowest pressure is generated at flow rates of 1 m/s.Furthermore, the thruster's performance is within acceptable limitations and capable of achieving good results.The greatest static pressure of ROV model with 4 blades thruster was 9724.37 Pa at a flow velocity of 3.5 m/s.Similarly, the minimum static pressure of the model was 3647.997Pa.The velocity distribution for the ROV body with a four-blade thruster model is also shown in Table 3.The velocity distribution shows that when flow velocities increase, so does the average value of flow velocity on the surface of ROV models equipped with four blade thrusters.According to the figures, the maximum average flow velocity on the surface of the ROV model 1 is 3.5 m/s, while the lowest average flow velocity on the surface of the ROV body is 1m/s.It has been studied that the number of the blade affects the amount of thrust directly.If the blade number of rotor blades increases, the more thrust is produced Thus, four blade propeller generate more thrust than three and two blade thruster models.

Conclusions
The performance of the ROV can be affected by a number of variables, including flow velocity, geometrical shape, and propeller design.Thrusters, which are propellers, are typically powered by electricity in autonomous underwater vehicles.As a result, the thrust force is affected simultaneously by the ROV model, propeller shape, and hydrodynamic effects.Different thruster concepts with two, three, and four-blade thrusters have been proposed to address the issues in this study.For underwater vehicles, there are a variety of thruster layouts that can be used, as well as different thruster numbers and placements.The efficiency of the thrusters in the particular vehicle allows for the production of a variety of thrust forces.At various flow velocities, CFD evaluations of the ROV body with various thruster blades were also conducted.For the purpose of CFD simulation, three distinct types of ROVs with two, three, and four-blade thrusters are used.Choosing the most potent thruster model is the main objective of using these three different types of thrusters.The four-blade thruster generates the maximum thrust force when compared to other ROV thruster variations.This larger thrust force is mostly caused by the increased fluid velocity.More blades produced more thrust than fewer blades, and it was also discovered.At flow velocities of 3.5 m/s, the maximum and minimum values of thrust forces of 13 N and 3.5 N were recorded for four-blade and two-blade thrusters, respectively.This increase in thrust force is mostly the result of increased fluid velocity via the thruster blades.The ROV model 4 with a four-blade thruster was ultimately found to be the ideal type for underwater applications.The present proposed CFD simulations help us to compute the drag and thrust force for optimizing the ROV thruster attached to the ROV body.

2. 1 .
Physical modelTo simulate fluid flow according to a particular condition, a physical 3D CAD model of the fluid domain must be created as the initial stage in CFD modeling[12].The physical 3D model is created in Solidworks, and then the Solidworks file is imported into CFD fluid fluent.The computation domain is generated in the design modeler of ANSYS fluent, and the ROV model lies inside the computation domain.The ROV models with different blade thrusters are shown in Figure2.The computation domain is completely constructed by deducting the ROV model from the fluid domain as shown in Figure3.

Figure 2 .
Figure 2. 3D-CAD models of ROV models: (a) ROV Model with two blade thruster (b) ROV Model with three blade thruster (c) ROV Model with four blade thruster.

Figure 3
Figure3represents the Two-Dimensional model of ROV body.The front and side views of ROV models are shown in Figure3.The units were used for modeling all ROV models millimeters.In this proposed structure model, two thrusters are installed on the both side of the model.In addition, the camera system and other control systems are inserted inside the ROV structure model.The curve surface of the ROV structure model helps to decrease the drag force and increase the velocity of the ROV body.Two thrusters are mounted on the both sides of the model.The diameter of the thruster blades is 240 mm.This ROV structure model total length of the ROV body is 454 mm and width is 200 mm.In addition, total vertical height of the ROV body is 105 mm.

Figure 5 .
Figure 5. (a) Mesh of three-dimensional flow domain (b) Mesh of flow domain and cut section.

Figure 6 .
Figure 6.(a) Variation of drag force with different flow velocities (b) Variation of thrust force with different flow velocities.

Figure 7 .
Figure 7.Comparison of drag and thrust force (a) Variation of thrust force with different flow velocities (b) Variation of drag force with different flow velocities.

Table 4 .
Pressure distribution and velocity distribution with 4 blades at different flow velocities.

Sizing and Selection of ROV Models Is Assembly Proper? lmport geometry in ANSYS and generate mesh ls Mesh Quality Acceptable? Input Boundary conditionand initial condition in CFDsimulation software Flow simulation usingANSYS fluid fluent ls Mesh Quality Acceptable? Results Creation of 3D model of ROV Yes No No Yes Yes No Figure 1. Methodology
flow chart of CFD analysis of ROV design.

Table 1 .
Description of mesh study in computational domain.

Table 2 .
Drag force at different velocities.

Table 3 .
Thrust force at different velocities.