Introduction

Groynes are hydraulic structures that protrude from river banks to prevent erosion by redirecting flow velocity1. They also improve navigability by deepening the main channel by constricting the width of the river flow, which increases the depth and velocity of the flow2,3,4,5,6. Globally, constructing these control structures on rivers can alter the hydrodynamics of the flow downstream, thereby reducing scouring and pollution transport1, 7, 8. The effectiveness of groynes in erosion protection depends on various design parameters, such as their shape, projection, permeability degree, submergence ratio, spacing, the number used, and orientation9, 10 These design parameters control and direct the discharge to safeguard river banks and protect the structure from damage11, 12. When a vortex forms in a river with an even riverbed, it causes the rotational zone to grow larger13,14. The flow lines are directed towards the center of the Groyne and become more assertive near the riverbed as they flow downstream15,16.

The shapes of groynes can vary, with options like straight, L-head, T-head, and hockey-shaped groynes based on various river conditions17,18,19. Additionally, curved groyne are available in elliptic, semi-parabolic, and quadrant shapes, adding further versatility to erosion protection design and allowing designers to tailor the protection measures based on the specific requirements of the river environment20. The restriction of the surface flow generated by groynes leads to increased velocity and discharge21. The unidirectional flow field in the river transfers into a three-dimensional flow after meeting with a barrier like a groyne, which develops and separates the vortex flow2,3,22,23,24. The static pressure gradient leads to acceleration drawdown flow tawdries upstream of the groyne25,26. The combination of downward flow near the boundary layer of the river and generated bow wave results in a periodic vortex system at the groyne’s base and substantial bed shear stresses27,28. turbulent flow fluctuations around groyne include the development of a shear layer characterized by high scouring, and it starts within the base, near the upstream of the groyne, and is deposited to the channel downstream29, 30. The previous numerical and experimental studies have concentrated on estimating the morphology of max and min scour depth, mean flow, and turbulence around straight, L-head, and T-unsubmerged groynes19,30,31,32,33. Limited research exists on investigating the behavior and hydrodynamics of turbulent fields around curved hockey groynes under fixed-bed conditions. The hockey groynes diaphragm is used because it can more efficiently improve hydraulic flow control and reduce discharge than conventional diaphragms34. This curved groynes type has a unique design that allows for improved pressure distribution and reduced energy loss, making it a practical choice in various hydraulic applications35. In addition, modifying the geometric properties, such as the hockey shape and degree of rotation, allows for improved performance in controlling water flow, making it an important tool for reducing the risk of corrosion and enhancing the efficiency of hydraulic structures.

The study was simulated using ANSYS Fluent to software, which provides advanced numerical modelling options such as turbulence models (k-ε, k-ω SST) and adaptive mesh techniques, ensuring more accurate results than traditional experimental methods.

The research gap is summarized in modelling the hockey groynes' using computational fluid dynamics with ANSYS Fluent software and comparing it in terms of preference with other conventional types to determine the efficiency of this model compared to previously used methods. In addition, the study addresses the hydrodynamic behaviour in open channels of this model impact on velocity distribution, bed shear stress, and flow turbulence when changing some geometric properties, such as the Hockey shape and the degree of rotation, which contributes to understanding the effect of these modifications on the hydraulic performance and improving its future designs. The study's limitation is that it focuses on the hydrodynamic performance of the barrier without analyzing the impact of environmental factors such as sediments and vegetation cover. It also does not address the impact of temporal changes such as erosion and flooding.

Materials and methods

Study area

The breakwater system of the Al-Faw Grand Port Project is one of the longest in the world, stretching over 15 km. Located in Basra, Iraq, it spans between longitudes 46° and 48°E and latitudes 30° to 32°N, as map illustrated in (Fig. 1) by Arc GIS 10.5. This system plays a vital role in enhancing the country's trade capabilities. Strategically positioned at the confluence of the Shatt al-Arab and the Arabian Gulf, the port provides efficient shipping routes. It features a robust breakwater system known as Groynes, which is essential for protecting vessels from harsh sea conditions while ensuring safe docking and loading operations. The breakwater reduces wave action, which in turn minimizes erosion and sedimentation in the harbor area. The hydraulic engineering work involved in the breakwater system for the Al-Faw Grand Port Project includes extensive measures to manage and mitigate the effects of wave action, tidal currents, and sediment transport along Iraq's Arabian coastline. Designed to protect the port's infrastructure, this hydraulic work ensures safe berthing, loading, and unloading operations within the port area, which is subject to high-energy wave conditions due to its open coastal location. The methodology followed in this research summarized in Fig. 2.

Fig. 1
figure 1

Map of breakwater system (Groynes) of the Al-Faw Grand Port Project generated by Arc GIS 10.5.

Full size image
Fig. 2
figure 2

Flowchart of methodology adapted in this study.

Full size image

Description of the investigated model

The study examined a curved groyne of a single hockey shape, with dimensions of 1 cm thickness and 10 cm height, as depicted in Fig. 3. The design parameters that are included are the orientation, ϴ, submergence of groynes, Sg. Three orientations of 60, 90, and 120° and three submergence ratios of 75, 100, and 125% were applied. The flow simulation took place in a laboratory channel with dimensions of 4 m length, 0.4 m width, and 0.175 m height (Fig. 4).

Fig. 3
figure 3

Hockey groynes with various orientations angels.

Full size image
Fig. 4
figure 4

Geometry of the flume used and the position of the groyne.

Full size image

The groyne orientations (60°, 90°, 120°) and immersion ratios (75, 100 and 125%) were chosen based on conventional engineering assumptions and preliminary experiments that indicate that these values ​​balance hydraulic performance and structural stability36. The 90° orientation is often optimal because waves strike perpendicular to the breakwater, minimizing their impact onthe structure. The 60° and 120° orientations were chosen to study the effect of oblique orientation on the force distribution and wave action. For the immersion ratios, 75 and 100% were chosen to ensure maximum breakwater stability and evaluate depth's effect on performance.

CFD model description

Computational fluid dynamics, CFD is the software to simulate and analyses systems of fluid flow, and other associated phenomena. A commercial software package, ANSYS Fluent, is a part of the CFD that is used in this study to simulate flow around groynes12.

Mesh independence generation and tests

The numerical mesh was generated using ANSYS Workbench with tetrahedral mesh cutting to ensure the accuracy of the geometric representation. The process included model preparation, importing it into setting Meshing and adjusting quality parameters such as high smoothing and improving the distribution of elements around important hydraulic regions. The mesh quality was evaluated via Fluent, with an average maximum deviation of 0.79 and a minimum orthogonality of 0.24, with approximately 800,000 mesh elements. (Fig. 5) illustrates the numerical modelling and mesh preparation.

Fig. 5
figure 5

Geometry meshing process using the meshing tool in ANSYS Fluent.

Full size image

Runs design models

The numerical water flow simulation around the hockey groynes barrier was performed using ANSYS Fluent, where the mesh was imported, and its quality was checked. The Navier–Stokes equations were adopted with an appropriate turbulence model (k-ε or k-ω SST), and boundary conditions were determined to ensure the stability of the numerical solution. After running the simulation, the velocity and pressure distribution were analyzed, the results were compared with experimental data, and the influence of geometric parameters on the flow was studied.

Sensitivity analysis hydrodynamic flow

The main flow models selected are the multiphase and turbulence models for open channel flow. The multiphase flow model utilizes the Volume of Fluid (VOF) method to handle the interactions between air and water in the available channel.

Generally, k-ε and k-ω are considered two turbulence models that are commonly used for flow simulation around hydraulic structures but there are other models. Recently, the power of the SST, k-ω, model has been proved for simulation of the open channel flow around groynes by using ANSYS Fluent. Therefore, the (SST-k-ω) model was employed for the turbulence modelling, The Shear stress transport, SST, model is a combination of a k-ω model that is used close to walls, and a k-ε model, that is used in zones far from walls. This model is useful and usually works well close to solid boundaries.

The multiphase flow includes air and water as the primary and secondary phases, respectively. These two phases are characterized by a constant surface tension of 0.072 N/m between them, allowing the simulation to accurately capture the interactions and dynamics of the air–water interface. Boundary conditions was set to a discharge, Q, at the inflow side, and a uniform water depth, y, at the outflow side. Moreover, hydraulic parameters such as bottom level and free surface level, hydraulic diameter, and turbulence intensity, were specified for inflow and outflow boundaries. The sidewalls and the bottom of flume boundaries are considered a wall without slip, excluding the bed is set a roughness height of, d50 = 0.7 mm.

The roughness height (d50 = 0.7 mm) was chosen to match the typical properties of bed sediments in natural and hydraulic channels, where it directly affects the boundary layer thickness, flow resistance, and friction coefficient. Previous studies support this choice, showing that a d50 value in this range provides a realistic representation of bed roughness in similar flows, ensuring the accuracy of the numerical simulation and limiting unrealistic effects on the velocity and pressure distribution38,39.

The pressure–velocity coupling utilized a scheme-segregated algorithm in the CFD modelling. A second-order upwind scheme was also applied to handle turbulent kinetic energy (TKE), momentum, and dissipation rate calculations. This approach ensures accurate and stable simulations for fluid flow and turbulence phenomena.

Table 1 presents the hydraulic data obtained from the CFD model runs. Initially, the simulations were performed to represent the flow in an open channel under three different discharge conditions without using hockey groynes (control conditions). Subsequently, additional runs were conducted to simulate the flow around a single hockey groyne with three different orientation angles to analyze their effects on the flow patterns. In this research, the sensitivity analysis test is performed by changing the basic parameters (such as the rotation angle, the immersion ratio, and the flow conditions) and observing their effect on the numerical results, such as the velocity and pressure distribution.

Table 1 The hydraulic information for the CFD Runs.
Full size table

The sedimentation process is started when the maximum shear stress ofthe channel bed reaches the critical shear stress. The critical shear stress calculated to erosion zone according to the mean diameter, d50, that is found equal to be 0.37Pa37.

Governing equations

The governing equations of fluid flow serve as mathematical representations of the fundamental conservation laws of physics. These equations encompass vital principles such as the conservation of mass, expressed through the continuity equation, and the conservation of momentum. The letter states that the momentum change ratefor a fluid particle is equivalent to the sum of the forces acting upon it40. A fluid particle represents the tiniest conceivable unit of fluid. Fluid behavior is described in terms of properties, including pressure, velocity, temperature, and density along with their spatial and temporal derivatives. The governing equations used in Computational Fluid Dynamics (CFD) modelling for transient simulation of three-dimensional, incompressible fluid flow consist of the continuity equation and Navier–Stokes (N.S) equations. The Finite Volume Method (FVM) is employed, providing a practical numerical approach for simulating fluid flow phenomena and capturing the behaviour of fluid particles in a time-dependent manner. The conservation law is applied to discrete control volumes created through meshing. By taking into account the initial and boundary conditions, the balance equations are subsequently solved. Finally, the equations (Eqs. 1 and 2) for the mass conservation, and the conservation of momentum, respectively, can be written as follows: ANSYS Fluent Theory Guide.

Continuity equation (conservation of mass):

$$\frac{\partial \rho }{\partial t}+\nabla .\left(\rho \overrightarrow{v}\right)=0$$
(1)

To ensure that no mass is lost or gained within the studied area.

Navier–Stokes equations (conservation of momentum):

$$\frac{\partial }{\partial t}\left(\rho \overrightarrow{v}\right)+\nabla .\left(\rho \overrightarrow{v}\overrightarrow{v}\right)=-\nabla p+\nabla .\left(\overline{\overline{\tau }}\right)+\rho \overrightarrow{g}+\overrightarrow{F}$$
(2)

Which represents the balance of forces acting on the fluid, including pressure and viscosity.

where: T: Time, s. \({\varvec{\rho}}\): Density, kg/m3; \(\overrightarrow{{{v}}}\): Overall velocity vector, m/s; P: Static pressure, Pa; \(\overline{\overline{{{\tau}}}}:\) Stress tensor, Pa. \(\overrightarrow{{{g}}}:\) Gravitational acceleration, m/s2; \(\overrightarrow{{{F}}}:\) External body forces vector, N.

The two variables calculated are usually clarified, k, is the turbulent kinetic energy, and, ω, is the dissipation rate of the vortex.

Turbulence models (k-ε or k-ω SST)

The model of SST k-ω can be defined by the following equations (Eqs. 3–10), ANSYS Fluent Theory.

$${\mu }_{t }=\frac{\rho k}{\omega }\frac{1}{max\left[\frac{1}{{\alpha }^{*}} , \frac{S {F}_{2} }{{a}_{1 }\omega }\right]}$$
(3)

To characterize the effects of turbulence on the flow, additional equations are solved for the turbulence energy and its dissipation rate.

where: S: is the strain rate magnitude, a1: 0.31, and α*: is defined as follows:

$${\alpha }^{*}= {\alpha }_{\infty }^{*} \left(\frac{{\alpha }_{0 }^{*}+{Re}_{t }/{R}_{k} }{1+{Re}_{t }/{R}_{k}}\right)$$
(4)
$${Re}_{t }=\frac{\rho k}{\mu \omega }$$
(5)
$${R}_{k}=6$$
(6)
$${\alpha }_{0 }^{*}=\frac{{\beta }_{i}}{3}$$
(7)
$${\beta }_{i}=0.072$$
(8)

where:

Note that in the High-Reynolds number form of the k-ω model,\({\alpha }^{*}= {\alpha }_{\infty }^{*}=1\).

And \({F}_{2}\) is given by following equations (Eqs. 9 and 10):

$${F}_{2}=\text{tanh}\left({\varnothing }_{2}^{2}\right)$$
(9)
$${\varnothing }_{2}=max\left[2\frac{\sqrt{k}}{0.09\omega y}, \frac{500\mu }{\rho {y}^{2}\omega }\right]$$
(10)

where: y : is the distance to the next surface.

In this study, the SST k-ω turbulence model was chosen and not compared to other models based on its suitability for complex turbulent flows near surfaces. It is a commonly used model in hydraulic studies due to its accuracy in predicting turbulence at bed and boundaries.

Extreme flow scenarios were not used in this study because the focus was on standard flow conditions reflecting the most common conditions encountered by the barrier. In addition, focusing on normal conditions contributes to obtaining accurate and reliable results for barrier design under typical flow conditions.

Results, analysis and discussion

CFD model validation

A comparison was performed for model validation between the CFD model and experimental results obtained under comparable conditions. Published experiment data on the elliptic groynes conducted by41 was used to validate the use of the CFD Software. The considered parameters for the single groyne are and length (Lg = 20 cm) and width (Wg = 13 cm). The groyne has a thickness of 1 cm and a height of 10 cm. The experimental setup used a flume with dimensions of 4m in length, 0.4 m in width, and 0.4 m in height, with a zero slope.

Figures 6 and 7 shows the obtained contours of the variation of the bed shear stress by using the model and experiment photo under different conditions and by using single and double elliptic groynes of different projections. The CFD model results are presented using contours to represent the variation in bed shear stress visually. These contours are then compared with the observed sedimentation distribution during41 experiment. In the experiments, a movable bed was used, and visual observations were made to identify the patterns of scouring and deposition around the groynes. Generally, in the single elliptic groyne, the results showed an increase in bed shear stress when the width of the groynes is increased. The scour volume increase with an increase of bed shear stress for the flow simulations around the single elliptic groyne. Moreover, the maximum bed shear stress increased with the increase of groyne width at just the upstream side of the single elliptic groyne. In runs with double groynes, the shear stress decrease when increasing the spacing between groynes. The maximum bed shear stress formed at upstream of the first groyne i.e. scour zone, while the minimum bed shear stress located at downstream of each groyne i.e. deposition zone. Notably, the experimental and simulated results obtained under the same conditions show good agreement regarding the locations of scouring and deposition. This agreement validates the CFD model's capability to accurately represent the flow patterns and sediment transport dynamics around the single elliptic groyne. The slight discrepancy between the numerical and experimental results can be attributed to the CFD model's assumption of a channel bed. The study assumes a fixed bed to simplify the simulation and reduce numerical complexity, allowing the hydraulic performance of the barrier to be investigated independently of sediment transport effects. However, in a real environment, erosion and deposition lead to morphological changes that may affect the flowand behaviour of the barrier.

Fig. 6
figure 6

Contours variation of bed shear stress and experiments photo for three projections of the single elliptic groyne, y = 2.9 cm, and Q = 0.0024 m3/sec.

Full size image
Fig. 7
figure 7

Contours variation of bed shear stress and experiments photo for double elliptic groyne, Wg = 13 cm, Lg = 20  cm, y = 2.9  cm, and Q = 0.0024 m3/sec.

Full size image

Additionally, the photographs taken during the experiment were not perfectly perpendicular to the flow, leading to a slight mismatch in image interpretation. Moreover, a movable bed can be improved by simulating the effect of erosion and sedimentation on water flow over time and analyzing the impact of these changes on barrier stability and efficiency. Sediment dynamic models can also be incorporated to study flow interactions with changing beds in multiple river environments.

The laboratory experimental results show only the depth and volume of sediments. It is interesting to present detailed results under the same conditions as CFD Software experiments. Table 2 presents the minimum and maximum velocity values and bed shear stress obtained during the validation model runs. The velocity and bed shear stress values show the best projection of the three models of the elliptic groyne and the best spacing between the double elliptic groyne. The negative sign of the minimum velocity and bed shear stress means its direction is opposite to the flow direction. The ratio ranges of the maximum velocity and bed shear stress varied by 62 to 86% and 51 to 162%, respectively, for three cases of the single groyne. At upstream of nearly the first groyne, the maximum velocity values of the water surface increased in cases of different spacing 1 Wg, 1.5 Wg, 2 Wg, and 2.5 Wg about 138, 71, 71. and 67%, respectively. At the same time, the ranges values of maximum bed shear stress increased by 124 to 322% with decreased spacing between groynes. Finally, the validation runs and their comparison with experimental results showed that the best projected single groynes are to 7 cm, and the best spacing between groynes is 2 Wg.

Table 2 The values of min and max velocity and bed shear stress for runs of the validation model.
Full size table

Analysis of flow under control conditions

The flume flow in the control case is simulated without hockey groynes with a different flow. Three uniform water depths were defined as 7.5, 10, and 12.5 cm, corresponding to discharges of 0.0057, 0.0087, and 0.0119 m3/sec, respectively. From the simulation results, the mean flow velocity at the water surface was equal to 0.195, 0.221, and 0.241 m/sec for the depth of 7.5, 10, and 12.5 cm, respectively. Figure 8. presents the locations of selected cross-sections and the single hockey groyne located in the flume. Moreover, this is required to draw profiles of the velocity variations with channel width and a flow inlet and outlet. Figure 9, illustrates the relationships of velocity profile variations with channel width at a mid-height position of the hockey groyne under control case conditions. The average velocity at mid-height obtained is 0.213, 0.236, and 0.256 m/sec for three water depths, respectively. Finally, the results of velocity variations are an index to know the impact of the single hockey groynes on the flow.

Fig. 8
figure 8

Locations of selected cross-sections, and the single hockey groyne located in the flume.

Full size image
Fig. 9
figure 9

Velocity profiles with different channel width.

Full size image

Alternative schemes such as PISO or Coupled are not adopted because the case studied is based on a fixed bed and does not involve time variations or unsteady flow conditions. In this case, the SIMPLE scheme is sufficient to achieve stability of the solution and convergence of the results without the need for advanced techniques dedicated to unsteady or time-varying flows.

Analysis of the single hockey groyne

The velocity variations

Figures 10 and 11 display contours illustrating velocity variations and the variation of velocity along the streamlines around a single non-submerged hockey groyne. Generally, the maximum velocity is observed upstream of the hockey groyne, while the minimum velocity is located downstream, near the wall. The velocity variations at the water surface gradually increase at the front edge of the hockey groyne and then gradually decrease along the side of the groyne. Furthermore, the maximum velocity slightly increases with an increase in the orientation angles of the hockey groyne. The streamlines at the water surface reveal the presence of vortices near the downstream section of the hockey groyne. The size of the vortex area increases with higher orientation angles of the groyne, and the vortex center moves away downstream from the hockey groyne. These observations provide valuable insights into the flow patterns and behaviour around the hockey groyne under non-submerged conditions.

Fig. 10
figure 10

Contours of the variation of the velocity at the water surface around the single hockey groyne with different three orientations, y = 7.5 cm, and Q = 0.0057 m3/sec. (a) 60° ; (b) 90° ; (c) 120°.

Full size image
Fig. 11
figure 11

Displays the variation of velocity along the streamlines around a single hockey groyne with three different orientations, and the simulation was conducted using parameters y = 7.5 cm (distance from the bed) and Q = 0.0057 m3/sec (flow rate). (a) 60°; (b) 90° ; (c) 120°.

Full size image

Figures 12 and 13 show contours showing variations in velocity and distribution along the streamlines around a single hockey groyne under 100% submergence ratio conditions. Generally, in this case, the behavior of velocities observed around the single hockey groyne is similar to the non-submerged case. However, the difference was formed in the water surfaceclose to the side wall upstream of the single hockey groyne. The water depth increased at part of the top of the first groyne as well as the values of velocities were more amplified from the non-submerged groynes. The behavior of the velocity variations along streamlines is proximate, similar to the previous case. However, there was an increase by in the intensity with increases in the orientation angles of the hockey groyne.

Fig. 12
figure 12

Contours of the velocity variation at the water surface around the single hockey groyne with three different orientations, y = 10 cm, and Q = 0.0087 m3/sec. (a) 60°; (b) 90°; (c) 120°.

Full size image
Fig. 13
figure 13

Displays the variation of velocity along the streamlines around a single hockey groyne for three different orientations, and the simulation was conducted with parameters y = 10 cm (distance from the bed) and Q = 0.0087 m3/sec (flow rate). (a) 60°: (b) 90°; (c) 120°.

Full size image

The formation of vortices around hockey groyne is not comparable to field measurements due to the difficulty of obtaining accurate field data at the studied sites and practical constraints such as limited time and resources. Furthermore, variable environmental conditions can make comparing simulations and field measurements challenging. However, future studies involving field data collection can be conducted to improve the comparison and enhance the accuracy of the modelling.

Figures 14 and 15 present the contours of the velocity variations and the variation of the velocity along the streamlines around a single hockey groyne in the submerged case. Generally, there are some substantial changes for the submerged case of the single hockey groyne compared with the two cases previously. The maximum velocity at the water surface observed at upstream of the hockey groyne close to the wall for the different orientations. Although, the water surface is higher than the top of the hockey groyne. The streamlines at the surface of the water flow showed that the vortex appears around the single hockey groyne for the orientation angle of 120°. These vortex properties have less area, as well as the vortex centre, moved away towards downstream of the groyne compared with the two cases previously. For the orientations of 60° and 90°, the behavior of the streamlines demonstrated the absence of a surface vortex when compared to the previous cases.

Fig. 14
figure 14

Contours of the variation of the velocity at the water surface around the single hockey groyne with different three orientations, y = 12.5 cm, and Q = 0.0119 m3/sec. (a) 60°; (b) 90°; (c) 120°.

Full size image
Fig. 15
figure 15

Depicts the variation of the velocity along the streamlines of water surface around a single hockey groyne with three different orientations, y = 12.5 cm (distance from the bed) and Q = 0.0119 m3/sec (flow rate). (a) 60°; (b) 90°; (c) 120°.

Full size image

Figure 16a–i shows the relationships of profiles of velocity variations with channel width at a mid-height of the hockey groyne for the submergence of 75, 100, and 125%, and the orientation angles of 60, 90, and120°. The velocity profiles were needed to clarify the ratio of increasing the velocity at the front side of the single hockey groynes. Moreover, the decreased velocity in selected cross-sections at the single hockey groyne side for each case. The ratio of increasevelocity ranges between 5–13%, 25–41%, and 36–48% for the orientation angles of 60, 90, and 120°, respectively, with different submergence ratios. The ratio of maximum velocity was increased at the front edge of single hockey groyne with an increase in the orientation angles for different submergence ratios. The reference measuring of the distance of reduced velocity is located in the single hockey groyne. The single hockey groyne is located at a distance of 1m from the flow inlet. In the non-submerged single hockey groyne, the distance of reduced velocity was equal to 0.25, 1, and 1.25 m for the orientations angle of single hockey groyne of 60, 90, and 120°, respectively, from the reference measurement. While, for the submergence of 100%, the distance of reduced velocity was equal to 0.25, 1, and 1.25 m from the reference measurement for the orientations angle of 60, 90, and 120°, respectively. In the submerged case, the distance of reduced velocity from the reference measurement was 0m, 0.5m, and 0.5m for orientation angles of 60, 90, and 120°, respectively.

Fig. 16
figure 16

Velocity profiles with channel width for, (a): ϴ = 60°, and Sg = 75% ; (b): ϴ = 60°, and Sg = 100% ; (c): ϴ = 60°, and Sg = 125%; (d): ϴ = 90°, and Sg = 75%; (e): ϴ = 90°, and Sg = 100%; (f): ϴ = 90°, and Sg = 125%; (g): ϴ = 120°, and Sg = 75%; (h): ϴ = 120°, and Sg = 100%; (i): ϴ = 120°, and Sg = 125% .

Full size image

The bed shear stress variations

Figure 17 presents the contours depicting the shear stress variation around single hockey groynes in the non-submerged scenario, considering three different orientation angles. The maximum shear stress formed upstream of the single hockey groyne. While the minimum shear stress observed downstream of the groyne close to the side wall. Moreover, it formed at upstream of the groyne close to the side wall. The area of maximum shear stress increased with a rise in the orientation angle of hockey groynes.

Fig. 17
figure 17

Displays the bed shear stress variation contours around a single hockey groyne for three different orientations with parameters used in the simulation y = 7.5 cm (distance from the bed) and Q = 0.0057 m3/sec (flow rate). (a) 60°; (b) 90°; (c) 120°.

Full size image

Figure 18 the contours illustrate the variation of shear stress at the bed canal around single hockey groynes for a 100% submergence ratio, considering three different orientation angles. Ultimately, as in the non-submerged single hockey groyne observed, the minimum and maximum bed shear stress locations are similar. However, there is a slight increase in the areas and values of the bed shear stress variations around the single hockey groyne, unlike the values of the non-submerged case. Finally, the bed shear stress value has more impact on the orientation angle of 120° from other orientations.

Fig. 18
figure 18

Exhibits the contours depicting the variation of bed shear stress around a single hockey groyne for three different orientations and the simulation was conducted with parameters y = 10 cm (distance from the bed) and Q = 0.0087 m3/sec (flow rate). (a) 60°; (b) 90°; (c) 120°.

Full size image

Figure 19 displays the contours of bed shear stress variation around single hockey groynes in the submerged case, with three different orientation angles. Generally, the values of bed shear stress a slight amplified at the locations of the minimum and maximum bed shear stress, unlike the two cases previously but the behavior is almost similar. The location of the minimum shear stress changed to downstream of the hockey groyne close to the wall for two the orientations angles of 60° and 90°. Moreover, the areas of minimum and maximum bed shear stress were increased in this case, but it is increased with increases the orientation angles.

Fig. 19
figure 19

Contours of bed shear stress variation around single hockey groyne at three orientations (y = 12.5 cm, Q = 0.0119 m3/sec). (a) 60°; (b) 90°; (c) 120°.

Full size image

The maximum and minimum velocity values and shear stress for the hockey grooves with different orientation angles are presented in Table 3. At an orientation angle of 60 degrees, the maximum velocity ratio of control cases slightly decreased with varying submergence ratios, ranging from 61 to 66%. However, the maximum bed shear stress ratio to critical shear stress increased with different submergence ratios, ranging from 59 to 124%. For an orientation angle of 90 degrees, the maximum velocity ratio of control cases remained constant at 61, 71, and 63% with increasing submergence ratios, respectively. The maximum bed shear stress ratio to critical shear stress increased with different submergence ratios, ranging from 24 to 94%. At an orientation angle of 120 degrees, the maximum velocity ratio of control cases was equal to 78, 60, and 63% with increasing submergence ratios, respectively. The maximum bed shear stress ratio increased with different submergence ratios, ranging between 52 and 120%.

Table 3 Minimum and maximum velocity, and shear stress values at bed flume for hockey groynes at various orientation angles.
Full size table

After the results of the comparison of two types of groynes , the elliptic in previous research12 and the hockey types, the hydraulic conditions are the joint parameters between the two types of groynes as well as the groynes numbers that included the single groyne and series of groynes, N = 4, with the spacing between groynes equal to 2Wg. Moreover, these hydraulic conditions are presented by three submergence ratios of groynes equal to 75, 100, and 125%. General, for two shapes of groynes, the numbers have depended on the length of the river-the bank to be protected that may be straight, curvature, and meandering length of a river. The bed shear stress ratio has increased with an increase of the submergence ratio for the single and series groyne, and the submergence ratio is preferably used between 75 and 100%. Moreover, overall, the orientation angle 90o has the most negligible impact on the values and the variations of the velocity and the bed shear stress.

Conclusions

This work has successfully used Computational Fluid Dynamics (CFD) to show how well submerged hockey groynes function in adjusting hydrodynamic conditions inside open channels. The results of numerical simulations under different orientation angles and submergence ratios showed that hockey groynes had a major impact on mean velocity profiles, bed shear stresses, and flow patterns.

Important results show that the ideal submergence ratio is between 75 and 100%, which minimizes scour depth and allows for the best flow characteristics. A 90-degree arrangement was shown to be the most successful in increasing flow velocity and decreasing bed shear stress among the studied orientations, which is in line with real-world river management applications. The choice of 90° as the ideal orientation angle depends on specific conditions but may vary in different river environments due to hydrological and geomorphological factors such as flow velocity, bed slope, and sediment transport. These changes can affect flow stability and barrier efficiency.

The CFD model's accuracy in predicting sediment transport dynamics is demonstrated by its validation against experimental data, which also demonstrates the simulation approach's resilience. These understandings are essential for groyne design and execution, especially in schemes for riverbank stability and erosion control.

Future research should examine how groyne designs affect sediment transport and ecosystem dynamics over the long term. They should also consider practical factors like fluctuating flow rates and sediment properties. The research can be expanded by comparing the hydrodynamic performance of hockey breakers with conventional breakers in terms of hydraulic energy reduction efficiency and their effect on water flow and sediment transport. Hockey breakers are easy to implement and have a modular design, making them an economical and flexible option compared to conventional structures that may require higher construction and maintenance costs. The accuracy of the model could be improved by additional simulations using a moving bed, allowing the sediment dynamics and their effects on flow to be more realistically represented.