Three-Dimensional Numerical Simulation of Flow Through an Inclined Bar Rack with Surface Bypasses: Influence of Inlet Velocity Conditions and Comparison with Field Measurements

Abstract

To mitigate the impact of hydroelectric power plants on downstream fish migration, fish-friendly intakes, combining a low bar spacing rack and several bypasses, are implemented. There are still sites that can be improved thanks to a better bypass design. For this purpose, Computational Fluid Dynamics (CFD) can be a useful tool, even if such devices are still uncommon. This paper investigates the use of a 3D model based on the Reynolds-Averaged Navier–Stokes (RANS) equation for a single phase to simulate the flow in a real-scale water intake equipped with an inclined bar rack and three surface bypasses. The results of numerical simulations are compared to in situ measurements of flow velocities at four cross-sections along the rack, gauging the discharge flowing into the bypasses. The simulated velocities are in accordance with the velocities measured in situ, with a mean square error for the longitudinal velocity ($v_x$) of 0.034 (m²/s²) for the initial simulation and 0.021 (m²/s²) for the improved simulation. The split of the total bypass discharge between the three bypass entrances was satisfyingly predicted by the simulation with the true inlet velocity condition, showing the significant influence of upstream flow non-uniformity.

1. Introduction

Hydroelectric power plants (HPPs) are a source of sustainable energy, but can hinder both upstream and downstream migrations of fish. Concerning the downstream migration, fish can suffer mortality and injury if they pass through the turbines (Larinier and Dartiguelongue [1], EPRI [2], and Pracheil et al. [3]). In France, diadromous species (species performing long migrations and spending part of their lives in saltwater and in freshwater), such as European eels, sea trout and Atlantic salmon, are particularly concerned.

One of the solutions developed to reduce the passage of fish through turbines consists of fish-friendly intakes combining a low bar spacing rack and one or several bypasses depending on the intake size (Courret and Larinier [4] and Courret et al. [5]). These racks should be designed with a narrow bar spacing to physically block fish and prevent their entry into turbines. They are also inclined from the ground or angled from the bank in order to guide fish towards bypass channels located at the downstream end of the bar rack. The design of such devices has been the subject of extensive research and has been implemented at more than 200 sites in France to date. Their efficiency has been assessed at eight sites for salmon smolts (Tomanova et al. [6] and Tomanova et al. [7]) and at five sites for silver eels (Tissot et al. [8]), with turbine discharge globally between 4 to 50 m³/s, and showing satisfactory results. However, the efficiencies observed for fish like smolts that are not physically blocked by the recommended bar spacing (20–25 mm) range from 80% to 100%. So, there are still some sites where it would be interesting to further improve the efficiencies, notably thanks to a better bypass design.

In the case of an inclined rack, among the criteria established for the hydraulic conditions, a normal velocity $V_n$ lower than 0.5 m/s and a tangential-to-normal velocity ratio $V_t/V_n$ higher than 2 must be ensured immediately upstream of the rack to, respectively, avoid fish impingement and guide them towards the surface bypasses. In addition, the flow velocity at the bypass entrances should not show sudden acceleration or deceleration, so as not to generate fish reluctance to enter (Courret and Larinier [4] and Courret et al. [5]).

To be able to predict the flow field in the rack vicinity and at bypass entrances and verify the compliance of the criteria, it can be useful to implement validated numerical simulations, especially in the case of complex and heterogeneous approach conditions. The simulation of flow through bar racks presents significant challenges, particularly due to the need for fine mesh refinement between bars with narrow spacings, which contrasts with the typically larger computational domains. To address computational cost and time, two-dimensional (2D) Computational Fluid Dynamics (CFD) approaches based on Reynolds-Averaged Navier–Stokes (RANS) equations have been proposed for inclined and oriented bar racks (Lucin et al. [9] and Leuch et al. [10]). While effective in reducing computational times, two-dimensional simulations remain limited when applied to configurations involving inclined bar racks with surface bypass systems, where the flow becomes inherently three-dimensional. Three-dimensional (3D) simulations, particularly those incorporating multiphase modelling with Volume of Fluid (VOF) methods, have been used to better represent free surface flows (Feigenwinter et al. [11], Latif et al. [12] and Bon et al. [13]). However, these methods are computationally intensive. As an intermediate solution, 3D monophasic RANS simulations, considering only the water phase, may be developed. These allow for the representation of complex 3D flow patterns while keeping mesh size and computational time within feasible limits (Hribernik et al. [14] and Carija et al. [15]). Despite these developments, a comprehensive 3D numerical study covering the full system of inclined bar racks with surface bypasses is still lacking. Such a study is essential to improve our understanding of the hydraulic behaviour of these systems and to optimize their design for enhanced performance and ecological compatibility.

This paper deals with a numerical simulation of the real-scale water intake of Las Rives equipped with a bar rack inclined at β = 26° and three surface bypasses, using the 3D Computational Fluid Dynamics suite OpenFOAM. The results of the numerical simulations are compared to in situ measurements of flow velocities at several cross-sections along the rack, gauging the discharge flowing into each of the three bypasses (Lemkecher et al. [16]).

In the next sections, the studied site is first presented. Then, the numerical parameters of the model are detailed. The fourth part shows the results of the initial and improved numerical simulations.

2. Study Site

The Las Rives HPP is located on the Ariège river in the southwest of France (43°2′12.55″ N, 1°36′57.06″ E). The hydrological regime of the Ariège river is pluvio–nival and its mean inter-annual discharge is 41.8 m³/s ($Q_m$). The Las Rives HPP is a diversion weir scheme that bypasses a 550 m long reach of the river. The main plant is composed of three historical Francis turbines and a dive turbine added in 2015. Its maximum turbine discharge is 45 m³/s (108% of $Q_m$). The maximum head is 6.65 m and the gross power is 2544 kW. The minimum discharge to be delivered in the bypassed reach is 4.85 m³/s (11.6% of $Q_m$) and is composed of 0.5 m³/s flowing through the fishpass for upstream migration, 3 m³/s through a dive turbine added in 2017, and 1.35 m³/s through the bypass for downstream migration. Figure 1 allows picturing the scheme of the HPP.

The fish-friendly intake built in 2014 is located at the beginning of the headrace canal, so that the discharge flowing through the bypass is delivered near the foot of the weir and is included in the required flow to sustain ecological conditions in the bypassed reach of the river.

Between the intake gates and the inclined rack, the intake channel width reduces from 16.4 m to 14.0 m with a non-symmetrical convergent (Figure 2). The intake depth is 4.18 m. The mean approach velocity is 0.77 m/s for the maximum turbine discharge (without including the bypass discharge). The device combines a rack with an angle of inclination from the ground of β = 26° and a 20 mm bar spacing, and three surface bypass entrances placed at the top of the rack to collect the fish, each 0.5 m deep and 1 m wide. A unique transversal gallery collects the discharge flowing through the three bypass entrances (Figure 3). The total bypass discharge of 1.35 m³/s (3% of maximum turbine discharge) is controlled by a fixed weir placed at the downstream end of the gallery. The corresponding mean velocity at bypass entrances is 0.9 m/s. The total bypass discharge can vary depending on the upstream water level fluctuations. The width and thus the wetted section of the gallery increase at the junction of the second and third entrance. This is intended to ensure as much as possible a uniform split of the total discharge between the three entrances. The space between bars is fully sealed at the upper section of the rack, from the top to the bottom of the bypass entrances, which reduces the flow velocity between the entrances and generates transverse currents. This is intended to improve the fish guidance transversally towards the bypass entrances. The effective filtering area of the rack is 117.5 m², and the corresponding mean normal velocity is 0.38 m/s for the maximum turbine discharge. The rack under consideration is composed of bars with a hydrodynamic profile. The width of these bars is 8 mm, the spacing between them is 20 mm, and the width of the seven horizontal spacer lines is 12 mm (see Figure 3).

3. Methodology

3.1. Numerical Setup

Numerical simulations were carried out with the open-source Multiphysics library OpenFOAM v2212 (Open Field Operation And Manipulation [17]), which provides meshing utilities, solvers, and post-processing tools for a wide range of mathematics and physics problems. Implemented in C++, the code employs the finite volume method to solve partial differential equations (PDEs) and can be customized to address diverse fluid mechanics applications, including incompressible and compressible flows, multiphase flows, combustion, and heat transfer.

The Navier–Stokes Equations are solved using the SIMPLE algorithm, and the full-scale simulations of the HPP intakes have been conducted using the steady incompressible single-phase simpleFoam solver. Temporal discretization employed a first-order implicit Euler scheme, while spatial gradients were evaluated with a linear Gauss scheme. The turbulence transport equations (k, ω) were discretized using limited linear schemes. Pressure–velocity coupling was achieved with the SIMPLE algorithm, with pressure solved by the GAMG multigrid solver and velocity/turbulence variables by the Smooth Solver with Gauss–Seidel smoothing. Monophasic simulations were considered, as multiphase flow simulations would be too time-consuming for real-scale simulations. In addition, the results of the monophasic simulations remain perfectly coherent compared to the field measurements. Different turbulence models are available with OpenFOAM, each with its own advantages and disadvantages. Turbulence has here been modelled using the steady Reynolds-Averaged Navier–Stokes Equations (RANS) with the k-ω SST hybrid turbulence model, as this is well suited to such simulations, providing accurate results far from walls with the k-ε model and near walls with the switch to the k-ω model. The boundary conditions are summarized in

Table 1. Boundary conditions of the simulation.

	Inlet	Outlet	Bottom	Walls	Atmosphere	Bar Rack	Outlet Bypasses
Velocity	Dirichlet	Neuman homogeneous	No-Slip	No-Slip	Slip	No-Slip	Dirichlet
Pressure	Dirichlet	Neuman homogeneous	Neuman homogeneous	Neuman homogeneous	Neuman homogeneous	Neuman homogeneous	Neuman homogeneous
k	Dirichlet	Neuman homogeneous	Wall function	Wall function	Neuman homogeneous	Wall function	InletOutlet
$\omega$	Dirichlet	Neuman homogeneous	Wall function	Wall function	Neuman homogeneous	Wall function	InletOutlet

. The InletOutlet condition corresponds to a hybrid boundary condition, with a homogeneous Neumann condition for the outgoing flux and a Dirichlet condition for the incoming flux. The inlet turbulent intensity is fixed to 5% in accordance with classical turbulence intensity values in such a channel and some works from the thesis of Raynal S. [18]. It is assumed that the turbulence kinetic energy (k) is imposed as homogeneous at the inlet, since the limited number of field measurements available in the study does not permit a calculation of its real distribution. The inlet flow rate is set as the sum of the turbined discharge and the bypass discharge, amounting to 46.35 m³/s. The bypass flow rate outlet is also imposed as 1.135 m³/s. The y⁺ value near the walls ranges from 1 to 300 (Figure 4), with an average value of around 95, which justifies the use of the hybrid OpenFOAM wall functions for k (KqRWallFunction) and ω (omegaWallFunction), able to switch between low y⁺ values (close to 1) and high y⁺ values (as stated in the source code). (user manual [19]). The value ω is obtained through a combination of the kinetic energy and the formulation outlined in the user manual.

3.2. Meshing

The basic computational domain is 60 m long, 15 m wide, and 4.20 m deep, with the inlet positioned 30 m upstream of the bypass entrances and the outlet 30 m downstream. The bar racks and bypass structures have been modelled using CAD elements (Figure 5) and have then been subtracted from the initial blocks using mesh castellation and local surface adaptation. All simulations have been initiated with channels defined as Cartesian blocks, with base cell size set to 20 × 15 × 7 cm³. Close to the bar, the base cell size set is reduced to an average of 0.5 cm³. Mesh convergence based on velocity along several lines in the domain has been produced. The results of the mesh convergence are presented in Figure 6 for two vertical lines at mid-distance in the channel and 10 m upstream and downstream of the bar rack system (Figure 5). The mesh convergence validates the final mesh size, comprising 2.4 × 10⁶ cells. Pre-processing operations were performed using the OpenFOAM utilities blockMesh and snappyHexMesh (Figure 7). For meshing reasons, the bar rack is modelled more roughly while respecting the similarity conditions with the same bar rack obstruction $o_b=b/\left(e+b\right)$ of around 0.3 (bar width b of 31 mm and bar spacing e of 71 mm). The convergence of the residuals was analyzed, showing a reduction by a factor of 2.4 for the pressure and between 3.5 and 4.3 orders of magnitude for the other variables (from 1.0 to an order of 10⁻⁴). The continuity error remained below 10⁻⁶, demonstrating that mass conservation is well satisfied and confirming the overall convergence of the simulation.

3.3. In Situ Measurements of Flow Field Along the Rack and Bypass Discharge

Lemkecher et al. [16] present a first campaign of in situ measurement of the flow field along the rack and bypass discharge at Las Rives HPP, for a low flow condition with a turbine discharge of 15.2 m³/s. In the present study, numerical simulations are compared to a second campaign of in situ measurement for a high flow condition with a turbine discharge of 45.21 m³/s and a total bypass discharge of 1.135 m³/s (total inflow in the intake of 46.35 m³/s and approach velocity of 0.8 m/s). The methodologies were exactly the same as the ones employed by Lemkecher et al. [16] and are not presented in detail here. The flow field along the rack was characterized at 4 cross-sections located 10 m, 6 m, 4 m, and 2 m upstream of the rack (Figure 8). The discharge flowing in the collection gallery was gauged by exploration of the velocity field using an electromagnetic flowmeter at 2 locations: downstream of the first bypass entrance and downstream of the junction of the second bypass entrance. The total discharge of the 3 bypasses was evaluated at the weir controlling the discharge using a classical formula of a rectangular weir. The discharge flowing in each bypass entrance has been deduced by subtraction between the different measurements.

4. Results

4.1. Results with Homogeneous Inlet Condition

Full-scale single-phase numerical simulations were conducted for the same conditions as the in situ measurements (turbine discharge of 45.21 m³/s and total bypass discharge of 1.135 m³/s).

Figure 9 presents the cartographies of the numerical and the in situ non-dimensional longitudinal velocity $V_x$ (divided by the mean intake velocity $V_o$ = 0.8 m/s). The velocity $V_x$ has practically the same value as the average velocity $V_o$ (between 0.9 and 1.1 Vo) for the first three transects (10 m, 6 to 4 m). The numerical results are more homogeneous than the in situ measurement, given the constant velocity imposed at the inlet to the domain.

At the transect located 2 m upstream from the top of the rack (about 0.15 m upstream of the entrances), the $V_x$ components decrease significantly outside the closed area between bypasses, with values between 0 and 0.5 $V_o$, and remain between 0.5 and 0.8 Vo in front of the bypass entrances. The simulated $V_x$ components are globally in accordance with the velocity measured in situ.

Figure 10 presents the cartographies of the numerical and the in situ non-dimensional normal velocity $V_n$ (divided by the mean intake velocity $V_o$ = 0.8 m/s). For the three transects located 10 m, 6 m, and 4 m upstream from the top of the rack, the normal components $V_n$ are similar and are between 0.3 and 0.6 Vo. At the transect located 2 m upstream from the top of the rack, the $V_n$ components are equal to 0.5 $V_o$ in front of the bypasses and decrease between 0.1 and 0.3 Vo in front of the closed areas. The simulated $V_n$ components are globally in accordance with the velocity measured in situ.

In dimensional values, the $V_n$ components vary between 0.08 and 0.52 m/s and are therefore almost all in compliance with the criteria $V_n$ < 0.5 m/s.

Figure 11 shows the cartographies of the ratio between tangential and normal velocities $V_t/V_n$ for numerical simulation and in situ measurements. This ratio varies globally between 1.7 and 2.5, with average values of the order of 2, in accordance with the expected theoretical value and in situ measurements.

Figure 12 illustrates the velocity distribution along free-surface level streamlines above the inclined rack and within the bypass channel. The attractiveness of each bypass entrance and the homogenizing effect created by the progressive enlargements along the bypass channel are highlighted by the streamline’s curvature. Hydraulic attractiveness at the bypass entrances, located at the upstream boundary of the domain, was found to be equivalent to 77% of the total channel width. When compared to measurements from the field (

Table 2. Comparison between measured and simulated discharges in each bypass entrance.

		Bypass Entrances
		1 (Left Bank)	2 (Central)	3 (Right Bank)
In situ measurement	Cumulated non-dimensional flow rate (-)	0.16	0.59	1.00
	Percentage of flow rate by bypass (%)	16.2	43.0	40.8
Numerical modelling	Cumulated non-dimensional flow rate (-)	0.26	0.58	1.00
	Percentage of flow rate by bypass (%)	25.7	32.4	41.9
	Relative difference (%)	58.6	24.7	2.7

), the numerical results tend to overestimate the discharge through the left bank entrance by 37% and underestimate that through the central entrance by 25%. Nevertheless, the overall distribution of discharges is satisfactorily reproduced, particularly in terms of flow deficit at the left bank entrance. To better approximate field conditions, an additional simulation is presented in the following section.

4.2. Results with Measured Inlet Velocity Condition

In the first simulation, the velocity was imposed homogeneously at the inlet. This leads to homogeneous transects and an imprecise flow distribution at bypass entrances. The domain here is modified to have an inlet condition at 10 m upstream of the bypasses, corresponding to the most upstream section of in situ measurements. The new domain is shown in Figure 13. The inlet velocity condition is directly calculated and imposed from the interpolation of in situ values at this section. The other parameters of the simulation are the same. This second simulation allows us to assess the impact of the non-homogeneity of the inlet velocity on the flow distribution in the bypasses.

Figure 14 presents the cartographies of the numerical and the in situ non-dimensional longitudinal velocity $V_x$ at the four measurement transects. As the velocity on the first and most upstream transect is imposed as an inlet condition from the in situ measurements 10 m upstream of the bypasses, the simulated and experimental values are identical on this boundary. On the three other transects, the simulated $V_x$ distributions better reflect the in situ measurements than in the initial computations using a uniform flow 30 m upstream of the bypass entrances. These results emphasize the need for realistic inlet boundary conditions in situations for which upstream flow non-uniformities cannot be numerically predicted.

Figure 15 presents the cartographies of the numerical and in situ non-dimensional normal velocities $V_n/V_o$. The results obtained on the 3 simulated transects are very similar to the in situ values.

Figure 16 shows the cartographies of the ratio between tangential and normal numerical and in situ velocities $V_t/V_n$. Despite some under-prediction along the two intermediate transects, the two distributions remain very similar. The ratio varies between 1.7 and 2.5, with average values of the order of 2, in accordance with the expected theoretical value and in situ measurements. CFD therefore allows for predicting the flow across the device with reliable estimates of hydraulic fish-friendly criteria, provided that realistic values can be applied as upstream boundary conditions.

The mean square error is calculated in each transect between field measurements and numerical simulations (initial and improved simulations):

$$MSE={\displaystyle \frac{\sum {\left(v_{num}-v_e\right)}^2}{N}}$$

(1)

where $v_{num}$ is the numerical velocity (m/s), $N$ the number of points on the section and $v_e$ the experimental velocity (m/s).

Table 3. Comparison of the mean square error (MSE) of the three velocity components ($v_x$, $v_y$, $v_z$) for the initial and improved simulations. The results for all transects are shown in bold, with the colour code indicating the results of the best simulation in green and those of the least accurate simulation in red.

		Transect at 10 m	Transect at 6 m	Transect at 4 m	Transect at 2 m	All Transects
MSE (m2/s2) (Initial simulation)	$v_x$	0.0313	0.0319	0.0299	0.0422	0.0338
	$v_y$	0.0068	0.0061	0.0121	0.0262	0.0128
	$v_z$	0.0026	0011	0.0044	0.0157	0.0060
MSE (m2/s2) (Improved simulation)	$v_x$	0.0088	0.0069	0.0339	0.0312	0.0202
	$v_y$	0.0008	0.0038	0.0071	0.0133	0.0081
	$v_z$	0.0001	0.0026	0.0021	0.021	0.0019

illustrates the improvement brought by the second simulation. The general improvement in the mean square error for the improved numerical simulation is less noticeable for the transects located at 4 m and 2 m. The underestimation of the in situ velocity at 4 m and 2 m upstream of the bypasses was highlighted by comparison with the flow rate on the bypasses and explains the significant mean square error on these transects. Figure 17 and Figure 18 present the comparison between the two simulations and in situ measurements of the longitudinal velocity on these two transects. Despite the higher longitudinal velocity than for the measured values, the improved simulation better represents the velocity field with similar high and low velocity zones and demonstrates the limitation of focusing exclusively on quantitative MSE without qualitative observations of the flow on the transects, even if there are still differences between both. It is important to note that the residual disparities may be attributed to the monophasic consideration or other simplifications employed in the modelling process of the real complex site.

Regarding the flow rate passing through each bypass, compared to field measurements, the repartition of the flow of the improved simulation is more accurate than in the first simulation (

Table 4. Comparison between measured and simulated discharges in each bypass entrance for the new improved simulation.

		Bypass Entrances
		1 (Left Bank)	2 (Central)	3 (Right Bank)
In situ measurement	Cumulated non-dimensional flow rate (-)	0.16	0.59	1.00
	Percentage of flow rate by bypass (%)	16.2	43.0	40.8
Numerical modelling	Cumulated non-dimensional flow rate (-)	0.15	0.55	1.00
	Percentage of flow rate by bypass (%)	15.0	40.3	44.7
	Relative difference (%)	7.4	6.5	9.6

). These improved numerical results tend to overestimate the flow at the right bank inlet by 8% (relative difference) and underestimate the flow at the central inlet by 6% (relative difference). The flow distribution rates are well reproduced across the left bank entrance in terms of flow deficit. Compared to the figures in Table 2, these values indicate that despite the non-homogeneity of the individual flow rate evidenced by the initial simulation, a significant part of the flow repartition is due to the non-uniformity of the upstream flow. From this point of view, CFD can be seen as a valuable step prior to designing bypassing devices, which can prove sufficiently accurate provided that knowledge of the upstream flow conditions is available.

5. Conclusions

Numerical simulations of the real-scale water intake of Las Rives equipped with a bar rack inclined at β = 26° from the ground and three surface bypasses, using the 3D Computational Fluid Dynamics (CFD) suite OpenFOAM, are presented. The results of the numerical simulations are compared to in situ measurements of flow velocities at several cross-sections along the rack, gauging the discharge flowing into each of the three bypasses.

The simulated velocities are globally in accordance with the velocity measured in situ, and the compliance of the water intake with fish-friendliness hydraulic criteria has been confirmed by both the field measurements and numerical simulations. These results confirm the angular criteria proposed for the fish guidance along inclined racks by Courret and Larinier [4] and studied experimentally by Raynal et al. [20] on a down-scaled model. The split of the total bypass discharge between the three bypass entrances was satisfyingly predicted by the simulation with an improved inlet velocity condition. The significant influence of upstream flow non-uniformity, even slight, on the distribution of the bypassed flows has been highlighted.

This study confirms that 3D CFD can be implemented for the design of fish-friendly intakes at existing or new HPPs, to define an optimized configuration. It can be especially useful in the case of complex and heterogeneous approach conditions.

To further improve the results of the numerical simulations, enhancements could be made to the inlet conditions, particularly regarding turbulence intensity, and to the computational domain to better replicate the real system. Moreover, with increased computational resources, modelling the two-phase flow would allow a more accurate representation of the flow dynamics. Nevertheless, the actual results remain perfectly correct, with a significant improvement thanks to the measurements of the inlet velocity field and their incorporation into the simulation.