Numerical modeling of interaction of turbulent flow with trash screen in open channels

Trash screens are widely employed at the entrance of hydraulic structures, water intakes, and pumping stations to trap flowing debris that could exasperate downstream troubles. The characteristics of the vertical trash screen flow are measured using a Three-Dimensional Acoustic Doppler Velocimetry instrument for different flow conditions. The governing equations of the flow are numerically solved using k–ω SST, k–ϵ STD, k–ϵ RNG, and Reynolds Stress Model (RSM) and Large Eddy Simulations (LES). ANSYS-Fluent is used for these numerical simulations. The free surface of the vertical trash screen flow is computed by the volume of fluid method. The Grid Convergence Index is used to analyze the impact of the chosen grid structure on the numerical results. Experimental measurements of the velocity field and free surface profiles are compared with the numerical results of 3D simulations for validation. This study aims to identify the behavior of flow through screens in more detail through experimental and numerical simulations. The computed flow profiles considering all five cases agree well with the measured profile, whereas streamwise velocity in most portions of the flow, the k-ω SST outperforms the other models, and the RSM turbulence model is the second most effective.


Introduction
Debris blockage is a persistent concern and a danger linked with trash racks; it is regarded as one of the primary elements leading to numerous flow inlet difficulties.The accumulation of debris at a screen can significantly limit flow and generate much higher water levels, resulting in catastrophic floods [1].A blocked screen can significantly increase downstream flow speeds, leading to substantial local erosion, and consequently, raising the risk of structural failure and collapse.The continuous hazards due to screen clogging in hydroelectric plants and turbines caused significant head loss, resulting in reduced operational efficiency or fatal operational failure.Several experimental research on-screen performances under various screen blockage instances have been carried out e.g., [2,3,4,5,6,7], and flow pattern variations caused by screen blockage results in an intensifies screen head losses, leading to a less hydraulically efficient inlet condition.The efficiency of screen blockage typically has a substantial impact on a variety of societal facets, including vital domains like infrastructure, the built environment, and economic activity.Moreover, it is essential to conduct a comprehensive assessment of hydraulic head loss in the design of trash screens [8,9,4] This is crucial due to the potential risks associated with an increasing head loss across the screen.Hence, the structural design of the inlet screen holds paramount importance, as intake conditions can significantly influence both the effectiveness of hydraulic operations and associated financial outlays.
Trash interception by a pumping station's trash rack assures the pump unit's safe functioning.Although the trash rack's head loss is minor when intercepted trash obstructs the flow section, a significantly larger water level differential forms between before and behind the trash rack, It not only raises the pump's operation head but also its shaft power and reduces its flow.Consequently, there is a decline in the energy efficiency and an increase in the cavitation tendencies of the pump.Odinets's experiments [10] demonstrate that the location of the blocked section of a trash rack has negligible impact on head loss, whereas the extent of blockage in the trash rack is a critical factor.Gao Xueping [11] computations and examined the flow velocity patterns at both the inlet and outflow of a pumped storage power plant.Additionally, the numerical study analyzed head losses in scenarios where there was no debris obstructing the trash racks.
Various forms of debris accumulate in front of trash racks, with alligator weed being the prevalent type found in rural pumping stations.Creating an accurate geometric model for numerical simulation of the trash barrier is challenging due to the overlaid of layers of debris that accumulate in front of the trash rack.Based on both experimental observations and numerical simulations, it was observed that once the waterweeds in front of the trash rack attain a certain thickness, only a limited quantity of water can pass through the trash rack.The head loss generated by a collection of waterweeds in front of the trash rack is almost equivalent from the loss caused by a solid object of equivalent size and shape as the waterweed mass.Furthermore, the flow patterns in both scenarios exhibit identical behavior.Hence, when simplifying the geometric model of the trash barrier, the debris accumulation in front of the trash rack is regarded as a watertight entity.He Shuquan, et al [12] employed ANSYS CFX software and the volume of fluid(VOF) approach to carry out a numerical analysis of the flow fields behind a trash rack.The accumulation of waterweeds in front of the rack was represented as a watertight entity with dimensions matching those of the waterweed lump.The results showed that although the waterweeds built up in front of the rack to a particular thickness, very little water was able to flow through the trash.The flow velocity through the bottom, unblocked portion of the rack increased quickly, whereas it dropped in the upper, weed-blocked portion.Additionally, With an increase in the blockage ratio, the turbulence scale also increased.Rodi et al.,[13] classify turbulence models into four categories for addressing and simulating turbulence effects in hydraulic flows: (a) empirical correlations, (b) statistical turbulence models based on Reynolds-averaged Navier-Stokes (RANS), (c) direct numerical simulations (DNS), and (d) large-eddy simulations(LES).The empirical relations are still helpful for making first estimations and addressing simple problems.Turbulence models coupled with RANS equations have evolved into a potent tool for dealing with problems involving complex irregular boundaries and the interaction of many flow regimes with the advent of the computer.Except for applications involving sediment transport [14] the Re-Normalization Group (RNG) k-ε version performs superior than the others the RANS-based turbulence models in the field of hydraulics [13].
The applicability of RANS-based models is constrained when addressing scenarios in which turbulent transport primarily arises from large-scale structures.The DNS approach is preferable in these circumstances, but it significantly increases the computational cost, making it inappropriate for practical problems.Both LES and the advanced version by Sotiropoulos (2015) [15] explicitly capture only scales exceeding the mesh size of the affordable grid.Moreover, advanced DNS and LES techniques, including the hybrid LES/RANS approach, have the capacity to address highly intricate real-world multiphysics problems while comprehensively capturing all aspects of turbulent motion.This work uses numerical analysis to evaluate the flow through screens(with a blockage ratio of 65 %) using FVM, the volume of fluid (VOF), k-ω SST, k-ϵ STD, k-ϵ RNG, and Reynolds Stress Model (RSM), and LES by using the Ansys FLUENT software.The author's experimental results confirm the numerical velocity and water surface profiles.A 3-D Acoustic Doppler Velocimetry (3D ADV) device is employed for the measurement of instantaneous flow velocities.We utilized the Vectrino Plus, a four-receiver down-looking Acoustic Doppler Velocimeter (ADV) probe, which notably decreased measurement noise signal compared to a three-receiver probe.To record instantaneous three-dimensional flow velocities, the system functioned at an acoustic frequency of 10 MHz and collected data at a frequency of 100 Hz.It is not possible to acquire data in close proximity to the free water surface due to the measurement location being positioned 5 cm below the probe.

Methodology
To achieve statistical time independence for the time-averaged velocities, a sampling duration of 300 s was employed.The signal-to-noise (SNR) ratio and correlation coefficient were maintained at their minimum values, which were 20 and 74, respectively.Due to the interaction between incident and reflected pulses, the Vectrino Plus signal displays spikes in the near-bed flow region.Hence, the raw data underwent filtration through the utilization of the phase-space threshold approach, a spike removal algorithm devised by Goring and Nikora [16].

Three-dimensional hydrodynamic turbulent flow modeling
The CFD software ANSYS-Fluent 2022R2 was used for the numerical model, and 3D CFD analysis using Eulerian Multiphase solver with VOF has been performed to track the water surface profile.The first step in simulating a flow condition using a numerical scheme is to set up a computational grid within a defined computational domain.

Hydrodynamic model governing equations
Eulerian approach has been used for the numerical simulation of multiphase flows with threedimensional double precision (3ddp) solver.The continuity and momentum equation solved by Fluent is as follows.

Continuity equation
The continuity equation was utilized to monitor the boundary between the two phases.The continuity equation for the q th phase, can be shown in the following form: where − → u q is velocity of q phases and α is the volume of fraction.
The volume fraction for the primary phase is computed using the following equation The equation of volume fraction can be solved either explicitly or implicitly.

Momentum equation
In the Volume-of-Fluid (VOF) multiphase method, a single momentum equation is resolved within the flow region.This momentum equation, pertaining to phase q yields ∂ ∂t Eq. 3 can be transformed as RANS equation where p = pressure, g = acceleration due to gravity, u = average velocity.

Volume of Fluid (VOF) method for simulating free-surface
The VOF methodology establishes the shape and position of a constant-pressure free surface boundary represented by utilizing the concept of a fractional volume of liquid.To distinguish between the full and empty cells in the meshing volume, it employs a filling technique [17].In a fixed Eulerian mesh representing three-dimensional flow, a volume fraction field (F) is established with values ranging from 1 to 0, corresponding to whether the cell is entirely occupied by liquid or unoccupied.A partial fill with the free surface within the cell is indicated by a value of F between 0 and 1.The air-water interface in the VOF model was resolved using the georeconstruct scheme approach.In this scheme, when a cell is entirely occupied by one phase or the other, standard interpolation techniques are employed to calculate the face fluxes.The geometric reconstruction method employs a piecewise linear approach to represent the boundary between fluid phases.The first step of this approach relies on information regarding the volume fraction and its derivatives within the cell, enabling the determination of the position of the linear interface relative to the center of each partially filled cell.The second step involves computing the quantity of fluid being transported through each interface using the computed linear interface representation and data regarding the normal and tangential velocity profiles on that interface.The third step entails determining the volume fraction within each cell by employing the flux balance computed in the preceding step.

Numerical Modeling
Eqs. 1 and 3 were discretized and solved using the finite-volume method (FVM) for the variables u, v, w, and p, involving the integration of these equations across the elementary control volume.
To obtain numerical solutions for Eqs. 1 and 3 and to compute the free-surface profile using the Volume of Fluid (VOF) method, we employed the ANSYS-Fluent 2022R2 software [18].The computational domain was completely empty (i.e., F = 0) when the time-dependent solution method was initiated.Void elements do not exert any influence on fluid dynamics; thus, the finite-volume equations were exclusively formulated for elements that were either completely filled or partially filled.A second-order upwind scheme was employed to discretize the momentum equation and turbulent quantities.We applied the Semi-Implicit Method for Pressure-Linked Equations (SIMPLE) algorithm, as outlined by Patankar (1972) [19], for the purpose of pressure-velocity coupling.This algorithm establishes a connection between velocity and pressure corrections to ensure mass conservation and derive the pressure distribution.For pressure discretization, the pressure staggering option (PRESTO) scheme was used [20].

Computational Domain, Initial, and Boundary Conditions
The conditions defined for the numerical simulations mirrored those applied in the experimental setup.Fig. 2 depicts the boundary conditions and the geometry of the computational domain used in the numerical simulations.The fluid-wall interface, i.e., the channel bottom, the side wall, and the screen surface all had zero velocity components (u = 0, v = 0,w = 0), which were used as the no-slip boundary condition.The flow's free surface, which has pressure (p) = 0, is represented as the top boundary.The outlet boundary at the channel end was subjected to the zero-pressure condition.The measured approximation of the average velocity at the inlet boundary, u 0 = 0.102 m/s, was used.At the initiation of the time-dependent solution approach, the initial conditions were defined as F = 0 within the computational domain and F = 1 at the inlet boundary at t = 0. Based on the outcomes of initial computations, a timestep of t = 0.01 s was determined to be suitable for achieving timestep-independent solutions.A limit of 10 iterations was imposed for each timestep.The convergence thresholds for continuity, velocities, turbulent kinetic energy, and dissipation rate were set at 10 −4 .After initializing the entire flow field, the patching process was done for particular variables into different cells.In the present simulation, a cell register was created for a 0.2 m depth water zone, and the cell register was patched with a value of 1.0 for the water volume fraction.approach for assessing the numerical discretization uncertainty in computational results [21].The fine-grid convergence index is defined by comparing the three grids using the Richardson error estimator is where represents an estimate of the relative error between medium and fine mesh solutions, denote the velocities obtained from medium and fine mesh configurations with grid spacings of d 2 and d 3 , respectively, and P = local order of accuracy.P is determined for the three-grid solutions through the solution of the following equation: in which e 12 = u s1 − u s2 , e 23 = u s2 − u s3 , and r 12 = d 1 /d 2 and r 23 = d 2 /d 3 represent the grid refinement factors between the coarse and medium grids and between the medium and fine grids, respectively.The grid spacing for the current three-grid comparisons is as follows The numerical errors due to discretization were determined using the profiles of computed streamwise velocities at x = 5.7 m, 5.9 m, 6.1 m, and 6.5 m in this study.Calculations for the GCI values in computed velocity profiles at x = 5.7 m, 5.9 m, 6.1 m, and 6.5 m using the k-ϵ standard turbulence model are shown in Table 3.The highest level of discretization uncertainty observed in the velocity profiles selected for the medium-grid solutions on Mesh 2 is determined to be 1.77%.The error assessments within the present three-grid comparisons, as shown in Table 3, reveal that the numerical discretization uncertainty in the computed velocities for Mesh 2 is below 2%, signifying excellent accuracy.Table 3. Sample error estimates for velocity profiles at x= 5.7 m, 5.9 m, 6.1 m and 6.5 m.

Validation of the Models
The observed and numerically simulated free-surface profiles obtained through the Volume of Fluid (VOF) approach employing all turbulence models and LES on Mesh 2, which performs better in estimating the velocity field are shown in Fig. 3.It illustrates that the flow profile computed in all five cases closely matches the observed profile across the entire computational domain at a flow rate of 0.04 m 3 /s.

Experimental and Computed Velocity Profiles
The observed and numerically simulated streamwise velocity profiles derived from the turbulence models and Large Eddy Simulation (LES) on Mesh 2 at different parts of the channel flow x = 5.7 m, 5.9 m, 6.1 m, and 6.5 m along the streamwise direction are shown in Fig. 4. The mean square error (MSE) is used to provide a quantitative comparison of observed and simulated velocity measurements.
in which u n m and u n c represent the observed and numerically simulated streamwise velocities, respectively; and N represents the total count of data points on the velocity profile.The MSE results from Eq. 7 for various channel sections for the flow rate of 0.04 m 3 /s are given in Table 4.In the screen downstream region, where the influence of the streamline curvature is significant, different turbulence models perform better at different sections.In terms of the mean MSE values in Table 4, the k-ε RNG turbulence model predicts the streamwise velocity component better in the upstream region of the screen, whereas downstream it gives poor results.At the downstream location of 6.5 m both k-ω SST and RSM models are giving better results.In most sections of the flow, the k-ω SST outperforms the other turbulence models.In this region, RSM is the second most effective turbulence model in computing the streamwise velocity component.

Conclusions
The free-surface flow through the vertical screen was studied experimentally and numerically.A 3D Acoustic Doppler Velocimetry instrument was employed for the quantification of velocity patterns in the free-surface flow.Employing k-ω SST, RSM, k-ϵ standard, k-ϵ RNG turbulence models, and LES, the finite volume approach was used to solve the governing equations.When the experimental and numerical findings are compared, the simulations employing the k-ω SST produce marginally more accurate predictions for the streamwise velocities compared to the alternative closure models.The computational profiles of the free-surface flow generated from all five scenarios was found to be consistent with the experimental data reasonably well.Conclusively, the primary discoveries of this investigation are summarized as follows.
• Throughout the computational domain, the computed flow profiles considering all five cases agree well with the measured profile.• During streamwise velocity computation, it is noticed that different turbulence models perform better in different regions.• The k-ε RNG turbulence model predicts the streamwise velocity better in the upstream region of the screen.• Both the k-ω SST and RSM models perform better at the downstream region at 6.5 m.
• For computing the streamwise velocity in most portions of the flow, the k-ω SST outperforms the other models, and RSM turbulence model rank as the second most effective.• Velocity contours obtained from k-ω SST, and RSM are almost identical in nature.
Comparisons of experimental observations with numerical findings show that computational fluid dynamics (CFD) approaches are successful in modeling complex flow cases as flowthrough trash racks at higher blockage ratios (Br=65%) and numerical simulation can give practical benefits for studying such flow problems without resorting to laboratory tests.
2.1.Experimental SetupThe experiments are carried out in the Hydraulic Engineering Laboratory at the Indian Institute of Technology Kharagpur, India in a 10 m-long glass-walled rectangular recirculating flume having 0.6 m width and 0.65 m depth.The longitudinal slope of the channel bed is consistent throughout the flume at 0.3 %.Fig.1depicts the definition sketch of the flume with the vertical screen and ADV.A valve regulated the incoming flow rate, and the flow meter measured it.To regulate the water depth in the flume, a tailgate positioned at the downstream end of the flume was utilized.The water depths are measured to the nearest ±1 using a movable point gauge.

Figure 1 .
Figure 1.Definition sketch of the flume with the vertical screen and ADV

Figure 2 .
Figure 2. computational domain for flow through the vertical screen with boundary conditions.

Figure 3 .
Figure 3. Comparisons of measured and computed vertical screen's water-surface profiles obtained for grid size=0.01mwith flow rate 0.04 m 3 /s

Fig. 5
Fig.5illustrates the velocity contours of all five cases around the vertical trash rack.Velocity contours obtained from k-ω SST, and RSM are almost identical in nature, whereas little deviation is noticed in LES.Flow development attains relatively faster in k-ε RNG.

Figure 4 .Figure 5 .
Figure 4. Comparisons of measured and computed vertical screen's streamwise velocity profiles obtained by the present models at four different sections for grid size=0.01m with flow rate 0.04 m 3 /s

Table 1 .
CFD-model set-up with different boundary conditions.
4. Computational Meshes4.1.Discretization Error EstimationTo validate the computed velocities with the three-mesh system, we computed a Grid Convergence Index (GCI).This method is the most commonly employed and dependable

Table 2 .
P valuesx (m) P max P min P avg

Table 4 .
MSE (m 2 /s 2 ) values for streamwise velocity profiles at upstream and down stream of the vertical screen for the five models