Inlet efficiency is a requirement for characterizing the flow transfers between surface and sewer flow during rain events. The dual drainage approach is based on the joint analysis of both upper and lower drainage levels, and the flow transfer is one of the relevant elements to define properly this joint behaviour. This paper presents the results of an experimental and numerical investigation about the inlet efficiency definition. A full scale (1:1) test platform located in the Technical University of Catalonia (UPC) reproduces both the runoff process in streets and the water entering the inlet. Data from tests performed on this platform allow the inlet efficiency to be estimated as a function of significant hydraulic and geometrical parameters. A reproduction of these tests through a numerical three-dimensional code (Flow-3D) has been carried out simulating this type of flow by solving the RANS equations. The aim of the work was to reproduce the hydraulic performance of a previously tested grated inlet under several flow and geometric conditions using Flow-3D as a virtual laboratory. This will allow inlet efficiencies to be obtained without previous experimental tests. Moreover, the 3D model allows a better understanding of the hydraulics of the flow interception and the flow patterns approaching the inlet.
During extreme rainfall events uncontrolled amounts of runoff that are not captured by the surface drainage inlet system. This can produce serious hazard conditions for pedestrians and vehicles. These can cause significant direct and indirect damages related, respectively, to the assets exposed to flooding and the activities that can be affected (e.g. traffic disruption). In this context, it is clear that the surface drainage system needs to be composed by a series of well-located inlets. In order to determine correctly the inlet spacing need to guarantee safe conditions for pedestrians and vehicles during a storm event and to avoid economic losses, a full knowledge of the hydraulic behaviour of the flow approaching the inlet and its performance is essential (FHwA, 1979).
So, the drainage system must then be understood not only as a number of pipes but as a set of streets, grates and pipes which interact. This is the concept of dual drainage, which considers the stormwater flowing in two parallel layers, one formed by underground sewers and the other by the network of streets, interconnected by the ‘link element’, the inlets (Schmitt et al. 2004).
Nowadays, in numerous cities, it is quite common to see serious urban floods while the underground collectors are half empty. This is simply due to a deficit in flow collection, causing an excess of uncontrolled water flowing along the streets that could be increased due to clogging problems in the inlets, responsible for many flood events (ten Veldhuis & Clemens 2011), where efficiency has been observed to reduce to one third of the original value estimated in clean conditions (Gómez et al. 2013). In these cases, the global drainage system has not been well designed, because the focus has concentrated only on the sewer design, assuming that 100% of runoff arrives to the pipe system. In order to correct this, the number of inlets should be increased or inlet positions should be modified. Another option could be to modify the dimensions and the geometry of the grates in order to increase their efficiency.
However, to do this, it is necessary to evaluate and quantify the water exchange through the grate. This flow collection for a rain event depends on several factors such as the grate size, its geometry, the street geometry and spatial density of the inlets. Following this idea, a better understanding of the hydraulics of this element and the interactions between surface flow and the underground drainage systems is clearly needed. Some institutions or companies have promoted the experimental testing of inlets. Examples of this type of study can be found in the technical literature, such as Li (1956), Argue (1986), Spaliviero & May (1998), FHwA (2009) or Gómez & Russo (2011), but manufacturers or municipal technicians do not have the resources to test all the different grates that they use. Therefore, one option could be the use of a three-dimensional (3D) code to simulate the flow behaviour of the grates, in some ways like a virtual laboratory.
In recent years, several experiments using 3D simulations have been carried out (Djordjević et al. 2013; Lopes et al. 2013), but these have focused on the hydraulics of the inlet manhole with poor regard to the efficiency of the grated inlet defined as the ratio between the intercepted flow and the flow approaching the inlet.
Lopes et al. (2013) developed a 3D approach using OpenFOAM® code to study the surcharge flow in a gully, especially focusing on the jet characterization and the height it reaches above the gully. The code and a very detailed mesh allowed the researchers to obtain good similarity between numerical and experimental results. Djordjević et al. (2013) carried out a 3D study of the flow pattern near one grate with the same code, considering the flow in both directions, entering the grate and leaving the sewer.
Noted above, these experiments did not focus on the hydraulic efficiency of the grates, so, in this context, a 3D computer code to reproduce grated inlet performance was applied and the results are shown in this paper. This paper focuses on the 3D modelling of one specific inlet, the so-called ‘Barcelona1’, one of the most common grates in the metropolitan area of Barcelona, Spain. The inlet was previously tested in the UPC hydraulic laboratory which enables us to compare the numerical results with the experimental values.
PHYSICAL MODEL: EXPERIMENTAL SET UP
For different combinations of circulating flow Q (25, 50, 100, 150 and 200 L/s), and longitudinal (0, 0.5, 1, 2, 4, 6, 8, and 10%) and transverse (0, 1, 2, 3, and 4%) slopes, intercepted flow Qint was measured. Water levels next to the inlet (immediately upstream) were measured, too. These experimental data were compared to the data obtained by the 3D calculations.
The computer code used for the simulation is Flow-3D. It is a commercial code developed by Flow Science Inc. of the type called CFD (computational fluid dynamics) for a general three-dimensional analysis. The three-dimensional numerical modelling developed through Flow-3D code is used for numerous applications by incorporating a ‘multiphysics’ environment (considering different types of fluids) and is especially suited for simulation of free surface flows. The numerically solved equations by Flow-3D for hydraulic studies are mass and momentum conservation equations with some additional terms:
where (2) is the continuity, Equations (3)–(5) are the Navier-Stokes equations, with u, v and w being the velocity components in the x, y and z directions, respectively. In addition, Flow-3D adds some components to the equations:
Ai: Fractional area open to flow in the i direction
R: coefficient used to change Cartesian to cylindrical coordinates
ξ: For Cartesian coordinates this has a value of 0
RSOR: Mass source. You can add flow entries, for example
VF: Fraction volume of fluid (VOF)
uw, δus: Components of relative velocities related to the mass source. For this study, they are not taken into account
Gi: Part of the gravity acceleration in the i direction
fi: Component of the viscous forces in the i direction
bi: A factor that is only taken into account when there are porous media. It was 0 in calculations of this study.
The code solves the 3D Reynolds Averaged Navier Stokes equations (RANS) with a numerical scheme considering finite volumes (Savage & Johnson 2001). The flow domain is subdivided using Cartesian coordinates considering a 3D mesh composed by variable-sized hexahedral cells, with smaller dimensions in the inlet zone. In a first analysis, this type of network may be considered as a limitation, but it is advantageous because the process to create the mesh is relatively easy and less memory is needed using the tools, VOF and FAVOR™, in Flow-3D.
For each cell, the numerical scheme considers the values for pressure and velocity at discrete times as indicated in the user's manual. The grid assumes that all variables are calculated at the geometrical centre of each cell (hexahedrons), except the velocities and fractional areas in the boundary cells. The last two are considered in the centre of the cell faces normal to each direction. All terms of the RANS equations are computed from the current time-step values of each variable with an explicit numerical scheme, although other implicit options are available, as indicated in the technical documents of Flow-3D. The explicit approach generates an efficient numerical scheme that is more easy to program, but requires a limited time-step value to ensure the stability and accuracy of the results, as happens in all explicit numerical schemes.
If a mesh with square or rectangular sides is used, it is difficult to define curved elements. One possibility is to define a precise mesh with a very small dimension for the hexahedrons and so produce a soft contour, but this incurs a high computational cost.
One advantage of the VOF method over other methods that define the free surface is that in the VOF method the mesh remains fixed and therefore there is no mesh deformation. This makes the computer algorithms easier, providing better CPU performance and therefore a lower computational cost, although it is still high.
The turbulence model, chosen among all the possibilities included in Flow-3D, is the RNG (renormalized group) (Yakhot & Orszag 1986; Yakhot & Smith 1992). It applies probabilistic methods to the derivatives of the equations describing the amount of turbulence, as turbulent kinetic energy and rate dissipation. This model uses equations similar to the k-ɛ model, although constants of the equations in the k-ɛ model are empirical while in the RNG model they are explicitly derived (Smagorinsky 1963).
The choice of this turbulence model was made after a calibration between the physical and numerical model in which several turbulence models, such as RNG, K-ɛ and LES (Large Eddy Simulation) were tested in order to achieve the best of both numerical accuracy and computational cost.
The defined mesh is composed of 1,336,440 cells representing 2.57 m3 of simulated volume (real scale). Mesh blocks with an element size of 2 cm for the main part of the platform and a mesh block with cells of 1 cm in the vicinity of the inlet were used. Increasing precision near to the inlet allows us to increase the precision of the intercepted flow and therefore of the model results. The 1 cm cell size has been established according to the geometry of the inlet. With the FAVOR™ algorithm, it is possible to see how the program interprets the ‘Barcelona1’ inlet.
Despite Figure 2, in which it is possible to see that initially the platform is empty in the model, the initial condition of the simulation, from now on, has been modified. In the experimental set up in laboratory, the model starts with the platform empty, and it fills progressively to reach a steady flow. In the numerical model, the simulation starts with the platform partially filled with water. This has been done to decrease the computer time and because the results of this study consider only steady flow conditions.
COMPARISON OF EXPERIMENTAL AND NUMERICAL RESULTS
Different set ups (longitudinal and transverse slopes) with the same inlet (Barcelona1) were considered in this study to analyse the interaction between surface flow and pipe flow, and specifically the flow interception phenomenon through the grate. In all cases, the flow captured by the inlet is not influenced by other conditions, so all the flow enters through the inlet with no restrictions that could appear due to the pressure flow in the sewer systems.
Computer time is currently a limiting drawback of the numerical analysis. The average time of simulation oscillates around 2 or 3 days using a computer, Intel Core TM with 2 CPU, 2.3 GHz and 2.99 Gb RAM. A more powerful workstation or the use of GPUs could reduce the computational time but nowadays there is no commercial version of the software including this feature.
Small irregularities in the platform can produce non-negligible modifications in flow patterns for low flows (25 L/s). This consideration could explain the relative error (23%) found in the 25 L/s simulation although the absolute error is only 3 L/s. On the other hand, for flows of 150 L/s and above, the error reaches 10% of measured collected flow and, again, absolute errors are only 3.5 L/s. This could be due to the characteristics of the upstream tank. It is not large enough to dissipate all the energy introduced by the injection of high flows and turbulence prevents the generation of a complete one-direction flow condition upstream the inlet and distorts the accuracy of results.
In order to assure a good response of the simulation working with high inflows, it will be convenient to simulate a deeper upstream tank and a larger platform. In this way, clearer one-direction flow behaviour upstream of the inlet could be achieved, at the cost of increasing the computational time. However, the object of this study is not to generate the best simulation but to reproduce as accurately as possible the experimental set up previously used.
It can be seen that for low input flows, the simulation model captures more water than observed in the experiments, while for high flow rates the opposite happens. In any case, excluding the extreme flows, the simulated values fit adequately the experimental results (errors of 4% or less of the total collected flow). Moreover, in terms of absolute errors the differences are usually lower than 1 to 2 L/s. A similar graph for water depths immediately upstream the inlet can be obtained (Figure 9). In this graph, it is possible to observe an error of a few millimetres in absolute values, and less than 10% of measured water depth for relative values.
Taking into account the accuracy of the results of both models, the match between observed and simulated depths upstream of the inlet, the only place where ‘y’ was measured, is quite good. As a matter of fact, the measurements in the physical model are made with a millimetre ruler (1 mm precision) and the cells of the numerical model, which are 2 cm height just before the inlet and 1 cm height within the inlet (the measurement was taken in the border of this two mesh blocks), had a 1–2 mm precision (with VOF code). As a general trend, numerical results underestimate the water levels but less than 1 cm in all cases.
Furthermore, numerical analysis allows us to obtain more information from each simulation. In this study, it was proposed to study the captured water, distinguishing between the frontal and the lateral contribution to the intercepted flows.
ANALYSIS OF FRONTAL AND LATERAL FLOW USING THE 3D MODEL
Other combinations of longitudinal and transverse slopes have been run in order to compare the frontal and lateral contribution to the intercepted flow. Test cases are indicated in Table 1.
|Longitudinal slope [%]||0||0||2||2||2||2||2||4||6||10|
|Transverse slope [%]||0||2||0||1||2||3||4||2||2||2|
|Longitudinal slope [%]||0||0||2||2||2||2||2||4||6||10|
|Transverse slope [%]||0||2||0||1||2||3||4||2||2||2|
From the obtained numerical outputs, we can conclude that three-dimensional modelling is a real alternative to laboratory tests, providing additional useful information. Differences between numerical and experimental values are acceptable in most cases. So, inlet grates that cannot be tested in a laboratory can be studied with the 3D model, to approach its efficiency.
Once validated, the numerical model can differentiate and quantify the frontal, side and rear flows approaching the inlet. It is possible to appreciate how this distribution varies with different combinations of inflows and longitudinal and transverse slopes.
It has been observed that, for the grate ‘Barcelona1’ and any combination of approaching flow and slopes, both SL and ST, within the scope of this study, the frontal interception is the main mechanism to capture water, representing 60–80% of the total water collected. This interception occurs mostly in the first half of the inlet while the lateral collection is distributed almost evenly along the inlet except in the first quarter of the length, a transition zone where the flow changes from a one-dimensional behaviour to a clearer two- and three-dimensional pattern.
The results of three-dimensional numerical modelling are then not only a real alternative to laboratory tests to estimate the inlet efficiency, but can even obtain key data of flow patterns that cannot always be easily seen or measured in physical models. This could help in the design of new inlet models. The only drawback at this time is the computational time. Each numerical test takes around 2 or 3 days in the average desktop PC used. Experimental analysis for one grate in the platform located at the laboratory takes 5 days, for the 200 tests usually conducted to characterize the grate according to the undertaken protocol, combinations of five different flows, eight different longitudinal slopes and five different transverse slopes. Improvements in CPU and GPU technology could reduce this time drastically, making the use of this 3D numerical approach more attractive in the near future.
This work has been developed in the project CGL2011-26958/BTE, financed by the Spanish Ministry of Economy and Competitiveness.