DEMOCRATIZATION OF 3D CFD HYDRAULIC MODELS : SEVERAL EXAMPLES PERFORMED WITH ANSYS CFX Démocratisation des modèles hydrauliques CFD 3D : plusieurs exemples réalisés avec ANSYS CFX Gwenaël CHEVALLET 1, ISL Ingénierie [Montpellier], 65 avenue Clément Ader 34170 Castelnau-le-Lez Phone: +33 (0)4.67.54.51.73, Fax: +33 (0)4.67.54.52.05, E-Mail: chevallet@isl.fr Moez JELLOULI, ISL Ingénierie [Paris], 75 boulevard Mac Donald 75019 Paris Phone: +33 (0)1.55.26.99.91, Fax: +33 (0)1.40.34.63.36, E-Mail: jellouli@isl.fr Luc DEROO, ISL Ingénierie [Lyon], 29 rue Maurice Flandin 69003 Lyon Phone: +33 (0)4.78.18.31.85, Fax: +33 (0)4.72.34.60.99, E-Mail: deroo@isl.fr KEY WORDS Dams, spillways, 3D CFD, dykes, Navier-Stokes model, free surface model, flow on structures ABSTRACT In the past, 3D hydraulic models were restricted to the study of large projects with complex hydraulic issues. Today, CFD models are operated much more commonly both in order to validate with hindsight the design of projects and/or during the design itself. ISL Ingénierie recently conducted several hydraulic models performed with ANSYS CFX (2D or 3D) for large projects but also for smaller projects where CFD modeling brings a real added value : - Design of a ski-jump spillway of a 110 m high dam in Africa : as per the international standards, the spillway was designed to safely handle the 1:10,000 year flood ; it was designed for a discharge of about 10,000 m 3 /s and is equipped with tainter gates. - Hydraulic diagnostic made using a 3D model for a hydroelectric plant in France : the purpose of this study was to determine in detail the water levels associated with the passage of the different flow rates including the design flood (discharge 1,000 m 3 /s), - Design or diagnostic of various spillways for small and medium dams. - Maritime hydraulics : Study of cross swells and forces induced on the dykes. 1. INTRODUCTION In the past, 3D hydraulic models were restricted to the study of large projects with complex hydraulic issues. Today, CFD models are operated much more commonly both in order to validate with hindsight the design of projects and/or during the design itself. ISL Ingénierie recently conducted several hydraulic models performed with ANSYS CFX (2D or 3D) for large projects but also for smaller projects where CFD modeling brings a real added value. A few examples are presented here. 1 Corresponding author
2. VARIOUS EXAMPLES PERFORMED WITH ANSYS CFX 2.1 Feasibility study and detailed design of a large dam in Africa : gated spillway preliminary and detailed design 2.1.1 Preamble ISL Ingenierie is in charge of the design of a large multipurpose dam in Africa : - Energy : provide base, firm or peak energy, - Irrigation : irrigate 50,000 ha or more, including irrigation in the resettlement area, - Livelihood : provide minimum flow and 2 floods a year. In order to design the dam spillway, 3D hydraulic calculations were carried out using ANSYS CFX software. As per the international standards, the spillway was designed to safely handle the 1:10,000 year flood, and the 110 m high dam should also be safe in case of the even larger Probable Maximum Flood occurring. It was designed for a discharge of 9,977 m 3 /s and is a gated structure, with four Tainter gates, of 17.5 m length and 15 m height. The sill is at elevation 535.00 masl (meters above seal level) and the normal water level at 550.00 masl. The flow through the ski-jump spillway is then guided to a flip bucket allowing to deflect the jet of spilling water, thus dissipating its energy far from the dam, down into the river. The flow is attacked by air and jets are disintegrated due to (I) internal turbulence, (II) shearing action of one air surrounding it, and (III) the surface tension and fall down in the shape of cascades and droplets. The figures 1 and 2 inserted below present a section of the dam and a 3D architectural model of the dam and the spillway. Figures 1 and 2: Section and 3D architectural model of the dam and the spillway The CFD model was used very soon during the design process, at the preliminary design stage. The objectives of this modeling were multiple: - Check the discharge coefficients of the weir, - Define the bucket radius of curvature and thus define the angle of the jet, - Estimate the pressure on the bucket, - Locate and dimensionnate the plunge basin. 2.1.2 Discharge coefficient of the weir The top of the spillway crest is at 535.00 masl. When the reservoir level rises above 550.00 masl, the valve begins its opening to allow water releasing. When the reservoir level reaches 550.50 masl, the gate is supposed completely opened and its lip is 15 m distant from the spillway crest level. Thus, when the gates are totally opened, the discharge formulation of an uncontrolled overflow ogee crest can be considered.
When fully opened, the discharge of one spillway sluice is given by the formula: (1) Cd = discharge coefficient Be = effective width of the sluice Cd depends on the effective head on the sill according to the following curve, where Hd is the design head. Figure 3 : Approximation of Spillway discharge coefficient [1] The curve can be approximated by the formula (2) : C d /C Dd = (H/H D ) 0.12 (2) H D is the design head = 15 m C Dd is the discharge coefficient for the design head = 0.494 B e (effective width) is related to the actual width B by the formula (3) : Be = B 2 K H (3) Where K is a coefficient depending on the profiling of the piers. Figure 4: K-coefficient for Spillway [1] With profiling as provided in the design, K can be neglected. Based on the previous assumptions, the following figure shows the rating curve of the fully opened gates. Figure 5: Stage/discharge curve Thus for a discharge of 9,977 m³/s, the reservoir level reaches the elevation of 551.10 masl. Simulations were carried out to validate the spillway geometry. Using Computational Fluid Dynamics (CFD), flow over the ski-jump spillway was simulated.
The figures below present the CFD model : Figures 6 and 7: Overall view of the spillway mesh and model itsef The numerical grid is generated as 143 330 hexahedral elements. The minimum edge length was 0.35 m for the near wall elements (elements near the spillway crest). A constant water level (551.10 masl) was imposed as an inlet condition. Downstream, for the outlet condition a water level of 457.00 m was fixed. Only half of the spillway was modelled and a symmetry condition was imposed. An opening condition was chosen for the atmospheric condition. 5 and 50 mm of equivalent sand grain roughness were adopted on the wall condition representing respectively the spillway crest and the stream bed. The Volume of Fluid (VOF) method was used for computing free surface motion. Reynolds-averaged Navier-Stokes equations were solved. The turbulence models used is k-ε with scalable wall functions. The High Resolution scheme was used for both flow and turbulence equations. The flow rate computed by the CFD model was 9,335 m 3 /s, about 6% less than the flow rate calculated with empirical methods. 2.1.3 Stream line and jet trajectory Figure 8: Comparison of streamline empirical method and CFD simulation From figure 8, it can be observed that the streamline from the CFD simulation is in good agreement with the estimation from the empirical method. Curvatures of the jet trajectory from CFD simulation differs from the one obtained with the empirical method. The path of the trajectory, given by the equation below (4) [1], was
approximated basing on a ballistic analysis where the air resistance was neglected. This assumption can explain the difference observed in the jet trajectory. The equation below (5) [1] provides another empirical evaluation of the impact position. (4) (5) With z 0 (476 m) the bucket elevation, z av (457 m) the downstream level, h 0 (3.80 m) the water depth,the velocity (32 m/s) the flow velocity at the lip and θ (25 ) the trajectory angle. The distance obtained with this equation : x = 102 m from the bucket lip. The distance extracted from figure 8 is 100 m, which is a satisfactory result. 2.1.4 Pressure Based on experimental results, pressure over the bucket can be estimated as follow [1]. Figure 9 shows the relative overpressure P over the bucket in function of ξ = h 0 /R. For the studied case: ξ = 0,21 and P ~ 0,6. Figure 9 : Empirical overpressure The curves overpressure : p f = P.ρ.V²/2 = 0,27 MPa. The pressure over the bucket : p f = ρ.g.h 0 + p f = 0,3 MPa. Thus, the empirical pressure agrees with the averaged pressure obtained with the simulation which is displayed over the spillway crest on figure 10. For information, the pressure over the stream bed is also given on figure 11. Figures 10 and 11 : Pressure over the spillway crest and over the stream bed
2.2 3D hydraulics modeling of the behavior of a headrace canal with a side spill dam and a downstream bottom gate in flood situation To make a diagnostic on the behavior of a dam and a hydroelectric plant water intake during current and flood situations (including design flood, 1,000 m 3 /s), ISL carried out 1D and 2D models which quickly found their limit due to the presence of numerous gates and lateral overflows. It was therefore decided to perform a 3D CFD model, particularly to define clearly the division of flow between the river and the water intake. The photo below presents the dam and the intake channel. An illustration of the 3D CFD model is also shown on the figure 12. Figure 12 : Presentation of the dam and 3d model (velocity field) Added value of the 3D CFD model was a better understanding of the flow pattern for the frequent and design floods. It was, thanks to the 3D CFD model, possible to estimate in detail the discharge through the different hydraulics works, the water levels in the river bed and the intake channel, the velocity fields The simulation especially showed that water level was higher than expected by the client for the design flood because the hydraulics works were largely drowned by downstream river level. 2.3 3D CFD modeling and optimization of dam spillways 2.3.1 Lateral weir and discharge channel with strong rugosity ISL Ingénierie had to study the increase of a dam spillway flood design. Indeed, this spillway was not able to evacuate the design flow (1000 year return period) without any risk for the dam. The spillway is located on the left bank and includes a 33 meters reinforced concrete weir, a concrete variable geometry reception basin, and a rock variable geometry spillway channel. At the downstream of the spillway channel, there is a high slope fall flowing into the riverbed. The photos inserted below present the dam and the spillway. Figure 13 : Views of the spillway, weir and channel ISL performed a 3D computational hydraulics model of the spillway with ANSYS CFX, in order to optimize the shape of the spillway channel to reduce the water level on the right bank training wall of the spillway channel.this 3D model was calibrated on the results of a physical model built by the University of Liège in 2007 [2].
The figures inserted below present the CFD model. Figures 14 and 15 : Velocity field and free surface A tetrahedral mesh was chosen and the total number of cells was close to 1.12 million cells (with a cell size of approximatively 20 cm on the weir). The calculation times were about 16 h on a standard desk computer for the first model and about 3h for the next models, when an initial water line in the spillway could be taken as initial condition. The 3D CFD model was able to accurately reproduce the hydraulic phenomena observed on the physical model (hydraulic jumps, stationary waves ) and the flow rates calculated for a similar reservoir level were really close (difference inferior to 4 % for a design flow of approximatively 350 m 3 /s). Two types of solutions were studied on the 3D CFD model in order to get water levels in the spillway channel under a target water line defined by the client : - Solution a) rock excavation of the left bank training wall, - Solution b) lowering the apron. 2.3.2 Discharge channel with strong convergence The dam that was the subject of this study is a rockfill dam with a watertight upstream face. Its height is about 9 m for a volume of 170,000 m 3. It was built in the 1950s and is used for drinking water. Its watershed is small (16 km 2 ). A previous study had identified a particular risk associated with the spillway. Indeed it is composed of an arc-shaped weir and a strong convergent channel. The three-dimensional aspect of the problem here is obvious. Therefore a 3D CFD model was performed. The objective was to assess if the current height of the side walls was sufficient to discharge without overflow over the side walls, in the case of a 1:1,000 year flood. 3D modeling has identified the need for a 0.7 m raising of the side walls. Figure 16: Photograph of the spillway Figure 17 : Velocity field
2.3.3 Discharge channel with stepped chutes A 3D model of this curved gravity dam with buttress was performed, during the detailed design stage, in order to make a diagnostic of the spillway with stepped chutes. The model has highlighted an oblique hydraulic jump that had already been identified on a physical model in 2007. Oblique hydraulic jump Figure 18 : Oblique hydraulic jump The difference between the flow rate computed by the CFD model and the flow rates calculated with the physical model and the empirical methods is inferior to 5 %. 2.2 Maritime hydraulics : Study of cross swells and forces induced on the dykes During the storm Xynthia in France, the sea dykes of the west atlantic coast have been damaged by crossing seas and erosion of embankment behind the works. Figure 19 : Xynthia storm damages Three approaches were used to design the reinforcement of the dykes : (I) the historical analysis and feedback, (II) the semi-empirical formulations, and more recently (III) 2D CFX modeling calibrated on the results of the CLASH program on the one hand, a case encountered in the Cotentin on the other hand (figure 20). Based on this calibration, it was possible to test the effect of a wave return wall (figure 21) and estimate the constraints on the structure. Figure 20 : Calibration of the model on a observed case Figure 21 : Design of the wave return wall
5. CONCLUSIONS Nowadays, the use of CFD models (2D or 3D, steady or unsteady state flows) is more related to the complexity of hydraulic phenomena (lateral outflows, strong flow convergence, curved discharge channels...) than the project cost or the stage of the study (feasibility, preliminary or detailed design...). Indeed, the examples carried out by ISL (mainly for free surface flow studies) show that CFD models provide real added value during diagnostic, design of new structures or optimization of existing ones. The routine use of such calculations is also possible thanks to reduced computation time, typically a few hours. The results of these models are generally very close to those of empirical approaches and special hydraulic phenomena observed in physical/experimental models (regular or oblique hydraulic jumps, stationary waves, jets ) are well reproduced. CFD models are an interesting complement to the physical models and have the advantage of being flexible for the study of reinforcement solutions or optimization. REFERENCES AND CITATIONS [1] Willi H. Hager et Anton J. Schleiss (2009), Constructions hydrauliques, volume 15 [2] Université de Liège (2007). Modèle réduit hydraulique de l évacuateur de crues du barrage de la Petite Rhue. MAIN ASSUMPTION FOR CALCULATIONS Most models developed by ISL are carried out for free surface flow studies. The main assumptions for the calculations are as follows: -The Volume Of Fluid (VOF) technique is chosen. It allows tracking and locating free fluid surfaces. This method is used for its flexibility and efficiency. -Turbulence is modeled using the k-ε model. -The scalable wall function formulation is used for modeling flow near the wall.