CFD PREDICTION OF WIND PRESSURES ON CONICAL TANK

CFD PREDICTION OF WIND PRESSURES ON CONICAL TANK T.A.Sundaravadivel a, S.Nadaraja Pillai b, K.M.Parammasivam c a Lecturer, Dept of Aeronautical Engg, Satyabama University, Chennai, India, aerovelu@yahoo.com b PhD Research Scholar, WERC, Tokyo Polytechnic University, Japan. c JSPS fellow, WERC, Tokyo Polytechnic University, Japan ABSTRACT Computational analysis was performed using versatile fluid analysis software. The analysis was made in an unsteady three-dimensional turbulent flow with SST k-? as a turbulence model. Wind pressures on a conical tank have been predicted from this study. On the leeward side, strong intensity of RMS pressures are observed. This is consistent with RMS velocities on the same section. Conical water tank has a complex geometry, for which CFD is applied and results are validated with the experimental data for the mean pressure coefficients. Predicted mean pressure coefficients from the computational study were found to be in reasonably good agreement with experimental values for the tank, except in wake regions. Key Words: Computational analysis, Fluent 6.2, SST k-? model, Pressure?uctuations, conical water tank INTRODUCTION Developments in software and computer hardware have given increased impetus to the use of computer modeling research in recent years. If numerical simulations are used, need for validation arises for the results to be of practical use. Predictions can be validated against analytical solutions or data taken from experiments. Analytical solutions to standard problems can be found in the literature for many cases but to?nd existing experimental data that suit the problem under study can be difficult. However, for most practical problems no standard analytical solution exists and recourse to experimental data is required. Pressure?uctuations on bluff bodies have received a great deal of attention in recent years because they cause wind noise and structural damage. The knowledge can be obtained by experimental studies or computational studies. Performing an experimental study to understand the nature of pressure?uctuations is hard due to the sensitivity of pressure?uctuations to the size of the probe. An alternative approach is to develop a computational model that can simulate the?ow and predict the parameters of interest. Water tanks are tall, slender, non aerodynamic bodies with large mass on top and they are erected in all kinds of terrains to ensure adequate water supply to homes and industrial buildings. Scant information is available so far for 1

evaluation of the flow field and the aerodynamic loads on water tank towers or similar tall structures of variable cross section. Nowadays Computational modeling has become a powerful tool for wind engineering studies, which provides more precise information about the flow field over the complete structure. Moreover the flow field can be visualized and a better understanding can be gained using the CFD in addition to the wind tunnel tests. Flow field behind the structures such as the manner of vortex shedding etc can be better visualized in CFD studies. In the last three decades, extensive research work has been reported in the literature on flow past non-streamlined bodies because of its wide spread application in variety of engineering problems. Computational Wind Engineering has evolved as a new branch of Computational Fluid Dynamics (CFD) in the last two decades for evaluation of the interaction between wind and buildings numerically through mathematical modeling. THE EXPERIMENTAL STUDY Conical water tank towers were chosen for this study because of their failure due to cyclones on Shriharikota Island in 1984. Venkateswaralu et. al. (2007) discussed the reasons for the failure of the water tank on Sriharikota from the structural design viewpoint. In the experiments carried out by Parammasivam etal (2005 & 2007) in a boundary layer wind tunnel having a test section of 2.2m W x 1.8m H x 19m L, free stream velocity was fixed at 10 m/s at the tip of the water tower model and the corresponding Reynolds Number was 26000 based on the shaft diameter for a = 0.27. The conical tower model was fabricated from acrylic material to a 1:200 scale with 168 pressure taps on 11 levels along the height of the tower as shown in Fig. 1(84 on both shaft-bottom and top-cone sections). It was reported that Cp rms in the stagnation region is approximately proportional to the turbulence intensity of the approaching flow for smooth cylindrical surface, and has a peak at a point around the minimum pressure coefficient. The Cp (mean and rms) distributions for the conical water tank at various levels plotted from experimental data are shown in Figs. 2 to 5. THE COMPUTATIONAL STUDY The model used by Parammasivam et. al. (2005 & 2007) for the experiment is used for the present computational study, in which the SST k-? turbulence model is a two-equation eddy viscosity model which has become very popular. The use of k-? formulation in the inner parts of the boundary layer makes it directly usable all the way down to the wall through the viscous sub layer. Hence the SST k-? model can be used as a low Reynolds Number turbulence model without any extra damping functions. The SST formulation also switches to a k-e behavior in the free stream and thereby avoids the common k-? problem that the model is too sensitive to inlet free stream proprieties. Authors 2

who use the SST k-? model often merit it for its good behavior in adverse pressure gradients and separating flow. The SST k-? model produces a bit too large turbulence levels in regions with normal strain, like stagnation regions and regions with strong acceleration. In the conical tower surface and wall, the velocity components u, v & w are set to zero. At Inlet 1, u = U1 and at Inlet 2, u = U. At the outlet of the mesh, pressure is set to zero, which denotes the atmospheric pressure. Were u = Velocity component in the x-direction, v = Velocity component in the y-direction, w = Velocity component in the z-direction, U1= velocity profile corresponding to 0.27 power law coefficient & U = constant velocity. The computational domain is discretized in to 6, 52, 875 nodes, 6, 29, 676 cells and 19, 12, 006 faces. The inlet of the computational domain is discretized into two sections as inlet 1 and inlet 2. Inlet 1 is used to introduce the velocity profile using an UDF (User Defined Function) corresponding to the power law coefficient of 0.27 and inlet 2 has uniform velocity as obtained from the inlet 1 at corresponding height. The computational domain for the study is shown in Fig. 6. The shaft portion is divided into 36 divisions circumferentially and 25 divisions longitudinally. The cone section is divided into 36 divisions circumferentially and 15 divisions longitudinally. Finer mesh is made near the model and the coarseness of the mesh is increased away from the model as shown in Fig. 7. CFD PREDICTION OF WIND PRESSURES In spite of vast research material available on flow past simple circular cylinder, our understanding of the complex fluid mechanics for flow past circular cylinders at Reynolds numbers in excess of a few hundred thousand still remains incomplete. The computational analysis was performed using the versatile fluid analysis software package Fluent 6.2 using the finite volume method. The analysis was made in unsteady three-dimensional turbulent flow. The SST k-? model was used as a turbulent model for the present study. The existing experimental data by Parammasivam et. al. (2005 & 2007) has been used for the comparison of the CFD data. At the inlet, the velocity profile was introduced with the power law coefficient of 0.27, same as in the experiments. At the base of the shaft two clear symmetrical vortices are observed in contour plots as shown in Figs. 8 and 9 with less intensity of fluctuating velocities. It is expected that the flow is symmetrical with respect to the low velocity at the bottom of the model. The two vortices are formed at the leeward face of the model. It is clearly observed from Figs. 10 and 11. Vortices get mixed as the shaft height increases and near shaft-cone intersection (z/h = 0.73) two vortices are formed along with the shear layers from the cone. The predicted pressure coefficients and the RMS pressures on the conical tank are shown as contour plots in Figs. 12 and 13. On the leeward side of 3

the cone section strong intensity of RMS pressures are observed. This is consistent with RMS velocities on the cone section. The shear layers over the cone form two distinct vortices on the leeward side of the cone surface and it is shown in the Fig. 13. The plots of mean Cp vs circumferential angle for the 3 typical levels of the shaft (z/h = 0.1, 0.4 & 0.68) are shown in Figs. 14, 15 & 16 and similar plots for the cone sections (z/h = 0.73, 0.91&0.97) are shown in Figs. 17 to 19 along with the experimental results. It is clear that the predicted patterns of pressure coefficients from the computational study are found to be in reasonably good agreement for the conical tower except at circumferential angles from 90 degrees to 270 degrees. At 90 degrees to 270 degrees of the conical tank, the SST k-? model could not match the experimental data due to the vortices and turbulent nature of the flow field and finer mesh is needed at these regions to catch the wake. RMS pressures had peaks on the leeward side of the cone surfaces. The predicted profile coincides with the experimental one in both base levels (Fig. 14) as well as the levels at the cone surfaces (Figs. 17-19). The minimum value of mean Cp is found at the two locations approx at 80 degrees and 280 degrees from the wind flow direction. The result indicates that the flow separates from those points (80 degrees and 280 degrees). This agrees with the theory. Flow over the cone section of water tank tower is three-dimensional as against the shaft section, and can be considered as 2-D flow. CONCLUSIONS The adopted solution method for the velocity pressure fields was the SIMPLE Algorithm (Semi-Implicit Method for Pressure Linked Equations). PISO- Pressure Implicit Split operator can be used to improve the accuracy of the pressure filed. Some characteristics of the vertical structures of the shear layer behind the conical tower have been examined and it is found that two strong vortices are formed on the leeward faces. In order to enhance the stability of the solution process, under-relaxation techniques were applied to all the equations. Otherwise iteration may diverge. A finer mesh is required in the vicinity of walls and ground in order to accurately resolve the high-gradient regions of the flow field. One of the main problems in turbulence modeling is the accurate prediction of flow separation from a smooth surface. The k-? based Shear Stress Transport (SST) model was designed to give highly accurate predictions of the onset and the amount of flow separation under adverse pressure gradients by the inclusion of transport effects into the formulation of the eddy- viscosity. Due to the complex nature of the water tank structure and the inlet velocity profile, flow in the leeward side of the model will be highly turbulent and large eddy formation takes place. As mentioned by Lars Davidson (2003), the eddy viscosity models are simple due to the use of an isotropic eddy (turbulent) viscosity and as a consequence of the above; the model is found to be unable to account for curvature effects. So the results show that the k-? based Shear Stress Transport (SST) model is less effective in predicting the wake region in this study. For better accuracy of results, future study can be conducted using 4

Reynolds Stress model or LES (with a higher configuration computer system/ workstation) in which the above mentioned problem can be solved with the aid of finer mesh in the vicinity of walls. The mean flow characteristics appear to have been captured by the computational modeling, which attests the reasonability of the approach for the study. NOTATION a Power Law Coefficient u Velocity component in the x direction (m/s) v Velocity component in the y direction (m/s) w Velocity component in the z direction (m/s) mean Cp Mean Coefficient of pressure rms Cp rms coefficient of pressure z/h Ratio of height of a section to overall height of the water tank. REFERENCES 1. Bergstrom, Derksen and Rezkallah (1993), Numerical study of wind flow over a cooling tower J. Wind Eng. Ind. Aerodyn., Vol. 46, pp.657-664. 2. Fluent, Fluent 6 User s Guide2, Fluent INC., Lebanon, U.S.A, 2004 3. Fujisawa, Asano, Arakawa and Hashimoto (2005), Computational and experimental study on flow around a rotationally oscillating cylinder in a uniform flow J. Wind Eng. Ind. Aerodyn., Vol. 93, 137-153. 4. Gao and Chow (2005), Numerical studies on airflow around a cube, J. Wind Eng. Ind. Aerodyn., Vol.93, pp. 115-135. 5. Lars Davidson (2003), An Introduction to Turbulence models Publication 97/2, Dept. of Thermo and Fluid Dynamics, Chalmers University of Tech., GÖteborg, Sweden 6. Parammasivam and Yukio Tamura (2007), Aerodynamic characteristics of a conical water tank, Proceedings of 2007 Annual Meeting, Japan Society of Fluid Mechanics, Japan, pp.32. 7. Parammasivam (2005), Wind Tunnel Studies on Water Tank Tower with Terrain Simulation, Ph.D. Thesis, Anna University, Chennai. 8. Paterson (1993), Predicting rms pressure from computed velocities and mean pressures, J. Wind Eng. Ind. Aerodyn., Vol. 46, pp. 431 437. 9. Reichrath and Davies (2002), Computational fluid dynamics simulations and validation of the pressure distribution on the roof of a commercial multi-span venlo-type glass house J.Wind Eng. Ind.Aerodyn.,Vol.90, pp.139-49. 10. Senthooran,Dong-Dae Lee & Parameswaran (2004), A Computational model to calculate the flow induced pressure fluctuations on buildings J. Wind Eng. Ind. Aerodyn., Vol. 92, 1131-1145. 11. Venkateswaralu, Lakshmanan, Shanmugasundaram and Balakrishna Rao (1995), Failure of water tower shafts due to cyclonic winds, 9ICWE, pp. 1467 1478. 5

Fig. 4 rms Cp vs Angle for cone section (Experimental Data) Fig. 1 Model Dimensions and Levels Fig. 5 rms Cp vs Angle for shaft section (Experimental Data) Fig. 2 Mean Cp vs Angle for shaft section (Experimental Data) Fig. 6 Computational Domain and Grid System Fig. 3 Mean Cp vs Angle for cone section (Experimental Data) Fig. 7 Mesh Close to the model. 6

Fig.8 Contours of Velocity magnitude at z/h=0.73 Fig.9 Contours of Velocity magnitude at z/h=0.1 Fig. 10 Contours of RMS Velocity (m/s) at z/h=0.73 7

Fig. 11 Contours of RMS Velocity (m/s) at z/h=0.1 Fig.12 Contours of Pressure Coefficient Fig.13 Contours of RMS Static Pressure (pascal) 8

Fig.14 Mean Cp vs Angle at z/h = 0.1 Fig.15 Mean Cp vs Angle at z/h = 0.4 Fig. 16 Mean Cp vs Angle at z/h = 0.68 9

Fig. 17 Mean Cp vs Angle at z/h = 0.73 Fig.18 Mean Cp vs Angle at z/h = 0.91 Fig.19 Mean Cp vs Angle at z/h = 0.97 10