Mixing Process in a Water Storage Tank by CFD Simulations

Mixing Process in a Water Storage Tank by CFD Simulations
I.J. Moncho-Esteve and G. Palau-Salvador P.A. López-Jiménez
Department of Rural Engineering Hydraulic and Environmental
Engineering Department
Polytechnic University of Valencia
Polytechnic University of Valencia
Valencia
Valencia
Spain
Spain
W. Brevis M.O. Vaas
Department of Civil and Structural Engineering Institute for Hydromechanics
The University of Sheffield
Karlsruhe Institute of Technology
Sheffield
Karlsruhe
UK
Germany
Keywords: CFD, Turbulent Mixing, Water Storage Tank, Mixing Parameters.
Abstract
Mixing processes and their related residence times in water storage tanks are
an important factor for maintaining an adequate quality of water. These processes
are normally investigated with costly experimental studies. Furthermore, much has
been achieved in numerical simulation techniques in recent years. The main
objective of this project is to develop a CFD (Computational Fluid Dynamics) model
that could be used as a flexible modelling tool, in addition with experimental
procedures, for the study, design and improvement of these tanks. Mixing and
residence times in a water storage tank are investigated using Unsteady Reynolds
Averaged Navier-Stokes simulations (URANS). A good agreement between the
experimental dilution curve in the outlet section tank and the CFD results was
achieved. The flow structure and its relation to the different phases of the dilution
curve have been studied, proving a predominantly advective transport.
INTRODUCTION
Water storage tanks are important devices in hydraulic networks. They are
designed for several objectives such as keeping water supply constant when water
demand achieves flow peaks. Although the study and modelling of these tanks are often
simplified, the impact of the tanks for maintaining an adequate quality of water in the
network is of paramount importance. Some examples of fatal episodes due to inadequate
management are documented by Bolous et al. (1994) and Clark et al. (1993).
CFD methods can be seen as the best analysis and predictive tool in storage tanks
for water quality studies (Martinez-Solano et al., 2010), since these models can obtain
sufficient spatial and temporary detail of the studied domains. However, storage tanks,
have been normally studied with intensive experimental procedures (Patwardhan, 2002),
in which it is assumed an empirical or statistical relationship between residence times and
either geometrical parameters or hydraulic conditions. Furthermore, Marek et al. (2007)
have pointed out that most of the research in flow and mixing processes in water storage
tanks has been done with extensive and costly experiments. However, there are few CFD
studies applied to this sort of modelling in the literature (Grayman et al., 1996; Hannoun
and Bolous, 1997; Yeung, 2001; Palau-Salvador et al., 2007).

MATERIAL AND METHODS
The prototype used for the simulations is a 1:4 scale laboratory model of a
rectangular, open-top passage-type water storage tank with constant and equal in- and
outflow. Inflow takes place through a circular pipe (inner diameter: 65 mm) as it can be
observed in Fig. 1. After a 40° bend, the pipe ends in a jet nozzle (nozzle diameter: 16.7
mm). Water leaves the tank through a circular pipe (inner diameter: 102 mm), located
close to the inlet pipe (see Table 1 and Fig. 1). Water level is kept constant and no surface
waves were observed during the experiments. The experiment begins with a constant flow
of fresh water (see Table 1). After achieving an equilibrium with a constant level of the
water surface, brine with a salt concentration of 50 gr/l is injected (t=0) during 24 seconds
(the total volume of injected brine is 10 litters).
In this work, three-dimensional simulations are performed on the RANS and
URANS computational techniques by using the STAR-CCM+ commercial code (CD-
Adapco Inc). The numerical results are validated with experimental data which were
carried out at Institute for Hydromechanics, KIT (Karlsruhe). The model is based on the
mass conservation and momentum conservation equations by neglecting the temperature
effects. The code is based on a finite-volume method (see Veersteg and Malalasekera,
1998) for solving the Navier-Stokes equations. For the purpose of mass conservation a
standard pressure correction algorithm (SIMPLE) is used. For the turbulence closure, a
realizable k-e model was used.
For the inlet pipe, a velocity inlet boundary condition was used. For the tank walls
a slip condition was implemented. The free surface was modelled by a rigid-lid
approximation. To perform the steady simulations a RANS simulation was performed and
for the unsteady, URANS simulations were carried out. The initial conditions for the
URANS were fixed by the steady state of the previous RANS solution. A passive scalar
model was used to simulate the brine injection (STAR-CCM+, 2010). Since the purpose
of this work was to simulate mixing processes inside the tank of a brine injection (with
NaCl as the passive scalar), it was considered a variable-density model.
Different kinds of grids were also developed and tested: structured and
unstructured meshes with different grid sizes. After preliminary simulations, the best case
among all of them was T1 (structured middle grid). In order to make this selection, a
sensitivity analysis was carried out taking into account convergence criteria and
simulation time. Therefore, the final grid used for the calculations has 944,542 grid
points. The decrease (stretching near the wall) is kept to a value around 4%.
RESULTS AND DISCUSSION
Calibrated Model and Validation
Figure 2 shows a comparison between experimental and simulated dilution curves
in the outlet cross section of the tank over the first 6,000 seconds. It is possible to observe
that the simulated curve is in good agreement with the experimental results. The
beginning of the first peak of salt concentration, around 80 seconds after the injection, is
fairly good reproduced by the simulation in time and intensity (the numerical results show
a maximum of 1.04 gr/l versus 1.00 gr/l in the experiments). Between the first peak and
until 350 seconds, the model reproduces a sinusoidal behaviour. After that, the
concentration decays linearly to reach the average value of 0.2 gr/l, meaning an
homogeneous mixing of injection, which is fairly good reproduced by the simulation.

Hydrodynamics and Mixing Process
Figure 3 shows the three-dimensional streamlines (coloured by the mean velocity
magnitude,
U
u
2
v
2
w
2
) for T1 simulations. These mean flows results
have been obtained by means of RANS simulations. The flow is high three-dimensional
and complex with no dead-zones or clear short-circuiting, leading to homogeneous
distribution water into the tank. It is possible to observe a significant reduction of velocity
when the jet reaches the opposite corner and how there is clearly a bulk flow circulation
from the entrance to the outlet. It can also be seen two circulations both sides of the jet
and connected above the jet flow.
Figure 4 shows mean velocity contours in section Z=0.111. The mean velocity
magnitude is shown in each of the grid points. Hence, it can be seen clearly the structure
of the flow inside the tank and how the inlet injection influences the velocity patterns. It is
remarkable the acceleration of the simulated flow, which reaches a maximum value of 2
m/s (location: X=1.64; Y=0.25) compared with the mean inlet velocity of 0.126 m/s.
Moreover, when the jet strikes on the opposite corner the velocities are reduced and their
values get closer to the mean velocity within the tank (0.0268 m/s). Regarding to the
streamlines, their pattern shows that there are not any short-circuiting as it was expected.
Although the flow is clearly three-dimensional and complex, it is possible to observe at
section Z=0.111 two main structures both sides of the jet that rotate in anticlockwise
direction. It is also possible to identify a relatively small cell near X=1.1 and Y=1.5 that
rotates in the opposite direction.
The relevant stagnant zones in the tank are plotted in Figure 5. The shown isosurface
is determined by the mean velocity value equal to the 5% of the cumulative
histogram of (0.0056 m/s), representing then the dead zones within the tank. Two
dead zones stand out clearly: one of them seems to occupy the space between the two
aforementioned main recirculation structures and the jet; the other one seems to encircle
the jet in its right side and may correspond with the core of the second main recirculation
formed in that zone. At the same time, there is another remarkable stagnant zone on the
bottom of the tank and very near the opposite corner of the jet nozzle. Such dead zone has
an elongated shape and may be related to the first main recirculation (see section Z=0.111
in Figure 3). Finally, weaker dead zones can be appreciated, related to typical low
velocity zones in tanks such as corners or the free surface, where the transport is limited
by the reduced interchange with the mean flow of the tank (Mau et al., 1995).
After the mean velocity results are discussed, salt concentration computed values
inside the tank are also showed in this section. Figure 6 shows three (1 gr/l, 0.2 gr/l and
0.1 gr/l) iso-surfaces at two different times (13 and 103 seconds since the brine injection),
which were supposed to be characteristic of the dilution curve of this specific mixing
process. Therefore, from the snapshots it can be seen that the mixing process is clearly
affected by the flow on the dispersion pattern of the scalar in the tank, which seems to be
predominantly advective. The 1.00 gr/l iso-surface (at snapshot t=103 seconds) starts
leaving the tank, according to the first peak of the dilution curve (see Fig. 2). This means
that an amount of salt concentrations reaches the outlet before it gets completely mixed.
CONCLUSIONS
In this paper, the results of three dimensional numerical simulations have been
presented for a water storage tank. The paper shows a procedure for the analysis of the
mixing processes in water tanks using experimental and computational techniques.

A good agreement has been achieved between experimental and simulated dilution
curve. The mixing process and its relation to the different phases of the dilution curve
have been studied, showing a predominantly advective transport. The relevant stagnant
zones in the tank were also located and plotted. The results show a good mixing
capability of the prototype, achieving a homogeneous mixing of injection after 350
seconds, with no dead-zones or clear short-circuiting in the flow.
Future research will focus on the extrapolation ability of the technique, being
applied, in addition with experimental procedures, as a predictive tool on the design,
improvement and management of water tanks.
Literature Cited
Bolous, B. F. et al. 1994. A Discrete Simulation Approach for Network Water Quality
Models. J. Water Resour. Plng. and Mgmt, ASCE, vol. 121(1), pp. 49–60.
Clark, R. M. et al. 1993. Effect of the Distribution System on the Water Quality. J.
AQUA, vol. 42(1), pp. 30–38.
Grayman, W.M. et al. 1996. Water Quality and Mixing models for tanks and reservoirs.
J.AWWA, 88(7), 60– 73.
Hannoun, I.A. and Boulos, P.F. 1997. Optimizing Distribution Storage Water Quality: a
Hydrodynamic Approach. Journal of Applied Mathematical Modeling, 21, 495–502.
Marek, M., et al. 2007. CFD Modeling of Turbulent Jet Mixing in a Water Storage Tank.
XXXII IAHR Congress, Venice, Italy).
Martínez-Solano, F. J. et al. 2010. Modelling Flow and Concentration Field In rectangular
Water Tanks. International Congress on Environmental Modelling and Software
Modelling for Environment’s Sake, iEMSs, Fifth Biennial Meeting, Ottawa, Canada.
Mau, R.E. et al. 1995. Explicit Mathematical Models of Distribution Storage Water
Quality. ASCE Journal of Hydraulic Engineering, Vol. 121 (10), pp. 669-709.
Palau-Salvador, G. et al. 2007. Numerical Simulations to Predict the Hydrodynamics and
the Related Mixing Processes in Water Storage Tanks, Proc. IAHR Congress Venice.
Patwardhan, A.W. 2002. CFD Modeling of Jet Mixed Tanks. Chemical Engineering
Science, 57, 1307–1318.
STAR-CCM+ User’s Guide, Version 5.04.006. 2010. CD-Adapco, USA
Veersteg, H.K. and Malalasekera, W. 1998. An Introduction to Computational Fluid
Dynamics. The Finite Volume Method. Longman Scientific and Technical, New
York.
Yeung, H. 2001. Modelling of service reservoirs. Journal of Hydroinformatics, 3(3), 165–
172.
Tables
Table 1. Main Geometrical characteristics and hydraulic conditions of the Tank.
Estimated Residence
Inflow
Geometrical Parameters
Time
Q in
T r
θ φ A B C D E
(l/s)
( h) ( o ) ( o ) (mm) (mm) (mm) (mm) (mm)
0.42 1.58 40 0 150 345 305 150 75
T
r T
Q in
, being
T
Tank Volume

Figures
Fig. 1: Detail of the experimental case used for the simulations: T1 case. Left: top view;
right: side view.
Fig. 2: Concentration in the outlet section (logarithmic scale) for 6,000 seconds from the
injection of the brine: experimental mean value (dotted curve) and the sectional
averaged value for the simulation (continuum line).
Fig. 3: Views of the simulated three-dimensional mean flow field (T1 simulation):
2 2 2
streamlines coloured by the mean velocity magnitude ( U u v w ).

Fig. 4: Horizontal sections of mean flow results (T1 simulation). Left: contours of mean
velocity magnitude U
flow in section Z=0.111.
2
2
2
u v w in section Z=0.111. Right: streamlines of
Fig. 5: Different views of the tank (T1 simulation) showing stagnant zones (5% of the
cumulative histogram of = 0.0056 (m/s)).
Fig. 6: Different views at different specific times (t=13s and t=103s) of the salt
concentration iso-surfaces (1gr/l; 0.2 gr/l and 0.1 gr/l) for T1 simulation.