Get Your Free Goodie Box here

Applied Computational Fluid Dynamics by Hyoung Woo Oh - HTML preview

PLEASE NOTE: This is an HTML preview only and some elements such as links or page numbers may be incorrect.
Download the book in PDF, ePub, Kindle for a complete version.

refinement increases the computational costs (the number of equations to be solved and

the time it takes to compute the entire simulation). If one tends toward the other end of

the model-resolve spectrum models all turbulence of all length and time scales, the

computational costs decrease but one loses accuracy in the simulation. CFD researchers

usually tend to resolve a range of turbulent length and time scales and model the rest.

Usually the range is related to the range of interest of the flow simulation. For instance, if someone is simulating gas dynamics in the inner-ballistics of a particular weapon, it

Computational Fluid Dynamics


would be best to resolve turbulence on the length range of the chamber inside the weapon

and model anything much larger and much smaller. Likewise, any turbulence that occurs

over a longer period than the time it takes to fire the weapon would have smaller effects

on the simulation; it would be best to model turbulence on longer time scales and much

shorter time scales.

The most expensive turbulence scheme is Direct Numerical Simulation (DNS) (32). In DNS,

all length scales of the turbulence are resolved and little or no modeling is done. It is not used in cases of extremely complex geometries which can create prohibitive expense in

resolving the turbulence especially in special geometrically complex portions of the domain.

Less expensive than DNS, the Large Eddy Simulation (LES) resolves turbulence on large

length scales as the name suggests (33). A model is used to represent sub-grid scale effects of turbulence. The computational cost of turbulence at small length scales is reduced through


Reynolds-averaged Navier-Stokes (RANS) is the oldest approach to turbulence modeling

and it is cheaper than LES. It involves solving a version of the transport equations with new Reynolds stresses introduced. This addition brings a 2nd order tensor of unknowns to be

solved as well. Examples of RANS methods are K-ε methods (34), Mixing Length Model

(35), and the Zero Equation model (35).

The Detached-eddy simulation (DES) is a version of the RANS model in which portions of

the grid use RANS turbulence modeling and portions of the grid (or mesh) use an LES

model (36). Since RANS is usually cheaper to implement than LES, DES is usually more

expensive than using RANS throughout the entire domain or grid and usually cheaper than

using LES throughout the entire grid. If the turbulent length scales fit within the grid

dimensions or the particular portion of the grid is near a boundary or wall, a RANS model is used. However, when the turbulence length scale exceeds the maximum dimension of the

grid, DES switches to an LES model. Care must be taken when creating a mesh over which

DES will be used to model turbulence due to the switching between RANS and LES.

Therefore thought must be given to proper refinement to minimize computation while

maximizing accuracy (especially refinement near walls). DES itself does not utilize zonal

functions; there is still one smooth function used across the entire domain regardless of the use of RANS or LES in certain regions.

There are many more turbulence models including the coherent vortex simulation which

separates the flow field turbulence into a coherent part and a background noise part,

somewhat similar to LES (37). Many of the contributions today are coming through different

versions of RANS models.

3.4 Linear algebraic equation system

Once the mathematical equation has been chosen in the pre-processing stage, the mesh has

been partitioned and distributed, and the numerical discretization is chosen and coded, the

last part of the computer program is to solve the resulting algebraic system for the

unknowns. Remember in CFD we are calculating the unknowns (velocity and pressure, for

instance) at all nodes in the domain. The algebraic system usually looks like Ax = b. Usually with many steady problems, Ax is a linear equation system. Therefore we can just invert the

matrix A to find the vector x of unknown values. The problem is that for large

computations, for instance a computation involving 500 million nodes, inverting the matrix

A takes too long. Remember that the number of nodes does not necessarily equal the


Applied Computational Fluid Dynamics

number of unknowns. If you’re calculating 5 unknowns at every node, than you must

multiply the number of nodes by the number of unknowns per node to get the value of

actual number of unknowns and the length of the unknown vector x. So for such large

problems, we solve the equation system iteratively. These systems are solved iteratively

with iterations such as Newton or the Picard iteration.

In many cases with unsteady flows, Ax represents a system of ordinary or partial

differential equations. In this case, CFD researchers must choose either an implicit method

or an explicit method to deal with the time integration. An explicit method calculates the

solution at a later time based on the current solution. Another way to rephrase that is that it calculates the current solution based on an earlier solution in time. An implicit method

calculates the solution at a later time based on both the solution at a later time and the

current solution. Rephrasing that, an implicit method calculates the current solution based

on both the current solution and the solution at an earlier time. Once a method is chosen and the time derivatives have been expanded using an implicit or explicit method, Ax is usually

a nonlinear algebraic system.

As stated earlier, for large problems, it may be too time-consuming or too costly

(computationally) to compute this directly by inverting A. Usually, then, the linear system is solved iteratively as well (38).

One must then choose which type of iterative solver to employ to find the unknown vector.

Depending on the characteristics of this equation system, an appropriate solver is chosen

and employed to solve the system. The major implication of all computational research in

this area is that there is no one perfect iterative solver for every situation. Rather there are solvers that are better for certain situations and worse for others. When operating and

computing with no information about the equation system, there are, however, general

solvers that are quite robust at solving many types of problems though may not be the

fastest to facilitate the specific problem one may be working on at the moment.

A popular class of iterative solvers for linear systems includes Krylov subspace methods of

which GMRES appears to be the most general and robust (38) (39). Its robustness makes it a

great choice for a general solver especially when a researcher has no specific information

about the equation system she is asked to solve. GMRES minimizes residuals over

successively larger subspaces in an effort to find a solution.

Still, in recent years, the Multigrid method has shown better optimal performance than

GMRES for the same problems, motivating many to use this method in place of GMRES.

The Multigrid method minimizes all frequency components of the residual equally

providing an advantage over conventional solvers that tend to minimize high-frequency

components of the residual over low-frequency components of the residual. Operating on

different scales, the Multigrid method completes in a mesh-independent number of

iterations (40) (41).

CFD experts also employ methods to simplify the ability of a solver to solve an algebraic

equation system by pre-conditioning the matrix. The point of preconditioning is to

transform the matrix closer to the identity matrix which is the easiest matrix to invert.

Though we rarely invert matrices for such large problems, matrices that are invertible or

closer to being invertible are also easier to solve iteratively.

Preconditioning is an art, involving the correct choice of preconditioner according to the

type of linear system (just as in choosing the correct solver or iterative method). Examples include lumped preconditioners, diagonal preconditioners, incomplete LU, Conjugate-Gradient, Cholesky or block preconditioners such as block LU or Schwarz (38) (42) (43). The

Computational Fluid Dynamics


best preconditioners are those that take advantage of the natural structure of the algebraic system in order to facilitate the transformation of A to a matrix closer to the identity matrix, thereby facilitating the solving of the system.

The condition number roughly measures at what rate the solution x will change with respect

to a change in b. Low conditions numbers imply more ease in inverting and solving the

system. Characteristics such as condition number and even definite-ness of systems become

important in choosing a preconditioner.

3.5 Libraries

Many CFD programs require thousands of lines of code for one specific simulation. To

avoid writing a different program for every application, researchers often write general

programs and software packages that can be used for a variety of situations. This generality greatly increases the lines of code even more.

To help, there are many CFD and computational solid dynamics (CSD) libraries and applied

mathematics libraries for the solving of such differential equations. They include code libraries such as OFELI (44), GETFEM (45), OOFEM (46), deal.ii (47), fdtl (48), RSL (49), MOUSE (50),

OpenFOAM (51), etc. Sometimes a CFD engineer may use a package like ANSYS Fluent (52) to

do a simulation, and sometimes a CFD researcher may find that the software does not give

him the freedom to do what he would like to do (usually for very specific research

applications). In these cases, he can write his own code or piece code together using these

libraries. The most general Finite Element Library is deal.ii which is written in C++. It contains great support but currently does not support triangles or tetrahedral.

3.6 Moving problems

Moving problems are another class of CFD challenges. One can either use a body-fitted

mesh approach (an approach where the mesh fits around the solid body of interest), an

overlapping mesh method, or a meshless method. Body-fitted mesh methods must actual

move the mesh elements or cells. Overlapping methods have the option of moving the mesh

but capture the movement of interest in the overlapping regions. Meshless methods avoid

the need to move the mesh as moving the mesh has the ability to introduce error. Usually

when a mesh is moving the aspect ratio of the mesh elements must be checked. If the ratio

goes beyond some limit, the mesh must be reordered and remade, and the solution from the

old mesh must be projected to the new mesh in order to continue the simulation. Each of

those steps has the ability to introduce error. Therefore it is best to limit mesh distortion or concentrate it in elements that have the ability to absorb the deformation without reaching

the aspect ratio limit for the computation (7) (53).

There are also numerous methods that avoid meshes. Due to the problems and errors that

poor refinement and mesh distortion introduce, some people avoid mesh methods

altogether. Some meshless methods (54) include spectral methods (55), the vortex method

(meshless method for turbulent flows), and particle dynamics methods (56).

4. Post-processing

This is the final stage when the computations are complete. This involves taking the output

files full of velocity, pressure, density, and similar. information at each node for each time step and displaying the information visually, hopefully with color. Many CFD engineers

also animate the results so as to better show what happens in time or to follow a fluid particle or a streamline.


Applied Computational Fluid Dynamics

4.1 Engineering

Up to this point, all of the work we have spoken about deals with the computer

science/electrical engineering part or the computational and applied mathematics part of

CFD. The mechanical and chemical engineering part of CFD comes in the post-processing

and analysis.

The interpretation of the visualized results is also another point at which error can be

introduced. CFD scientists and engineers must therefore take care in not overextending the

analysis and simultaneously not missing important implications or conclusions that can be

drawn from it. Engineers also make sure to corroborate the results with physical

experiments and theoretical analysis. Additionally, the choice of problem and the

motivation can come from the engineering side of CFD at the very beginning before any pre-

processing work. Finally, the engineering analysis of the phenomenon directs the feedback

loop of the research work. At this point the CFD worker must decide what values to change,

whether it should be run again, what parameters should be maintained at current values,

etc. He must decide which parameters’ effect should be tested. He must determine if the

results make sense and how to properly communicate those results to other engineers,

scientists, scientists outside of the field, lay persons, and policy makers.

CFD work has taken exciting directions and comes to bear in many ways in society. When

the fluid is water, CFD workers study hydrodynamics. When the fluid is air, they study

aerodynamics. When it is air systems, they study meteorology and climate change. When it

is the expanding universe, astronomy and cosmology; blood, medicine; oil and fossil flows,

geology and petroleum engineering. CFD workers work with zoologists studying the

mechanics of bird flight, paleontologists studying fossils, and chemists studying mixing

rates of various gases in chemical reactions and in cycles like the nitrogen cycle.

Because of the importance and presence of fluids everywhere, the interaction of fluids with

structures throughout the real world, and the application of mechanics and chemical

engineering everywhere, CFD remains important. Moreover, the computational tools CFD

engineers use can be utilized to solve and help other computational fields. Since the advent and continual innovation of the computer, all scientific fields have become computational—

computational biology, computational chemistry, computational physics, etc. The same

computational tools used in CFD can often be applied in other areas (predicting the weather

involves a linear algebraic system for instance). This allows CFD engineers and scientists to move in and out of fields and bring their engineering analytical skills and critical reasoning to bear in other situations. CFD engineers and scientists are even used to make video games

and animations look more physically realistic instead of simply artistic (57).

5. Closing

There are a host of other interesting areas in CFD such as two-phase or multi-phase flow

(58), vorticity confinement techniques (similar to shock capturing methods) (59), probability density function methods (60), and fluid-structure interaction (FSI) (61). Other chapters in this book address those, so we will not talk specifically about them here. It is simply

important to understand that as computing capability increases as computer scientists

increase the clock speed of the microchip all the time, our ability to solve real-life problems increases. Problems involving two liquids or two phases occur all the time, and there are

many instances of fluids interacting with deforming solids—in fact that is the general

reality. So combining CFD with computational solid dynamics is an important partnership

that lends itself well to solving the major challenges facing us in the 21st century.

Computational Fluid Dynamics


6. References

[1] Phing, Anselm Ho Yen. Simulating Combustion Flow in a Rocket Chamber. Lulea: Lulea University of Technology, 2008.

[2] A Study of Sharkskin and its Drag Reducing Mechanism. Freidmann, Elfriede, Portl, Julia and Richter, Thomas. Berlin: Springer-Verlag, 2010.

[3] Three-Dimensional Aerodynamic Simulations of Jumping Paratroopers and Falling Cargo Payloads. Udoewa, Victor. 5, Reston, Virginia: AIAA, 2009, Vol. 46. 0021-8669.

[4] Blood Flow in Arteries. Ku, David N. 1, Palo Alto, CA: Annual Reviews, 1997, Vol. 29.

[5] Outflow boundary conditions for three-dimensional finite element modeling of blood flow and pressure in arteries. Vignon-Clementel, Irene E., et al., et al. 29-32, Stanford : Elsevier, 2006, Vol. 195.

[6] Numerical investigation of transitional and weak turbulent flow past a sphere. Tomboulides, Ananias G. and Orszag, Steven A. Cambridge: Cambridge University Press, 2000,

Vol. 416.

[7] Mesh Generation and Update Techniques for 3D Aerodynamic Simulations. Udoewa, Victor. 7, s.l.: Wiley, 2009, Vol. 29.

[8] Slip formulation for numerical simulations of jumping paratroopers. Udoewa, Victor. 7, Johannesburg: Academic Journals, 2009, Vol. 2.

[9] Models and Finite Element Techniques for Blood Flow Simulation. Behr, Marek. s.l.: International Journal for Computational Fluid Dynamics, 2006, Vol. 20.

[10] Sawley, Mark L. Numerical Simulation of the Flow around a Formula 1 Racing Car.

EPFL Supercomputing Review. [Online] November 1, 1997. [Cited: July 13, 2011.]

[11] Computational study of flow around a simplified car body. Guilmineau, Emmanuel. 6-7, Ottowa, Canada: Elevier, 2008, Vol. 96.

[12] Top 500. Top 500 Supercomputing Sites. [Online] Top 500, June 1, 2011.

[Cited: July 13, 2011.]

[13] Salisbury, David F. News Release. Stanford News Service. [Online] November 19, 1997.

[Cited: July 13, 2011.]

[14] MESHPART a Matlab Mesh Partitioning and Graph Separator Toolbox. Cerfacs. [Online]

Cerfacs, February 8, 2002. [Cited: July 13, 2011.]

[15] Karypis, George and Kumar, Vipin. METIS - Unstructured Graph Partitioning and Sparse Matrix Ordering System, Version 2.0. Minneapolis: s.n., 1995.

[16] Karypis, George, Schloegel, Kirk and Kumar, Vipin. PARMETIS - Parallel Graph

Partitioning and Sparse Matrix Ordering. Minneapolis: University of Minnesota,


[17] Applying Parmetis To Structured Remeshing For Industrial CFD Applications. Laflamme, S., et al., et al. 1, s.l.: Spring: International Journal of High Performance Computing

Applications, 2003, Vol. 17.

[18] OpenMP. OpenMP News. OpenMP. [Online] OpenMP, July 9, 2011. [Cited: July 13,



Applied Computational Fluid Dynamics

[19] Pacheco, Peter S. Parallel Programming with MPI. San Francisco: Morgan Kaufmann Publishers, Inc., 1997.

[20] Manticore: A heterogeneous parallel language. Fluet, Matthew, et al. Nice, France: DAMP

2007, ACM 2007, 2007.

[21] NESL: A Parallel Programming Language. Computer Science at Carnegie Mellon

University. [Online] Scandal Lab, August 1, 2005. [Cited: July 13, 2011.]

[22] Kaw, Autar and Kalu, E. Eric. Numerical Methods with Applications. s.l.: Lulu Self-published, 2008.

[23] Oliver, Rubenkonig. The Finite Difference Method (FDM) - An introduction. Freiburg: Albert Ludwigs University of Freiburg, 2006.

[24] Leveque, Randall. Finite Volume Methods for Hyperbolic Problems. Cambridge: Cambridge University Press, 2002.

[25] Huebner, K. H., Thornton, E. A. and Byron, T. D. The Finite Element Method for Engineers.

s.l.: Wiley Interscience, 1995.

[26] Ang, W. T. A Beginner's Course in Boundary Element Methods. s.l.: Universal Publishers, 2007. 978-1581129748.

[27] Beer, Gernot, Smith, Ian and Duenser, Christian. The Boundary Element Method with

Programming: For Engineers and Scientists. s.l.: Springer, 2008. ISBN 978-


[28] The immersed boundary method. Peskin, C. S. s.l.: Acta Numerica, 2002, Vol. 11.

[29] Wesseling, P. Principles of Computational Fluid Dynamics. s.l.: Springer-Verlag, 2001.

[30] Uniformly High Order Accurate Essentially Non-Oscillatory Schemes III. Harten, A., et al., et al. s.l.: Journal of Computational Physics, 1987, Vol. 71.

[31] The Piecewise parabolic Method (PPM) for Gasdynamical Simulations. Colella, P. and Woodward, P. s.l.: Journal of Computational Physics, 1984, Vol. 54.

[32] Pope, S. B. Turbulent Flows. Cambridge : Cambridge University Press, 2000. ISBN 978-0521598866.

[33] Garnier, E., Adams, N. and Sagaut, P. Large eddy simulation for compressible flows. s.l.: Springer, 2009. 978-90-481-2818-1.

[34] The Numerical Computation of Turbulent Flows. Launder, B. E. and Spalding, D. B. 2, s.l.: Computer Methods in Applied Mechanics and Engineering, 1974, Vol. 3.

[35] Wilcox, David C. Turbulence Modeling for CFD (3 ed.). s.l.: DCW Industries, Inc., 2006.


[36] Comments on the feasibility of LES for wing and on a hybrid RANS/LES approach. Spalart, P.

R. Arlington, TX: 1st ASOSR CONERFENCE on DNS/LES, 1997.

[37] Coherent Vortex Simulation (CVS), A Semi-Deterministic Turbulence Model Using Wavelets.

Farge, Marie and Schneider, Kai. 4, s.l.: Flow Turbulence and Combustion, 2001,

Vol. 66.

[38] Saad, Y. Iterative Methods for Sparse Linear Systems, 2nd edition. s.l.: SIAM, 2003. ISBN 978-0-89871-534-7.

[39] GMRES: A generalized minimal residual algorithm for solving nonsymmetric linear systems.

Saad, Y. and Schultz, M. H. s.l.: SIAM Journal of Scientific and Statistical

Computing, 1986, Vol. 7.

Computational Fluid Dynamics


[40] Wienands, Roman and Joppich, Wolfgang. Practical Fourier analysis for multigrid methods.

s.l.: CRC Press, 2005. 1584884924.

[41] Trottenberg, U., Oosterlee, C. W. and Schüller, A. Multigrid. s.l.: Academic Press, 2001.

ISBN 012701070X.

[42] Trefethen, Lloyd N. and Demmel, James W. Numerical Linear Algebra. s.l.: SIAM, 1997.


[43] Golub, Gene H. and Van Loan, Charles F. Matrix Computations 3rd Edition. s.l.: John Hopkins University Press, 1996. 0801854148.

[44] OFELI. OFELI An Object Oriented Finite Element Library. OFELI. [Online] OFELI, June 1, 2011. [Cited: July 13, 2011.]

[45] Renard, Yves; Pommier, Julien. GETFEM++. GNA. [Online] GETFEM, June 1, 2010.

[Cited: July 13, 2011.]

[46] OOFEM. OOFEM - free object oriented finite element solver. OOFEM. [Online]

OOFEM, March 29, 2011. [Cited: July 13, 2011.]

[47] Dealii. Dealii Homepage. Dealii. [Online] Dealii, January 9, 2011. [Cited: July 13, 2011.]

[48] Google. FDTL - Finite Difference Template Library. FDTL. [Online] Google, June 2, 2011. [Cited: July 13, 2011.]

[49] Michalakes, John. A Runtime System Library for Parallel Finite Difference Models with

Nesting. Argonne National Laboratory. [Online] May 18, 1995. [Cited: July 13, 2011.]

[50] MOUSE team. MOUSE. USASK. [Online] University of Duisburg, January 7, 2010.

[Cited: July 13, 2011.]

[51] OpenFOAM. OpenFOAM - The Open Source CFD Toolbox. OpenFOAM. [Online]

OpenFOAM, June 2, 2011. [Cited: July 13, 2011.]

[52] Ansys. Features of Ansys Fluent. Ansys. [Online] Ansys, June 3, 2011.

[Cited: July 13, 2011.]


[53] Huang, Weizhang and Russell, Robert D. Adaptive Moving Mesh Methods. s.l.: Springer, 2011. 978-1-4419-7915-5.

[54] Liu, G. R. Mesh Free Methods, 2nd ed. s.l.: CRC Press, 2009. 978-1-4200-8209-9.

[55] Hesthaven, J., Gottlieb, S. and Gottlieb, D. Spectral methods for time-dependent problems.

Cambridge: Cambridge University Press, 2007.

[56] Belytschko, T. and Chen, J.S. Meshfree and particle methods. s.l.: John Wiley and Sons, Ltd., 2007. 0-470-84800-6.

[57] Gourlay, Michael J. "Fluid Simulation for Video Games". s.l.: Intel Software Network, 2009.

[58] Two phase flow in complex systems. Levy, Salomon. s.l.: Wiley, 1999.

[59] Numerical Simulation of Vortical Flows Using Vorticity Confinement Coupled with

Unstructured Adaptive Grid Refinement. Murayama, M. and Kato, T. 1, s.l.:

Computational Fluid Dynamics Journal, 2001, Vol. 10.


Applied Computational Fluid Dynamics

[60] Fox, Rodney. Computational methods for turbulent reacting flows. Cambridge: Cambridge University Press, 2003. 978-0-521-65049-6.

[61] FOIST: Fluid–object interaction subcomputation technique. Udoewa, V. 9, s.l.: Wiley: Communications in Numerical Methods in Engineering, 2009, Vol. 25.


A Computational Fluid Dynamics Model of

Flow and Settling in Sedimentation Tanks

Ali Hadi Ghawi1 and Jozef Kriš2

1Department of Civil Engineering, Faculty of Civil Engineering, AL-Qadisyia University

2Department of Sanitary and Environmental Engineering, Faculty of Civil Engineering,

Slovak University of Technology, Bratislava



1. Introduction

Sedimentation is perhaps the oldest and most common water treatment process. The

principle of allowing turbid water to settle before it is drunk can be traced back to ancient times. In modern times a proper understanding of sedimentation tank behavior is

essential for proper tank design and operation. Generally, sedimentation tanks are

characterized by interesting hydrodynamic phenomena, such as density waterfalls,

bottom currents and surface return currents, and are also sensitive to temperature

fluctuations and wind effects.

On the surface, a sedimentation tank appears to be a simple phase separating device, but

down under an intricate balance of forces is present. Many factors clearly affect the

capacity and performance of a sedimentation tank: surface and solids loading rates, tank

type, solids removal mechanism, inlet design, weir placement and loading rate etc. To

account for them, present-day designs are typically oversizing the settling tanks. In that

way, designers hope to cope with the poor design that is responsible for undesired and

unpredictable system disturbances, which may be of hydraulic, biological or physico-

chemical origin.

To improve the design of process equipment while avoiding tedious and time consuming

experiments Computational Fluid Dynamics (CFD) calculations have been employed during

the last decades. Fluid flow patterns inside process equipment may be predicted by solving

the partial differential equations that describe the conservation of mass and momentum. The

geometry of sedimentation tanks makes analytical solutions of these equations impossible,

so usually numerical solutions are implemented using Computational Fluid Dynamics

packages. The advent of fast computers has improved the accessibility of CFD, which

appears as an effective tool with great potential. Regarding sedimentation tanks, CFD may

be used first for optimizing the design and retrofitting to improve effluent quality and

underflow solids concentration. Second, it may increase the basic understanding of internal

processes and their interactions. This knowledge can again be used for process optimization.

The latter concerns the cost-effectiveness of a validated CFD model where simulation results can be seen as numerical experiments and partly replace expensive field experiments

(Huggins et al. 2005).


Applied Computational Fluid Dynamics

Generally, many researchers have used CFD simulations to describe water flow and solids

removal in settling tanks for sewage water treatment. However, works in CFD modelling of

sedimentation tanks for potable water treatment, rectangular sedimentation tanks, and iron

removal by sedimentation tank in surface and groundwater treatment plants have not been

found in the literature. Moreover, the physical characteristics of the flocs may not be such significant parameters in the flow field of sedimentation tanks for potable water, due to the much lower solids concentrations and greater particle size distributions than those

encountered in wastewater treatment.

Design of sedimentation tanks for water and wastewater treatment processes are often

based on the surface overflow rate of the tank. This design variable is predicated on the

assumption of uniform unidirectional flow through the tank. Dick (1982), though, showed that many full-scale sedimentation tanks do not follow ideal flow behavior because

suspended solids removal in a sedimentation tank was often not a function of the overflow

rate. Because of uncertainties in the hydrodynamics of sedimentation tanks, designers

typically use safety factors to account for this nonideal flow behavior (Abdel-Gawad and

McCorquodale, 1984).

It can be concluded from the discussion that the current ways in which STs are designed and

modified could and should be improved. Providing a tool that might lead to sedimentation

tank optimization, as well as understanding, quantifying and visualizing the major

processes dominating the tank performance, are the main goals of this research.

2. Scope and objectives

This research focuses on the development of a CFD Model that can be used as an aid in the

design, operation and modification of sedimentation tanks (Ghawi, 2008). This model

represents in a 2D scheme the major physical processes occurring in STs. However, effect of

scrapers and inlet are also included, hence the CFD Model definition. Obviously, such a

model can be a powerful tool; it might lead to rectangular sedimentation tanks optimization, developing cost-effective solutions for new sedimentation projects and helping existent

sedimentation tanks to reach new-more demanding standards with less expensive

modifications. An important benefit is that the model may increase the understanding of the

internal processes in sedimentation tanks and their interactions. A major goal is to present a model that can be available to the professionals involved in operation, modification and

design of sedimentation tanks.. The ultimate goal of the project is to develop a new CFD

methodology for the analysis of the sediment transport for multiple particle sizes in full-

scale sedimentation tanks of surface and groundwater potable water treatment plants with

high iron concentration. The CFD package FLUENT 6.3.26 was used for the case study of the

effect of adding several tank modifications including flocculation baffle, energy dissipation baffles, perforated baffles and relocated effluent launders, were recommend based on their

field investigation on the efficiency of solids removal. An overview of the outline of the

project is given in Figure 1.

The specific objectives of this research include:

Improve the operation and performance of horizontal sedimentation tank in Iraq which

have been identified as operating poorly, by predicting the existing flow, coagulant

dose to remove iron and flocculent concentration distribution of the sedimentation tank

by means of CFD techniques.

Develop a mathematical model for sedimentation tanks in 2D;

A Computational Fluid Dynamics Model of Flow and Settling in Sedimentation Tanks


Introduce a flocculation submodel in the general ST model,

Introduce a temperature submodel in the general ST model.

Design CFD model for simulation of sedimentation tanks, i.e. grids and numerical


Develop a model calibration procedure, including the calibration of the settling

properties, and validate the models with experimental data.

Evaluate the suitability of CFD as a technique for design and research of rectangular

sedimentation tanks for drinking water treatment plants and iron removal.

Use CFD to investigate the effects of design parameters and operational parameters.

Retrofit and

Improvement of

Settling Tanks







 Cogulation Doses

2D-Settling Tank


 pH

 Cogulation Doses


 Temperature

 pH



 Particles Size Distribution

Prediction of Velocities, Temperature,


 Temperature

Iron and Solids Concentration Profiles

 Iron


 Manganese

 Settling Velocity

 SS

 SS


 Solids Concentrations





Fig. 1. Overview of the settling tank project

Finally, a CFD model was developed to simulate the full scale rectangular sedimentation

tanks at the AL-DEWANYIA purification works in Iraq. The CFD simulations of the AL-

DEWANYIA tanks were done by setting up standard cases for each, i.e. a configuration and

operating conditions that represented the physical tanks as they were built, and then

varying different aspects of the configuration or operating conditions one or two at a time to determine the effect. discrete particles in dilute suspension was simulated, as it is the

applicable type for the operating conditions in rectangular sedimentation tanks for potable

water treatment.

3. Modelling the settling tank

Figure 2 shows the set-up of the settling tank CFD model which developed in this work. The

code predicts fluid flow by numerically solving the partial differential equations, which

describe the conservation of mass and momentum. A grid is placed over the flow region of

interest and by applying the conservation of mass and momentum over each cell of the grid


Applied Computational Fluid Dynamics

sequentially discrete equations are derived. In the case of turbulent flows, the conservation equations are solved to obtain time-averaged information. Since the time-averaged

equations contain additional terms, which represent the transport of mass and momentum

by turbulence, turbulence models that are based on a combination of empiricism and

theoretical considerations are introduced to calculate these quantities from details of the

mean flow.

Equation solved on mesh


. Mesh

. Solid

Transport equation



. Mass

Physical model

. Species mass fraction

. Turbulence (k-e Model)

. Phases volume fraction

. DPM (Lagrangian Model)


. Momentum

. Phases change


. Energy

. Moving mesh

Equation of State

. Post-Processing

Supporting physical Models

. Velocity

. Concentration

. Temperature

. Dimensions

. Material properties

. Efficiency

. Boundary conditions

. Initial conditions

Fig. 2. CFD model

4. Numerical techniques used in Fluent

This section will shortly deal with the methods applied in (Ghawi, 2008). The Fluent software utilises the finite volume method to solve the governing integral equations for the conservation of mass and momentum, and (when appropriate) for scalars such as

turbulence and solids concentration. In the work (Ghawi, 2008), the so-called segregated

solver was applied; its solution procedure is schematically given in Figure 3. Using this

approach, the governing equations are solved sequentially, i.e. segregated from one another.

Because the governing equations are non-linear (and coupled), several iterations of the

solution loop must be performed before a converged solution is obtained.

Concerning the spatial discretisation, the segregated solution algorithm was selected. The

k-ε turbulence model was used to account for turbulence, since this model is meant to describe better low Reynolds numbers flows such as the one inside our sedimentation

tank. The used discretisation schemes were the simple for the pressure, the PISO for the

pressure-velocity coupling and the second order upwind for the momentum, the

turbulence energy and the specific dissipation. Adams and Rodi 1990 pointed out that for real settling tanks the walls can be considered as being smooth due the prevailing low

A Computational Fluid Dynamics Model of Flow and Settling in Sedimentation Tanks


velocities and the correspondingly large viscous layer. Consequently, the standard wall

functions as proposed by Launder and Spalding 1974 were used. The water free surface

was modeled as a fixed surface; this plane of symmetry was characterized by zero normal

gradients for all variables

Update properties, e.g. p

Solve numerical equations (u. v velocity)

Solve pressure-correction (continuity) equation

Update pressure, face mass flow rate

Solve turbulence and scalar equations




Update solution values with converged values at current time

Requested time steps completed?

Take a time step




Fig. 3. Solution procedure

5. Experimental techniques for model calibration and validation

The process of developing (incl. calibration), verifying, and validating a CFD code requires the use of experimental, theoretical and computational sciences. This process is a closed loop as presented in Figure 4.

The above clearly indicates that good experimental data are indispensable for settling tank

model validation; their quality largely depends on the applied experimental technique.

For the purposes of testing the numerical model presented in this thesis on a full scale tank, the data set gathered laboratories, was selected. Here, a comprehensive experimental study

of a working settling tank at AL-DEWANYIA in Iraq were carried out. Velocity and

concentration profiles were gathered at 7 stations along the length and 3 stations across the width of the tank for a variety of inlet conditions and inlet and outlet geometries.

Volumetric flow rates through the inlets and outlets were measured for each test condition

studied. Details of the tank geometry and the experimental conditions for which 3D

numerical simulations have been made are given in next sections. The following topics are

dealt with which measured in the sites:



Applied Computational Fluid Dynamics

Flow rate, (2) Settling velocity, (3) Solids concentration ( Turbidity), Iron, and Manganese, (4) Particle size distribution, (5) Velocity of liquid, and (6) Temperature