Content uploaded by Yaseen Aziz

Author content

All content in this area was uploaded by Yaseen Aziz on Oct 27, 2020

Content may be subject to copyright.

ZANCO Journal of Pure and Applied Sciences

The official scientific journal of Salahaddin University-Erbil

ZJPAS (2018),30 (5); 131-139

http://dx.doi.org/10.21271/ZJPAS.30.5.11

CFD Modeling of Simultaneous Flow Over Broad Crested Weir and Through Pipe

Culvert using Different Turbulence Models

Othman K. Mohammed1, Yaseen W. Aziz2

1- Department of Civil Engineering, College of Engineering, Salahaddin University-Erbil

2- Department of Dams and Water Resources Engineering, College of Engineering, Salahaddin University-Erbil

1. INTRODUCTION

In the case of culvert overtopping with water,

where the culvert cross sectional area is

insufficient to drain the incoming flood, the

ordinary solution is either to replace the old

culvert with a bigger capacity one or to add new

vents to the original one. An alternative solution is

to use a hydraulic structure (broad crested weir with

circular opening). In this case a part of the flow

will go through the culvert vents (circular

openings) and the rest will overtop it. (Mahmoud

S. M. 2002) and (Negm A. M. 2002) conducted

an experimental investigation on simultaneous

flow through box culvert and over contracted

broad crested weir. The flow at the culvert

outlet is considered as submerged flow, a

discharge prediction models have been

developed by means of multiple linear

regression techniques. (Othman K. Mohammed

2010) simulated experimentally the combined

flow through pipe culvert and over broad

crested weirs of different side slopes, he

developed empirical relations between the

discharge coefficient and geometrical

parameters of the combined weir culvert

model. Due to high cost in construction of the

physical models (Kositgittiwong, 2012). . In

addition, because of the difficulties in solving

the high order partial differential equations of

many fluid flow (Aziz, 2016). Nowadays, most

researchers turn to the use of numerical

methods. (Sarker and Rhodes 2004) compared

the free surface profile over a laboratory

rectangular broad crested weir with numerical

CFD model using commercial software

FLUENT applying both slandered k – ε model

and (RNG) k – ε model, they reported that the

A R T I C L E I N F O

A B S T R A C T

Article History:

Received: 05/04/2018

Accepted: 10/09/2018

Published:28/10/2018

Culverts and broad crested weirs are hydraulic structures that could be used

for measuring the flow rate in open channels. In this research, a simultaneous

flow over broad crested weir and through pipe culvert was simulated using

the numerical software ANSYS CFX. Three turbulence models were used for

the modeling of flow turbulent to determine the best turbulence model for

combined flow simulation. To achieve this purposes, results of simulations

have been compared with data gathered from lab experiments from literature.

The computational results showed a close agreement with obtained

experimental data, but that of the (RNG) k – ε model provides more accurate

results compared with other two turbulence models used in this study.

Therefore, it can be concluded that this turbulence model (RNG) k – ε model

can be used for simulation of simultaneous flow over broad crested weir and

below through culverts.

Keywords:

Broad Crested Weir

CFD Modeling

Simultaneous Flow

Turbulence Models

ANSYS CFX

Corresponding Author:

Othman K. Mohammed

othman.mohammed@su.edu.krd

132 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139

uncertainties in predicting the water levels

above and D/S the crest were higher compared

to the wave-like profile observed in the

laboratory experiments. (Hargreaves D. M.

2007) conducted a serious of CFD simulations

using version 6.2 of FLUENT, for predicting

free surface profiles over broad crested weir,

they used the experimental data of (Hager W.

and Schwalt M. 1994) to verify the validity of

the computational code in prediction the

position of free surface profile, velocity and

pressure distributions for different flow rates.

(Afshar, H. and Hoseini, H. 2013) used CFD

together with laboratory model in order to

simulate the flow over rectangular broad-

crested weir. Simulations were performed

using three turbulence models of the RNG k–ε,

standard k–ε and the large eddy simulation

(LES) to find the water level profile and

streamlines. Their results indicated that RNG

model has lowest error compared with the

other models. (S. Hoseini, S. Jahromi and M.

Vahid 2013) used ANSYS FLUENT V.14

together with laboratory model for determining

the discharge coefficient of the rectangular

broad-crested side weir located on the

trapezoidal channel, they found that both

results of CFD and physical model showed that

Cd coefficient decreases with increasing values

of Fr and Cd coefficient increases with

increasing values of Re. (Hoseini S. H. 2014)

simulated the free surface flow over the

triangular broad-crested weir using FLOW 3D.

The simulation results were found in

reasonable agreement with experimental

observations. (Jalil, Shaker and Qasim, Jihan

2016) used FLOW-3D and HEC-RAS

software’s to predict the free surface profile of

Flow over Single-Step Broad- Crested Weir,

they found that HEC-RAS has limited ability to

produce curved profiles past vertical faces,

while FLOW-3D produced more accurate

results. (Al-Hashimi A. S. 2017) used Fluent

Software to compare four different turbulence

models accuracy in computing free surface

flow over broad crested weir and stepped weir

with rounded corner. Results are compared

with the experimental data and showed that the

predictions provided by the standard k–ε model

are closer to the experimental data, whereas

those obtained from the standard k–ω model

deviate the most. As found from literature

survey that the characteristics of flow over

broad crested weir along with the development

of CFD codes have attracted the attention of

many investigators. In this study, the flow

characteristics through Combined Pipe Culvert

and Broad Crested Weir were investigated

using ANSYS-CFX 14. The results of the

numerical model were compared with the

experimental data of (Othman K. Mohammed

2010).

2. THEORETICAL ANALYSIS

Computational Fluid Dynamics (CFD) involves

the solution of the equations of fluid flow (in a

special form) over a region of interest, with

specified (known) conditions on the boundary

of that region. The set of the governing

equations of fluid flow which are solved by

ANSYS-CFX are the Reynold average Navier-

Stokes equations. The governing equations of

continuity and momentum for incompressible

flow can be written as:

Where:

ρ = fluid density,

= average velocity in x

and y directions, x and y = space dimensions, t

= time, P = the pressure, µ =µo + µt , µo is

dynamic viscosity and µt is turbulence

133 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139

viscosity, gi = acceleration due to gravity and

= the body force.

The suffices i and j indicate that the stress

component acts in the j-direction on a surface

normal to the i-direction. (Versteeg H. K. and

Malalasekera W. 2007)

ANSYS-CFX code uses finite volume method

to convert governing equations to algebraic

equation in order to be solved numerically. The

Naiver - Stokes equations with time average

velocity called Reynolds averaged Naiver –

Stokes (RANS) equations. since the Navier-

Stokes equations are non-linear, it is difficult to

solve them analytically especially for turbulent

flow. Because the size of the computational

cells should be smaller than the length scale of

the smallest turbulent this is impossible which

cannot be achieved in many cases (Versteeg H.

K. and Malalasekera W. 2007).

Turbulent models have been classified based

on the application of their design and number

of differential equations to create relation

between turbulence stresses and averaged rates

or their gradients. Among these models, two-

equations model for modeling turbulence with

RANS equations have been used, one-layer

model such as k – ε and (RNG) k – ε and two-

layer model such as shear stress transport

(SST).

2.1. Standard k – ε model:

This model expresses the turbulent

viscosity in terms of turbulent kinetic energy

(k) and its dissipation rate (ε). The following

two transport partial differential equations are

solved for the values of k and ε (Launder and

Spalding 1974):

The eddy viscosity µt is written as follows

Model constants: C1ε = 1.44, C2ε = 1.92, Cµ

=0.09, σk =1.0, and σε =1.3.

2.2. Renormalization Group (RNG) k – ε

model (Choudhury D. 1993):

The (RNG) k-ε turbulence model is derived

from the instantaneous Navier-Stokes

equations, from using a mathematical

technique called, “renormalization group"

(RNG) methods. The analytical derivation

results in a RNG model with constants

different from those in the standard k-ε model

and additional terms and functions in the

transport equations for k and ε.

134 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139

In above Equations, C1ε, C2ε, and Cµ are

constants and equal to 1.42, 1.68, and 0.0845,

respectively. ak and aɛ equal to 1.393, ηo equal

to 4.38, µεff equal to 1 and β equal to 0.012.

2.3. Shear Stress Transport (SST) model

(Menter FR, 1994):

Menter (1994) developed the SST turbulence

model to blend effectively the robust and

accurate formulation of the k- ω model in the

near-wall region with the free stream

independence of the k- ω model in the far field.

It is an eddy-viscosity model which includes

two main novelties:

It is combination of a k-ω model (in the

inner boundary layer) and k-ε model (in the

outer region of and outside of the boundary

layer);

A limitation of the shear stress in adverse

pressure gradient regions is introduced.

The transport equations and effective viscosity

are modelled in SST k-ω model, by the

following equations:

α* damps the turbulent viscosity causing a low

Reynolds number correction

, is the generation of and

F1, F2 are the blending functions

, represent the dissipation of and due

to turbulence

3. EXPERIMENTAL DATA

The experimental data (Table 1) used for the

comparisons were taken from laboratory tests

conducted by (Othman K. Mohammed 2010).

The geometry and dimensions of the combined

broad crested weir and pipe culvert model are

stated in Fig. (1). The experiments were

conducted in a horizontal research flume with a

width of 0.5 m, a height of 0.5 m and a total

length of 12 m. the laboratory model was made

of concrete box shape like of dimensions (50 x

50 x 13.1 cm), containing a plastic pipe 10.6

cm diameter. The notations in this paper are

kept identical to those defined by (Othman K.

Mohammed 2010).

135 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139

Table 1, Experimental data.

Run

H/P

Q l/sec

Cd

1

0.180

10.780

0.526

2

0.240

12.360

0.521

3

0.310

15.140

0.542

4

0.400

17.950

0.527

5

0.480

21.620

0.531

6

0.510

22.720

0.535

7

0.560

24.900

0.53

8

0.590

28.270

0.569

9

0.760

37.010

0.566

10

0.930

47.350

0.575

Fig. (1) Geometry of the tested Model D = 10.6 cm,

P = 13. 1cm, L = 50 cm

4. NUMERICAL MODELLING

The numerical model was constructed at the

same dimensions as the physical model. This

allows direct comparison of the predicted

results with physical model results.

4.1. Mesh Design

Meshing is an important step to solve the

hydraulic systems in numerical modelling.

According to earlier studies, the smaller the

mesh size the greater is the accuracy and the

more is the computational time (Aziz, Y. W.

2016). ANSYS ICEM was used for mesh

generation as it contains many methods for

mesh generation. In this study the Multi-zone

method was used with the maximum and

minimum mesh size of 0.05 m and 0.000196 m

respectively such as mesh sizes used by (Aziz,

Y. W. 2016), and the hexahedron mesh type

was provided as shown in Fig. (2).

Fig. (2) Meshing and its Distribution

4.2. Boundary conditions

ANSYS-CFX contains several boundary

conditions including inlet, outlet, opening and

wall. Fig. (3). Inlet boundary condition

imposed at inlet section with the average

velocity, water and air volume fraction. Static

pressure used at the outlet and opening

boundary condition was specified for the top of

the fluid domain. On the walls, the no slip wall

boundary condition was applied; that is the

fluid velocity next to the wall immediately is

equal to zero. Walls were assumed to be

smooth, since the channel sides were made

from glass.

136 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139

Fig. (3) Boundary conditions

5. RESULTS AND DISCUSSION

To have access to an appropriate turbulence

model for the simulation, the numerical model

is examined with different models of

turbulence such as standard k – ε model, RNG

k – ε model and SST model under the same

conditions (boundary condition, material, mesh

and so on). Then the results of these turbulence

models are compared with those provided by

the experimental data

The experimental and numerical results of

discharge through combined broad crested weir

and pipe culvert were plotted as shown in Fig.

(4). The results for all turbulence models with

the experimental data are very close to each

other, but some of them are in closer agreement

to the experimental data as presented in table 1.

Fig. (4) Comparison of QCFD with QExp for Combined

Weir and Culvert

Slight deviations are observed between the

predicted by numerical model and the

measured values from Fig. (4)

Fig. (5) shows the 3D and longitudinal section

at the center line of the simulated velocity

distribution through the culvert and over the

weir predicted by the k- ɛ turbulence model for

discharge flow rate of 28.27 l/s. Since from the

experiment there is no any measurement of

velocity, so the comparion with the CFD

modelling can not be done.

10

20

30

40

50

10 20 30 40 50

Q CFX

l/sec

Q exp

l/sec

k- ɛ

RNG k- ɛ

SST

137 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139

Fig. (5) Velocity distribution through combined structure

for discharge 28.27 (l/sec) using k-ε turbulence model.

Table (2) shows that discharge coefficient

results obtained from SST turbulence are

mostly closer than the other models to the

experimental data. Further, it can be observed

that the RNG k- ɛ turbulence model performs

better than k- ɛ model. In addition, k- ɛ has

lesser agreement with the experimental data as

it has higher error percentage.

Table (2) Discharge coefficient and relative error of the

numerical simulations

Exp.

CFX

Standard k- ɛ

RNG k- ɛ

SST

Cd

Cd

Error

%

Cd

Error

%

Cd

Error

%

0.526

0.521

1.018

0.519

1.267

0.521

0.939

0.521

0.514

1.433

0.512

1.742

0.513

1.541

0.542

0.554

2.163

0.552

1.849

0.552

1.934

0.527

0.525

0.391

0.525

0.468

0.525

0.288

0.531

0.542

2.079

0.539

1.468

0.542

2.064

0.535

0.539

0.840

0.535

0.023

0.538

0.564

0.53

0.539

1.658

0.533

0.554

0.535

0.888

0.569

0.565

0.675

0.560

1.536

0.562

1.280

0.566

0.565

0.202

0.565

0.263

0.565

0.188

0.575

0.566

1.625

0.563

2.064

0.566

1.582

Discharge coefficients Resulted from Applying

turbulent models together with experimental

values plotted against relative upstream water

depth (H/P) are shown in Fig. (6). In this figure

H and P stand for the head of water above the

weir and weir height respectively. It can be

seen that, for all cases Cd increased with (H/P)

increasing this is due to increase the ratio of

(Flow cross sectional Area/Contracted

parameter).

Fig. (6) Head-discharge coefficient of the numerical

simulations and Experimental data

In order to determine the accuracy of the

simulation results, the Relative Error percent

(E %) of the experimental and the numerical

discharge results are calculated using the

equation:

Table (3) Relative Errors of the average discharge

coefficient

Exp.

CFX

Standard k- ɛ

RNG k- ɛ

SST

Cd

Cd

Error

%

Cd

Error

%

Cd

Error

%

0.542

0.543

1.208

0.540

1.123

0.542

1.127

0.5

0.52

0.54

0.56

0.58

0.1 0.3 0.5 0.7 0.9 1.1

Cd

H/P

exp.

k- ɛ

RNG k- ɛ

SST

138 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139

Errors for discharge coefficient Resulting from

applying different turbulent models are shown

in Fig. (7).

Fig. (7) Discharge coefficient and their Relative Errors

from Applying Different Turbulent Models

It can be seen that (Fig 6 and Fig 7) the results

of k- ε turbulence model for discharge

coefficient are greater than those obtained by

experiments, but those of both (RNG) k – ε and

SST are lower than experimental results. From

table (3) it is clear that higher percentage error

obtained by using k – ε turbulence model,

while using RNG k – ε has lower average

percentage error with the experimental data.

These differences can be clearly seen in charts

shown in Fig. (7).

6. CONCLUSIONS

In the present study, flow over broad crested

weir combined with the circular culvert is

simulated using ANSYS – CFX. The

sensitivity of the results obtained from CFD

modeling of different turbulence models is

examined, to determine the turbulence model

that gives accurate predict of flow through the

combined structure. The summery of the

results of this study can be defined as follows:

1) SST model perform much better has the

maximum accuracy in comparison with

other turbulence models for most

discharges values, but for average relative

percentage error, (RNG) k- ε has a bit

greater accuracy than SST.

2) The results of k- ε have less accuracy

compared with other turbulence models.

3) The discharge coefficient in all methods

slightly increased with upstream relative

head (H/P) which was (from 0.526 to

0.575) such variation may be considered as

constant, same conclusion indicated by

(Hager W. and Schwalt M. 1994) for broad

crested weir flow.

4) It is also concluded that, such type of

software is useful to study the number of

fluid flow problems without going for

expensive and time consuming

experiments.

REFERENCES

Afshar, H. and Hoseini, H. "Experimental and 3D Numerical

Simulation of Flow over a Rectangular Broad-Crested

Weir". International Journal of Engineering and

Advanced Technology (IJEAT) August 2013, Volume-2,

Issue-6, 214-219.

Al-Hashimi A. S., Madhloom M. H., and Nahi N. T.

"Experimental and Numerical Simulation of Flow Over

Broad Crested Weir and Stepped Weir using Different

Turbulence Models", Journal of Engineering and

Sustainable Development Vol. 21, No. 02, March 2017.

Aziz, Y. W. "Evaluation of Hydraulic Performance of

Nazanin Dam Side Channel Spillway" MSc Thesis,

College of Engineering Salahaddin University Erbil

2016.

Choudhury D., (1993). "Introduction to the Renormalization

Group Method and Turbulence Modeling", Fluent Inc.

Technical Memorandum TM-107.

Duangrudee and Kositgittiwong "Validation of Numerical

Model of the Flow Behavior through Smooth and

Stepped Spillways using Large-scale Physical Model"

PhD Thesis, Faculty of Engineering, King Mongkut’s

University of Technology Thonburi 2012.

Duru, Aysel "Numerical Modelling of Contracted Sharp

Crested Weirs" MSc Thesis, School of Natural and

Applied Sciences of Middle East Technical University,

2014

0.0

0.2

0.4

0.6

0.8

1.0

1.2

1.4

Standard k- ɛ RNG k- ɛ SST

Exp.

CFX

E%

139 Mohammad O and Aziz Y /ZJPAS: 2018, 30(5): 131-139

Hager W. H. and Schwalt M. "Broad-crested weir", Journal

of Irrigation and Drainage Engineering, Vol. 120, No. 1,

(1994), pp.13-26.

Hargreaves D. M., Morvan H. P. and Wright N. G.

"Validation of the Volume of Fluid Method for Free

Surface Calculation: The Broad-Crested Weir",

Engineering Applications of Computational Fluid

Mechanics Vol. 1, No. 2, pp. 136–146 (2007)

Hoseini, S.H. "3D Simulation of Flow over a Triangular

Broad-Crested Weir", Journal of River Engineering,

2(2), 1-7 (2014).

Jalil, Shaker & Qasim, Jihan. (2016). “Numerical Modelling

of Flow over Single-Step Broad- Crested Weir Using

FLOW-3D and HEC-RAS”. Polytechnic General

Sciences Journal/ Erbil Polytechnic University. 6. 435-

448.

Launder, B. E., and Spalding, D. B. “The numerical

computation of turbulent flows.” computer methods in

applied mechanics and engineering 3 (1974) 269-289.

Mahmoud S. M. "Characteristics and Prediction of

Simultaneous Flow Over Broad-Crested Weirs and

Through Culverts", EJEST, Vol, 6, No.1, January 2002

Menter FR (1994). "Two-equation eddy viscosity turbulence

models for engineering applications". AIAA Journal

32(8):1598-1605.

Negm A. M. “Analysis and modeling of simultaneous flow

through box culverts and over contracted broad-crested

weirs” Proc. of 5th International Conference on Hydro-

science and Engineering. ICHE2002. Sept. 18- 21.

Warsaw, Poland.

Othman K. Mohammed "Flow Characteristics through Pipe

Culvert Combined with Broad Crested Weir" MSc

Thesis, College of Engineering Salahaddin University

Erbil 2010.

S. Hoseini, S. Jahromi, M. Vahid “Determination of

Discharge Coefficient of Rectangular Broad-Crested

Side Weir in Trapezoidal Channel by CFD” IJHE 2013,

2(4): 64-70

Sarker, M.A and Rhodes, D.G," Calculation of free surface

profile over a rectangular broad-crested weir". Flow

Measurement and Instrumentation, 2004, 15(4) 215-219.

Versteeg H. K. and Malalasekera W. "An Introduction to

Computational Fluid Dynamics" Second Edition,

Pearson Education Limited 2007, pp 14, 66.

Wilcox D. C., "Turbulence Modeling for CFD", DCW

Industries Inc., La Canada, California (1993).