In this thesis numerical simulation for classical case of flow over a cylinder is accomplished for 2D models using commercial CFD code Star CCM+ with k-ϵ model approach. The results are validated by comparing the Drag coefficients to the previously published data. The simulation is carried out to for Reynolds number 3900 to investigate the turbulence modeling on separation from curved surfaces of two different sizes of a circular cylinder, a cylinder with triangular cross section and a rectangular cross section. Investigation of different turbulence models and Mesh convergence is carried out. The investigation of the turbulence model of the circular cylinder is carried out by the drag coefficient obtained by four different turbulence models such as K-Epsilon Turbulence, K-Omega Turbulence, Reynolds Stress Turbulence and Spalart-Allmaras Turbulence. Drag coefficient found out by different turbulence model is compared with the experimental value of a previously published data. The Mesh Convergence have been carried out by implementing different base mesh size in a decreasing order and the convergence is obtained when the drag coefficient becomes constant

1. Simulation of segregated flow over the 2D cylinder using
STAR-CCM+
Burak Turhan
Abstract
In this thesis numerical simulation for classical case of flow over a cylinder is accomplished
for 2D models using commercial CFD code Star CCM+ with k-ϵ model approach. The results
are validated by comparing the Drag coefficients to the previous published data. The simulation
is carried out to for Reynolds number 3900 to investigate the turbulence modelling on
separation from curved surfaces of two different sizes of circular cylinder, a cylinder with
triangular cross section and a rectangular cross section. Investigation of different turbulence
models and Mesh convergence is carried out.
The investigation of the turbulence model of the circular cylinder is carried out by the drag
coefficient obtained by four different turbulence models such as K-Epsilon Turbulence, K-
Omega Turbulence, Reynolds Stress Turbulence and Spalart-Allmaras Turbulence. Drag
coefficient found out by different turbulence model is compared with the experimental value
of a previously published data. The Mesh Convergence have been carried out by implementing
different base mesh size in a decreasing order and the convergence is obtained when the drag
coefficient becomes constant.
1. Introduction and Literature View
Computational Fluid Dynamics (CFD) calculates numerical solutions using the equations
governing fluid flow which are called the Navier-Stokes equations. One of the classical
problems in fluid mechanics is the determination of the flow field past a bluff body represented
by a circular cylinder. Study of Flow around the Circular Cylinder plays significant role in
Aerospace, Automobile, Marine hydrodynamics and other technical applications. Flow over a
cylinder is one of the classical problems in Fluid mechanics. Many structures around daily life
are of cylindrical shapes like Risers, Pipelines, heat exchangers and chimneys. It is important
to understand the flow field around and forces acting on them.
The flow around circular cylinders involves various fluid dynamics phenomena, such as
separation, vortex shedding and the transition to turbulence. One such Interesting Phenomena

2. is Flow over a rotating non-slip cylinder wall creates a pressure gradient in turn creates lift
known as Magnus effect.
Viscus flow past a circular cylinder becomes unstable around Reynolds number 40. The wake
bubble grows in length approximately linear with Re. The cylinder moving in front with the
same speed supplies the same vorticity required to balance diffusion (Fornberg, 1984)
When Re > 40 the boundary layer over the cylinder surface will separate due to the adverse
pressure Gradient. This pressure gradient arises because of the divergent environment of the
flow at the rear side of the cylinder. The result of this is a shear layer. The boundary layer along
the cylinder contains a significant amount of vorticity. The vorticity will continue into the shear
layer downstream of the separation point and cause the shear layer to roll up into a vortex with
a sign identical to that of the incoming vorticity. (Sumer et al, 1997)
These flows can be studied by various methods such as Analytical method, Experimental and
Computer simulation (Numerical method). Computer simulation provides solution for less cost
compared to experimental method and solutions to complex models which are difficult to solve
by Analytical methods. There are various CFD codes available presently important once being
Star CCM+, Phoenix ,ANSYS Fluent and ANSYS CFX which has to be chosen properly
depending the application. The 2 major approaches ‘Large eddy simulation’ and RANS can be
used in these software. The working of CFD involves three steps Pre-processor, Solve and
Post-processor:
• Pre-processor involves preparing Geometry, define the simulation topology, generate
the mesh, define the physics, and prepare for analysis. The region of fluid domain to be
analysed is made up of number of discrete elements called mesh. Fluid properties and boundary
conditions are defined.
• Solver calculates the solution of the CFD problem by solving the governing equations.
The equations governing the fluid motion are Partial Differential Equations, made up of
combinations of the flow variables like velocity and pressure and the derivatives of these
variables. We use Finite volume method of discretization here in Star CCM+.
• Post processor is used to visualize and quantitatively process the results from the solver.
In a CFD package, the analysed flow phenomena can be presented in vector plots or contour
plots to display the trends of velocity, pressure, kinetic energy and other properties of the flow.

3. Also, another literature mentioned that, at low value of Reynolds number the geometry gives a
steady and symmetric flow pattern. Any disturbance introduced at the inlet gets damped by the
viscous forces. As the Reynolds number is increased, the disturbance in the upstream flow may
not be damped. This leads to a very important periodic phenomenon downstream of the
cylinder, known as “vortex shedding”. The vortices become stronger and larger with increases
in the Re number. This arrangement becomes unstable beyond a certain critical Reynolds
numbers (Re ~ 47) and von Karman vortex shedding takes place. At this point the flow is still
two-dimensional and laminar. (Iglesias et al, 2014)
Study shows that STAR CCM+ software performs well using LES and the Smagorinsky
subgrid scale turbulence model in case of cylinder in uniform, steady and infinite current. In
case of a cylinder in the vicinity of a rigid wall it is observed that the vortex shedding was
suppressed and the mean lift coefficient was increased and the mean drag coefficient was
decreased. The gap-to-diameter ratio and the boundary layer thickness affect the flow around
the cylinder. Also both the inlet velocity and the proximity of a rigid wall indeed affect the flow
around the cylinder and the forces acting on it. (Sunniva et al, 2013)
2. Methodology
Flow past thought the circular cylinder tends to follow the shape of the domain that change
with Reynolds Number. That means that, small Reynolds number corresponds to slow viscous
flow. If Reynolds number is increased, flows are characterised as velocity variation, the
occurrence of vortices and turbulence. Mathematically, Reynolds number of the flow around a
circular cylinder is represented by as following equation (1)
𝑅𝑒 =
𝜌𝑢𝐷
µ
(1)
where D is the diameter of the cylinder, u is the inlet velocity of the flow, ρ is a density of fluid
and µ is the dynamic viscosity of fluid (Zdravkovich, 1997). Moreover, Zdravkovich (1997)
mentioned that when Reynolds number changes, flow that is around a circular cylinder changes
from laminar to turbulent. Generally, the following regimes have been described from
experiment as follows;
Stable range 40 < Re < 150
Transition range 150 < Re < 300
Irregular range 300 < Re < 200; 000

4. Another significant parameter is that simulate all forces coefficient accurately of the past
thought the cylinder. Yogani (2010) described that the drag force performs in opposite
direction of the relative flow velocity. Drag depend on shape and orientation of the domain.
On the other hand, lift coefficient is calculated same as drag coefficient but vertical force is
considered rather than horizontal one. Both drag coefficient and lift coefficient are calculated
as following equations;
𝐶 𝑑 =
𝐹 𝑑
1
2
𝜌𝑢2 𝐴
𝐶𝑙 =
𝐹 𝑙
1
2
𝜌𝑢2 𝐴
where A is the projected area in the flow direction and Fd is the sum of the pressure force and
the viscous force components on the cylinder surface in the horizontal direction
(Yogani,2010).
In the current work, 2D CFD model in STAR-CCM simulate the classical case of flow over a
cylinder with turbulent models that chosen from the published data. According to benchmark
literature, in whole simulations Reynold number is chosen 3900. All results is compared with
drag and lift coefficient for each models. The brief details of the simulations are as follows:
2.1 STAR-CCM+ simulation
Computational Fluid Dynamics code STAR-CCM+ were used in the present study to get result
from domain which consisted of turbulence modelling over the cylinder. STAR-CCM+ was
also used to generate mesh, set up physics models, solve and conduct post-processing of the
results.
2.1.1 Geometry modelling
The computational domain is illustrated in following Figure 2.1.1-1 that is shown geometry
dimensions of modelling according to benchmark literature. Therefore, cylinder is simulated
with radius ( R ) of 3 mm. Moreover, cylinder is placed 20 times the radius from the inlet and
in the middle of vertical direction. Lastly, depth of the modelling is 2πR to incorporate the
spanwise effects.

5. Figure 2.1.1-1: Geometry Modelling with Dimension
2.1.2 Mesh generation
Polyhedral and prism layer meshing models were applied in the simulation. In the present
study, badge for 2D meshing was employed as a meshing model types. The polyhedral mesh
type was preferred considering such factors as, the turn-around time for building the mesh, the
accuracy of the solution and convergence acquires, the quality of the surface mesh and quality
of solution. The prism layer mesh model was used in model with the core polyhedral mesh to
generate orthogonal prismatic cells near the wall boundaries. Following Table 2.1.2.1 shows
mesh parameters that select in present study.
Parameters Values
Base size 5.0E-5 m
Surface curvature Default
Surface growth rate Default
Surface proximity Default
Absolute minimum size 5.0E-6 m
Absolute target size 5.0E-5 m
Number of prism layers 5
Prism layer thickness 1.665E-5 m
Table 2.1.2.1: Mesh Parameters and mesh distribution
2.1.3 Initial Conditions and Boundary Conditions
The boundaries for the computational domain are selected in regions section in STAR-CCM+.
Therefore, different boundaries are selected for each parameters. One part of the region is
selected as an inlet that defined as velocity inlet. Velocity value 9 m/s is introduced at the inlet
correspond to the Reynolds number of. 3900. Secondly, other part of the region is defined as
outlet that is pressure outlet that pressure is 0 pa. According to reference literature, cylinder is

6. defined as no-slip wall, both top and bottom wall are selected as symmetry plane. Following
figure 2.1.3.1 show as boundary condition of the present study.
Figure 2.1.3.1: Boundary Condition of the model
2.1.4 Setting up physics models
The physics continuum for single phase gas used for the present study consisted of the models
shown in Table 2.1.4.1
Space Two Dimensional
Time Implicit Unsteady
Material Gas
Flow Segregated Flow
Equation of State Constant Density
Viscous Regime Turbulent
Reynolds-Averaged Turbulence K-epsilon Turbulence
Wall treatment All y+
Table 2.1.4.1: Physics Models of Simulation
2.1.4.1 Material modelling
Constant density gas which was the material simulated in the continuum was responsible for
managing velocity and defined drag coefficient of the modelling and physical processes being
modelled in the continuum. Table 2.1.4.1.1 illustrates the properties of gas used in the present
study.
Properties Values
Temperature 275 K
Density 1.284 kg/m3
Dynamic Viscosity 1.725E-5 kg/m s

7. Table 2.1.4.1.1: Material Properties
2.1.4.2 Turbulence modelling
All turbulence models Intensity and Length scale parameters are used in the present study in
order to calculate parameters to use in model. Other turbulence factors can be derived from
these numbers, including the Modified Turbulent Viscosity and the Specific Dissipation Rate
(used for K-omega models). Calculation of these parameters that calculated following
definitions.
Turbulent Length Scale that is used in this case is approximately 7% of the inlet length that
is 0.00672 m.
Turbulent Velocity Scale that is used in this case is 10% of the inlet velocity that is
0.9 m/s.
Turbulence Intensity is calculated following equation and where vt is turbulent scale
and U is velocity.
𝐼 = √
3
2
𝑣 𝑡
2
𝑈2 = 0.12
3. Results and discussion
The simulations are conducted for Reynolds numbers of 3900 according to reference literature.
The choice of the Reynolds numbers of simulation depends largely on the experimental data
available in the benchmark paper. Therefore, critical flow parameters, which are drag
coefficient and fluctuating lift coefficient, have been predicted with different turbulence model
and all different cases are compared with experimental and benchmark literature. In addition,
all result are explain briefly as below.

8. 3.1 Comparison of benchmark literature
The experimental value of the paper is found to be closer to the value that was found from the
simulation. The experimental value is about 0.93±0.005 and the value that was found from the
simulation is 0.9487, which is about 1.87% higher than the experimental value. In the paper
the simulation is carried out by three different models, which are K – ϵ, SST and LES. The
results obtained by the K – ϵ, SST and LES models are 0.7446, 0.6208 and 1.0683 respectively
and the experimental value is about 0.93±0.005. The drag coefficient that was found by the
using the K – ϵ simulation is about 18% lower than the experimental value and that of the SST
simulation is about 30% lower than the experimental value. The drag coefficient obtained from
the LES simulation model is 1.0683, which is 13% higher than the experimental value. From
the comparison of the Cd values from the table, the value obtained with the LES model is the
closer equivalent to the experimental value.
ReD = 3900
Cd
(Yogini Patel, 2010)
Cd
(Implemented Model)
Experimental Value 0.93±0.005
0.9487
K – ϵ 0.7446
SST 0.6208
LES 1.0683
Table 3.1.1: Drag Coefficient Values both implemented model and benchmark paper
Figure 3.1.2: Velocity and residuals of the simulation
3.2 Mesh convergence
The following table and graph of mesh convergence for the model of circular cylinder of
diameter 0.006 m. The graph is plotted for base mesh size versus coefficient of Drag. It can be
observed that value of coefficient of drag reaches almost constant value after .00004 mesh size
and then the mesh converges at 0.00005 for Drag Coefficient 0.9487. Hence this Base mesh
size is used for further simulations and Turbulence models.

9. Base mesh
size
0.01 0.001 0.0001 0.00001 0.00002 0.00003 0.00004 0.00005 0.00006
Drag
Coefficient
1.0772 0.9967 0.8877 0.9271 0.9322 0.9411 0.9461 0.9487 0.9489
Table3.2.1: Mesh Convergence
Graph 3.2.2: Graph of the Mesh convergence
3.3 Effect of different turbulence model
The simulation have been carried out with four different turbulence model, which are K-
Epsilon Turbulence, K-Omega Turbulence, Reynolds Stress Turbulence and Spalart-Allmaras
Turbulence. The drag coefficient for each turbulence model have been noted down in the table.
K-Epsilon Turbulence model has the greatest value out of all the turbulence models, ie, 0.9487.
The least drag coefficient is found out as 0.88357 for Spalart-Allmaras Turbulence model. K-
Omega Turbulence and Reynolds Stress Turbulence have almost the same drag coefficient of
0.8994 and 0.8909 respectively. To sum up all these values are almost equal to the experimental
value.
Turbulence Models Drag Coefficient
K-Epsilon Turbulence 0.9487
K-Omega Turbulence 0.8994
Reynolds Stress Turbulence 0.8909
Spalart-Allmaras Turbulence 0.88357
0
0,2
0,4
0,6
0,8
1
1,2
0,01 0,001 0,0001 0,00001 0,00002 0,00003 0,00004 0,00005 0,00006
Coefficent of Drag
Coefficent of Drag

10. Table 3.3.1: Different Turbulence Models
3.4 Comparison of different computational domain
Four different computational models are created and have compared the velocity and drag
coefficient results for the simulation as show in the table below. Case-1 is the standard model
with the cylinder of diameter of 0.006 m and the inlet velocity as 9 m/s. The drag coefficient
of case-1 have been noted and that is 0.9487. Secondly, in Case-2, the diameter of the cylinder
is increased to 0.018. Hence, when increased the diameter, to keep Reynolds number constant,
according to numerical calculation velocity inlet have decreased to 6 m/s and drag coefficient
increases to 0.9843. In Case-3, the curvature of the cylinder have changed to a triangular shape
with sides 0.006 m and the drag coefficient compared to case 1 has increased to 1.last but not
least, in Case-4, the cylinder have reconstructed into a square shape with sides 0.006 m. The
drag coefficient of case-4 was found out to be 1.5363, which is the highest value of drag
coefficient among the other three cases. When all the geometries are compare, the square
cylinder has the greater value for drag coefficient and the circular cylinder has the smallest
value for drag coefficient. While designing a model these different values for different
cylinders should be taken into consideration.
Case Velocity Drag Coefficient
Case 1 0.9487
Case 2 0.7483

11. Case 3
1.08798
Case 4
1.5363
Table 3.4.1: Velocity and Drag Coefficient Result for different geometry
4. Conclusion
In this study different types of cylinder models have been implemented to show the flow of gas
over it by Computational Fluid Dynamics (CFD) using STAR-CCM+ software. Four different
models have been made with a Reynolds Number of 3900, the first one is a circular cylinder
with diameter of 0.006 m, the second one is also a circular cylinder but with an increased
diameter of 0.018 m and the third and fourth models are Triangular and Square cylinders
respectively with sides 0.006 m. For each cases the values of Drag Coefficients have been noted
down and compared. Few papers have been referred to verify our results. To sum up, all results
of different type of modelling that was found using the STAR-CCM+ in this present study are
extremely close to literature that have already published. In other words, values of the present
simulation are accurate for each cases.

12. References
Zdravkovich, M. M., (1997)’ Flow around circular cylinders’ Vol 1: fundamentals, First
edition. Printed in Oxford University Press.
Yogini P. (2010), ‘Numerical Investigation of Flow past a Circular Cylinder and in a Staggered
Tube Bundle Using Various Turbulence Models’, Lappeenranta University of Technology
N. Cinosi, S.P. Walker, M.J. Bluck, R. Issa (2014)’ ‘CFD simulation of turbulent flow in a
rod bundle with spacer grids (MATIS-H) using STAR-CCM+’. Nuclear Engineering and
Design Volume. 279, pp. 37–49.
V.Y. Agbodemegbea, Xu Chenga, E.H.K Akahob, F.K.A Alloteyc (2015),’ Correlation for
cross-flow resistance coefficient using STAR-CCM+ simulation data for flow of water
through rod bundle supported by spacer grid with split-type mixing vane ‘Nuclear
Engineering and Design Volume.285.pp.134-149.
STAR-CCM+® Documentation (2016), Version 11.02
Brengt Fornberg (1984) ‘Steady Viscus Flow past a Circular Cylinder up to Reynolds Number
600’. Journal of Computational Physics. 61(2) pp.297-320.
B. Mutlu Sumer, Jørgen Fredsøe (1997) ‘Hydrodynamics Around Cylindrical Structures’.
Advanced Series on Ocean Engineering, World Scientific Vol-12
Antonio Souto Iglesias Carlos Ariel Garrido Mendoza, Leo Miguel González Gutiérrez ‘Open
Course ware’. Universidad politecnica de Madrid).
Sunniva Selstad Thingbø (2013) ‘Simulation of viscous Flow around a circular Cylinder with
STAR-CCM+’. Master Thesis in Marine Hydrodynamics, Norwegian University of Science
and Technology.
Sercan Yagmur, Sercan Dogan, Muharrem H. Aksoy, Eyub Canli, Muammer Ozgoren, (2015).
Experimental and Numerical Investigation of Flow Structures around Cylindrical Bluff Bodies,
Selcuk University, Engineering Faculty, EDP Sciences.