Table of Contents
CFD Modeling of Laminar and Turbulent Flow Over a Circular Cylinder
By Dr. Sharad N. Pachpute
Flow Over a Cylinder
 Flow over a cylinder is important in many industrial application like cooling of iron or cylindrical pipe
 Circular pipes have more application in heat exchanger. High temperature flue gases flow over a circular cylinder in a cross flow.
 Depending on flow rate, fluid properties and size of cylinder, the flow can be laminar, transition and turbulent
 Larger vortexes are found at lower Reynolds number.
Geometry for CFD Simulation
 Geometry and Computational domain for cross flow over a circular cylinder inside the pipe
Computational Grid (Mesh Model)
 Structured and body fitted mesh used for CFD simulations using ANSYS GAMBIT
 High mesh density used around the cylinder to numerically resolve boundary layers for turbulent flow
 Various Mesh Models of used in this study is shown below
 Mesh 1
 Mesh 2
 Mesh3: Fine Mesh Model for flow over a circular cylinder
 Fine mesh region around the cylinder
Physical Properties
 Constant thermo physical properties used for the present numerical simulation
 The physical properties for a dummy fluid assumed to be constant with density (ρ) of 1 kg/m^{3} and viscosity 1 kg/ms.
Governing Equation for Laminar and Turbulent Flow
 In the present study, the flow is assumed to be twodimensional and incompressible. The effects of body forces and viscous dissipation are neglected in this study.
 The thermophysical properties for a dummy fluid are assumed to be constant
 Both laminar and turbulent flows are considered in this study. In the following subsections, the governing equations are given for laminar and turbulent flows.
Laminar Flow
 Continuity equation
 Momentum equations
In the above equations, u, v , w are the velocity in x, y and z directions p is the pressure ρ, and ν are density and kinematic viscosity of the fluid.
Turbulent Flow Modeling
Standard kε Model
The governing equations in unsteady turbulent flow for 2 equation Standard kε Model is given below. For 2D turbulent flow in a XY plane, all the gradients w.r.t. Zdirections are zero.
Turbulent Kinetic Energy Equation (k):
Dissipation of TKE (ε):
P_{k} denotes the rate of shear production of k
Standard Wall Functions
The standard wall functions for the mean streamwise velocity and turbulence kinetic energy are given as
Turbulence Model : Reynolds Stress Model (RSM)
 Transport equation for the Reynolds stress tensor τ_{ij} after some adjustments can be written as
Where,
Pressure strain rate in the Reynolds stress transport equation:
Dissipation term in the Reynolds stress transport equation:
Turbulent Transport in the Reynolds stress transport equation:
 For Reynolds stress modeling (RSM), 7 equations used to model the anisotropic turbulent flow
Initial and Boundary condition
In the present study, the flow is unsteady and periodic. The results must be taken only after the periodic flow is established.
Initial Condition: t he velocity is initialized as At t = 0 u = 0, v = 0 (10)
Boundary conditions:
 Inlet: A uniform velocity and constant free stream temperature are assumed at the inlet boundary
u = U_{∞,} v = 0 (11)
 Outlet: Outflow (zero gradient) condition used at the outlet.
 Symmetry: Since the problem considered is a 2D problem, symmetry boundary conditions are imposed for both top and bottom boundaries
 Wall: The cylinder surface and side walls ae considered as wall with no slip condition
Lift coefficient
To represent the results and characterize the combined heat transfer problem, the following nondimensional variables and parameters are defined.
The lift coefficients are computed from the following expressions
Where, D is the cylinder diameter, F_{x} and F_{y} are the force components resolved in the directions x and y.
 If τ_{s} is shear stress at wall and y is distance from it, then the nondimensional term in turbulent flow is given as
Numerical Details in ANSYS FLUENT
ANSYS GAMBIT used for mesh generation and meshing. Tthe numerical simulation carried out by using a commercial finite volume method solver (ANSYS FLUENT).
 Solver Setting
 Steady Incompressible Solver at Re=1
 Unsteady, second order Implicit Incompressible solver at Re=272, 2902
 Physical Model:
 Viscouslaminar Model for Re=1 and 272
 Turbulent Models; standard kε and RSM Models for Re=2902
 Velocity Boundary Conditions
 For inlet a fixed uniform velocity of 0.0005 m/s used such that, Reynolds number
(Re =ρ U D/μ ) are 1,272, and 2902 based on different velocities (U), 1, 272 and 2902 m/s at inlet with cylinder diameter (D), 1 m.
 Turbulent Parameters at inlet: Turbulent Intensity 1 % and Hydraulic diameter, D (1m)
 Pressure Boundary: The operating pressure 101325 Pa used at inlet.
P_{absolute} = P_{gauge} +P _{operating}, assumed zero gauge pressure at inlet
P_{total} = P_{static} + 1/2ρu^{2} for incompressible flow
 Pressure Velocity Coupling – Semi –implicit Method for Pressure Linked Equation (SIMPLE)
 Discretization Scheme or Spatial Interpolation–
 Pressure – Standard
 Momentum – QUICK (Quadratic Upwind interpolation for Convective Kinetics)

 Turbulent Kinetic Energy.: QUICK
 Turbulent Dissipation rate : QUICK
 Reynolds Stresses: QUICK
 Time Step (Δt) :
 Δt=1e3 S for laminar flow is less than the time period of vortex shedding , 0.021second.
 Δt=1e5 second used for turbulent, Standard ke models, it is less than time period of vortex shedding , 0.0018 seconds.
 Δt=1e6 second used for turbulent, RSM models, it is less than time period of vortex shedding , 0.00018 seconds.
 Convergence Criteria: Convergence criteria for all flow variable kept 1e7
 Convergence for laminar flow at Red = 1

 Residuals for turbulent flow
Grid Independence Study
Effect of different meshes on CFD results have been studied at Re = 272
Grid Sensitive studies for Velocities contours at Re=272
 Mesh 1
 Velocity Contours for Mesh 2
 Velocity Contours for Mesh 3
 From above grid sensitive studies for different gird sizes, it shows that the velocity contours around the cylinders for Grid3 are properly calculated, this grid is used for laminar flow and turbulent flow evaluation
Results for Laminar Flow
Coefficients of Lift (C_{L})
 Coefficients of Lift Vs Flow time for laminar flow over the cylinder, Re=272
Velocity Distribution at Re=272
 Velocity Contours over a cylinder
 Stream lines around the cylinder
 Velocity profile around the cylinder
 Velocity in wake region of the cylinder is low compared to other regions
Pressure Distribution (P_{Static}) at Re=272
 High pressure is front side of cylinder and low pressure in the rear portion of cylinder
CFD Results for Turbulent flow
Turbulent Flow and Pressure Field using Standard kε Model
 Velocity Contours and vectors in turbulent flow over a cylinder, Re=2902
 Velocity Contours over a cylinder is shown below
 Velocity profile in wake region of the cylinder
 Pressure fields in turbulent flow over a cylinder
 Coefficients of Lift Vs Flow time for turbulent flow over the cylinder, Re=2902
 Wall Yplus for turbulent flow over the cylinder, Re=2902
 As expected Yplus around the cylinder is less than 5 means and fine mesh used for turbulent study is acceptable at Re=2902
Results for RSM turbulent Model
 Velocity Contours and vectors in turbulent flow over a cylinder, RSMModel at Re=2902
 Stream lines for CFD simulation using the RSM turbulence model is shown below
Velocity Contours over a cylinder
 Velocity profile in wake region of the cylinder
 Pressure fields in turbulent flow over a cylinder
 Coefficients of Lift Vs Flow time for turbulent flow over the cylinder, Re=2902
 Wall Yplus for RSM turbulent flow over the cylinder, Re=2902
Comparison of flow Laminar and Turbulent Flow

Velocity vector for flow over a cylinder at Re=1, 272 and 2902
(a) Re=1
 Flow pattern is symmetrical above and below of the cylinder.
 The size of wake region is small
(b) Re=272
 At this Reynolds number, flow around the cylinder is laminar and the boundary layer region around the cylinder is significant up to an angle of 100 degree from stagnation point
 With an increase in Reynolds number, the size of wake region behind the cylinder increases
(c) Re=2902
 At this Reynolds number, flow around the cylinder is turbulent and the boundary layer region around the cylinder is significant up to an angle of 120 degree from stagnation point
 Compare to laminar flow, the size of wake region behind the cylinder is higher for turbulent flow
 Velocity vectors for Turbulent flow over a cylinder is presented as below
Velocity Contours for flow over a cylinder at Re=1, 272 and 2902
 Flow at Low Reynolds Number (Re=1)
 Velocity contours around the cylinder symmetrical
 Flow at Intermediate Reynolds Number (Re=272)
 Velocity contours around the cylinder is not symmetrical
 Unsteady (Von karman) vortexes are observed behind the cylinder
 Flow at High Reynolds Number (Re=2902)
 Velocity contours around the cylinder is not symmetrical
 Unsteady vortexes of small sizes are observed behind the cylinder
Vortex Shedding Frequency and Stroul Number
Reynolds Number, Re_{D}  Velocity, U (m/s)  Time Period, T (S)  Frequency (T^{1})  St=f D/U  ΔSt^{*} 
272 (Laminar flow)  272  0.0201  49.75  0.1829  1E04 
2902 ( Turbulent flow)  2902  0.0018  555.556  0.191  +0.0080 
Note: ^{* }The correlation for a circular cylinder, f*D/U=0.183, it is compared with numerical values
Concluding Remark
 CFD analysis of laminar and turbulent flow over a circular cylinder has been carried out for different Reynolds number. Coefficients of lift, contours of velocity and pressures are discussed in details.
 At low Reynolds number (Re=1) flow is steady, and streamline are symmetrical about Yaxis of cylinder
 With increasing in Reynolds number, the flow becomes unsteady, flow pattern shows periodic flow of vortex shedding in the wake region of the cylinder which is called the von Kaman vortex
 At a higher Reynolds number, flow around the cylinder becomes irregular. The increased inertia forces break the vortex generated behind the cylinder, with a higher frequency of vortex shedding than that in laminar flow
YouTube Video Modeling of Flow over Cylinder
 Watch YouTube videos on how to make a geometry of and meshing of flow over a circular cylinder using ANSYS Space claim and workbench. Simulation is carried out in FLUENT
 Click here: CFD Modeling of flow over a 3D circular cylinder
excellent points altogether, you simply gained a new reader.
What may you suggest in regards to your submit that you just made some
days in the past? Any certain?