Fill out the form to download

Required field
Required field
Not a valid email address
Required field


Large Eddy Simulation: Flow Over a cylinder


The purpose of this numerical simulation is to validate the following parameters of incompressible Large Eddy Simulation (LES) of flow over a cylinder:

  • Pressure distribution on the surface
  • Stream-wise Velocity distribution in the wake

The numerical simulation results of SimScale were compared with the experimental results. The flow regime selected for the study is classified as sub-critical with a flow reynold number of Re=3900



Import validation project into workspace


The geometry of the study is a straight cylindrical body (see Fig.1.). A brief description of the dimensions is provided by the table below.

Fig.1. Geometry of the cylindrical body
Value [m]πD


Domain and Analysis type

An O-type domain was selected as the flow domain around the cylinder. The domain was 15D


 in the radial direction and πD


 in the span-wise direction (see Fig.2.). For this study a structured hexahedral mesh was created with the open source ‘BlockMesh-tool’. The grid nodes are distributed by a geometric grading in the radial direction. Further, the nodes are clustered near the stagnation point and in the wake region along the stream-wise direction. The mesh is based on a y-plus (y+


) criterion of y+<1


in the radial direction. The complete details of the mesh are listed in the following table:

Mesh and Element types :

Mesh typeCells in radialCells in circumferentialCells in spanwiseNumber of nodesType
blockMesh1652043411444403D hexahedral
Fig.2. Mesh used for the SimScale case

The numerical analysis performed is detailed as follows:

Tool Type : OPENFOAM®

Analysis Type : Incompressible Large Eddy Simulation

Sub-Grid-Scale Model : Smagorinsky with Cube-Root-Volume delta

Simulation Setup


  • Air: Dynamic viscosity (ν




Boundary Conditions:

The inlet boundary was set as a non-turbulent fixed velocity condition, while a pressure boundary condition was applied at the outlet. For the spanwise boundaries a symmetry condition was applied. The following table provides the further details.

Boundary typeVelocityPressure
InletFixed Value: 0.59 ms1

0.59 ms1
Zero Gradient
OutletinletOutletFixed Value: 0 Pa

0 Pa
Wall no-slipFixed Value: 0.0 ms1

0.0 ms1
Zero Gradient


The numerical simulation results of mean pressure distribution and mean stream-wise velocity are compared with experimental data provided by C.Norberg [1] , L.Ong and J.Wallace [2] and L.M.Lourenco and C.Shih [3] . To ensure meaningful results, averaging was carried out over periods of atleast 100D/U


 time units or about 21 vortex shedding cycles.

A comparison of the mean pressure distribution obtained with SimScale and experimental results is given in Fig.3A. The mean stream-wise velocity profile is compared with experimental data as shows by the Fig.3B.

 Fig.3. Pressure distribution comparison (left), streamwise velocity profile comparison (right)

The instantaneous vorticity component wz


, and averaged streamlines in the cross-section (x-y plane) are shown by the Fig.4A and Fig.4B respectively.


A visualization of the instantaneous flow field is shown along the cross-sectional and spanwise planes provided by Fig.5A and Fig.5B.

 Fig.5. Instantaneous flow field along stream-wise (left), and along span directions (right)


  1. Norberg, ‘Effects of Reynolds number and low-intensity free stream turbulence on the flow around a circular cylinder’, Publ. No. 87 /2, Department of Applied Thermoscience and Fluid Mech., Chalmers University of Technology, Gothenburg, Sweden, 1987.
  1. Ong and J. Wallace, ‘The velocity field of the turbulent very near wake of a circular cylinder’, Exp. Fluids, 20, 441–453, Springer Verlag, Berlin (1996).
[3]L.M. Lourenco and C. Shih, ‘Characteristics of the plane turbulent near wake of a circular cylinder, a particle image velocimetry study’, Private Communication, 1993.


This offering is not approved or endorsed by OpenCFD Limited, producer and distributor of the OpenFOAM software and owner of the OPENFOAM® and OpenCFD® trade marks. OPENFOAM® is a registered trade mark of OpenCFD Limited, producer and distributor of the OpenFOAM software.

Last updated: January 8th, 2021

Data Privacy