CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Running, Solving & CFD (
-   -   LES of a turbulent channel flow stays laminar (

liu May 21, 2010 10:46

LES of a turbulent channel flow stays laminar
1 Attachment(s)
Hi folks,

I am trying to reproduce the channel flow case as in Baba-Ahmadi and Tablor (Computers & Fluids, 38 (2009):1299-1311) titled:" Inlet conditions for LES using mapping and feedback control".

The wall bounded channel is 20mX2mX2m. I wrote a m4 script for the grid. It has 60 grids in X direction and 30 in Z direction. The grid in Y direction is graded towards the wall (grading = 10) with a total of 60 grids.

The inlet velocity BC is "directMapped" with an offset of 0.5m and average velocity of 0.1375 m/s. Viscosity = 1E-5, So Re=13,750 which is the same as in the paper.

Other setups: LESModel = oneEqEddy, delta = cubeRootVol
div(phi,U) = Gauss linear;
ddtScheme = backward,

deltaT = 0.1s for total of Time = 1000 s (which is about 6-7 flow through)

But the flow stays laminar. Maybe I should run the case longer, say 100 flow through time?

I have attached the case file. Please help me setup the case correctly. Thanks.

eelcovv May 27, 2010 10:00

increase Re
Hi Liu,

I had the same problem with my channel. The problem is that the flow should first become unstable. If you start laminar you need to add some disturbance. The easiest way is to temporary decrease your viscosity (to say 1e-6 m2/s), run it until the flow shows turbulent structures, and then set it back to 1e-5 m2/s to set the correct Reynolds number.



cedric_duprat May 27, 2010 13:53

Hi Liu,

If you don't want to change your viscosity and your Reynolds number, you can add perturbation before beginning your calculation (i.e. as initial condition).

To proceed, you can :
1- first have a look at the perturbU tool which is usefull to add artificial noise close to the wall (where gradients are high). (you can find details in Eugene de Villiers Ph'D thesis)
2- then run your calculation using channelOodles solver to reach a turbulent state (simple channel flow solver)
3- then change your boundary conditions to use directMappedFields one with an already turbulent flow.
4- enjoy you calculation

This is working fine

I hope this will help.


All times are GMT -4. The time now is 06:46.