CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   no mesh independency of turbulent flow across tube bank (

rasko July 6, 2012 05:21

no mesh independency of turbulent flow across tube bank
Hello everybody,
I want to do a simulation of a turbulent cross flow over a staggered tube bank and encountered a problem Im not able to solve since a couple of days:
I want to calculate the pressure drop (not only but for now). The simulations converge (RMS 10e-5 and plotted value of pressure drop) and produce a value which is in the scale of results provided by empirical correlations. But when I refine the mesh, the numerical value changes quite arbitrary meaning with refinement it might first rise and after a greater refinement fall again.

I've tried a lot of different things e.g. using different kind of meshes, turbulence models (SST, k-omega), setting it up as 3D (actually it shall be 2D).

key features are
- 2D-channel with obstacles at the lower and upper wall (half tubes)
- symmetry BC at all walls besides inlet, outlet and tube walls (no-slip walls)
- isothermal
- steady-state

I would be very grateful for every hint, where the error might be. If you need more informations (files etc.) just tell me.


flotus1 July 6, 2012 05:55

Did you use a wall-function for the wall boundary conditions?

If you use automatic wall-functions, then an oscillating convergence with the grid spacing is a typical behaviour.

To eleminate this, resolve the boundary layer explicitly without a wall function (Y+ below 1)
Now when you refine the mesh, keep the size of the first cell constant (and also the cells in the prism layer).
Apply the refinement only to cells further away from the wall. Keep an eye on the volume change in the transition zone between boundary layer and the rest of the mesh.

ghorrocks July 6, 2012 06:25

Alexander's comments are important, but if they do not fix it I suspect you are suffering from a common problem with turbulence models in bluff body flows in that grid convergence is not always possible. As the mesh is refined the turbulence model tends to resolve features which arguably are large turbulent eddies, and as you refine you just resolve different eddies. This makes grid convergence difficult.

rasko July 6, 2012 10:47

@Alexander: Thank you for your helpful advice!
That seemed to be the problem. I have carried out your suggestions and it works now:)

Thank you for your hint too. I will keep that in mind!

flotus1 July 7, 2012 02:45

I love it when a plan comes together ;)

All times are GMT -4. The time now is 20:02.