no mesh independency of turbulent flow across tube bank

rasko · July 6, 2012, 06:21

Hello everybody,
I want to do a simulation of a turbulent cross flow over a staggered tube bank and encountered a problem I´m 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.

Thanks

flotus1 · July 6, 2012, 06:55

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, 07:25

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, 11:47

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

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

flotus1 · July 7, 2012, 03:45

I love it when a plan comes together

July 6, 2012, 06:21	no mesh independency of turbulent flow across tube bank	#1
rasko New Member Nils Schueler Join Date: Jul 2012 Location: Munich Posts: 11 Rep Power: 14	Hello everybody, I want to do a simulation of a turbulent cross flow over a staggered tube bank and encountered a problem I´m 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. Thanks

July 6, 2012, 06:55		#2
flotus1 Super Moderator Alex Join Date: Jun 2012 Location: Germany Posts: 3,427 Rep Power: 49	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. rasko likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
3D Hybrid Mesh Errors	DarrenC	ANSYS Meshing & Geometry	11	August 5, 2013 07:42
[Other] Mesh for swirling turbulent pipe flow	mahmutkaplan	OpenFOAM Meshing & Mesh Conversion	0	June 14, 2012 09:19
mesh quality and independency..!??	michelle	CFX	0	October 15, 2007 06:50
Icemcfd 11: Loss of mesh from surface mesh option?	Joe	CFX	2	March 26, 2007 19:10
mesh for laminer and turbulent flow over airfoil	M. Essuri	FLUENT	0	November 20, 2006 13:22

July 6, 2012, 07:25		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,844 Rep Power: 144	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.

July 6, 2012, 11:47		#4
rasko New Member Nils Schueler Join Date: Jul 2012 Location: Munich Posts: 11 Rep Power: 14	@Alexander: Thank you for your helpful advice! That seemed to be the problem. I have carried out your suggestions and it works now @Glenn Thank you for your hint too. I will keep that in mind!

July 7, 2012, 03:45		#5
flotus1 Super Moderator Alex Join Date: Jun 2012 Location: Germany Posts: 3,427 Rep Power: 49	I love it when a plan comes together