CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

no mesh independency of turbulent flow across tube bank

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By flotus1

Reply
 
LinkBack Thread Tools Display Modes
Old   July 6, 2012, 06:21
Default no mesh independency of turbulent flow across tube bank
  #1
New Member
 
Nils Schueler
Join Date: Jul 2012
Location: Munich
Posts: 11
Rep Power: 4
rasko is on a distinguished road
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.

Thanks
rasko is offline   Reply With Quote

Old   July 6, 2012, 06:55
Default
  #2
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,035
Rep Power: 17
flotus1 will become famous soon enough
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.
flotus1 is offline   Reply With Quote

Old   July 6, 2012, 07:25
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,758
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   July 6, 2012, 11:47
Default
  #4
New Member
 
Nils Schueler
Join Date: Jul 2012
Location: Munich
Posts: 11
Rep Power: 4
rasko is on a distinguished road
@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!
rasko is offline   Reply With Quote

Old   July 7, 2012, 03:45
Default
  #5
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,035
Rep Power: 17
flotus1 will become famous soon enough
I love it when a plan comes together
flotus1 is offline   Reply With Quote

Reply

Tags
cross flow, grid, refinement, tube bank, turbulent

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 07:42
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


All times are GMT -4. The time now is 11:11.