|
[Sponsors] |
no mesh independency of turbulent flow across tube bank |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
July 6, 2012, 06:21 |
no mesh independency of turbulent flow across tube bank
|
#1 |
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 |
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. |
|
July 6, 2012, 07:25 |
|
#3 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,854
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 |
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 |
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,427
Rep Power: 49 |
I love it when a plan comes together
|
|
Tags |
cross flow, grid, refinement, tube bank, turbulent |
|
|
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 |