|
[Sponsors] |
Grid refinement study for Order of accuracy and GCI |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
April 25, 2011, 16:04 |
Grid refinement study for Order of accuracy and GCI
|
#1 |
Senior Member
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 16 |
I am trying to ascertain the numerical accuracy of my simulations in CFX by following the procedure mentioned in the editorial policy of Journal of engineering.
My simulations are 3D turbulent flow . I take the overall pressure drop from inlet to outlet as the solution variable to calculate GCI and I use a representative mesh size for each mesh which I calculate as (total volume/total number of cells)^(1/3). I have generated results for many meshes and tried to calculate GCI for 3 meshes at any time. I have ensured that the grid refinement ratios r21 and r32 are both above 1.3 for any of the mesh set that i consider. However, I find that for the different mesh sets that i consider: a)either the the parameter GCI_fine*(r21^p)/GCI_course is not close to one. This parameter should be close to one for the grids to be in asymptotic range. b)when this parameter is indeed close to one for a set of meshes, (and GCI_fine is also is small..less than 2 percent), the observed order of accuracy p that I calculate comes out to be around 4 . Now I think it is incorrect and should be less than 2 (as the formal order of accuracy of CFX is 2...please correct me if I am wring). I have tried many fine and coarse meshes. Is the way I am calculating GCI correct? Is the value of p>2 indeed correct? For the results to be considered accurate what is the maximum acceptable value of GCI? Last edited by Chander; April 25, 2011 at 18:43. |
|
April 26, 2011, 23:27 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
Firstly well done on having a good look into mesh refinement. I reckon about half of the weird questions on this forum are from people who have not done a proper check of whether their simulation is accurate so I am glad you are doing it properly.
Yes, CFX is a second order code for much of its numerics but in my experience that rarely equates to a order of convergence of 2 due to numerical issues, non-linearities etc. So if it is converging nicely I am happy regardless of the number. If the parameter is not in the asymptotic range then you generally have to use a much tighter mesh for convergence, or you have a model which does not converge. Turbulence models with wall functions often do this as if they refine below y+<11 the model is not valid. |
|
April 28, 2011, 12:39 |
|
#3 | |
Senior Member
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 16 |
Quote:
Secondly regarding the turbulence models, I am using the standard k-omega model in CFX. As you know, it uses automatic wall treatment which as per CFX manual should work for any mesh refinement. I could not use the commonly recommended SST model as it simply does not converge. Do you think something could be wrong here? And lastly, I have obtained the converged results by reducing the automatically determined time-step for steady state simulations by one order of magnitude. I have checked my set-up again and again and it seems that it is fine. I have also played with boundary conditions for turbulence but convergence seems impossible without such large reduction in time-step. I remember that you had mentioned once before that convergence is fine irrespective of the time-step used as long as we get convergence. Still, it would be great if you could also have a look at another thread of mine here: http://www.cfd-online.com/Forums/mai...tions-cfx.html |
||
April 28, 2011, 19:39 |
|
#4 | |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
Quote:
|
||
May 3, 2011, 13:42 |
|
#5 | |
Senior Member
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 16 |
Quote:
I am a bit concerned after your reply. I am not able to get convergence with SST. I am attaching a crosssection of my mesh that I have used for SST. n the first pic showing the mesh, the fine mesh is the fluid part and the surrounding coarse mesh is the solid part. I am also attaching the convergence plots. The convergence criteria was rms residual of 1e-6 Do you see any obvious mistake/issue here? |
||
May 3, 2011, 20:13 |
|
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
It is common to have steady state convergence problems as you refine the grid. Some tips are here:
http://www.cfd-online.com/Wiki/Ansys...gence_criteria |
|
Tags |
gci, grid refinement |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
GCI non-uniform grid | Mat | FLUENT | 0 | June 14, 2004 15:21 |