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

Bumpy convergence in regions of very small y+<0.1

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 4, 2014, 06:35
Default Bumpy convergence in regions of very small y+<0.1
  #1
Member
 
Join Date: Apr 2011
Posts: 30
Rep Power: 6
MainzerKaiser is on a distinguished road
In a CHT setup, I solve the steady state compressible NS equations with the total energy equation and every scheme set to High Resolution and chose the SST model. The application is a turbine rotor stator cavity with a through flow Re of 2e6 and Mach numbers up to 0.6 in the labyrinth seals.

The CHT evaluation is incorporated in an automatic optimization routine. So for every set of design variables there are the same mesh settings, resulting in y+ values that can vary for every solution from very small numbers to y+=8... So far the high y+ values not necessarily impede my results. I experience problems with very small y+ values below 0.1. The convergence for my fluid residuals get bumpy and the solution takes way to long. Thus, Id rather set my mesh slightly to coarse values for effficient runtimes.

What happens when the y+ values get so small?
MainzerKaiser is offline   Reply With Quote

Old   April 4, 2014, 09:33
Default
  #2
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 290
Rep Power: 6
RicochetJ is on a distinguished road
I can't talk specifically about your case, but do I do know for some models that too fine a mesh can cause some errors. For example, recently I ran a simulation using the RPI wall boiling model. It didn't like a super fine mesh at the walls (small Y+) and didn't converge well. I did a bit of reading, coarsened the mesh and it worked a treat.
RicochetJ is offline   Reply With Quote

Old   April 6, 2014, 08:30
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,825
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
It is numerical round-off. As the mesh gets finer the difference between adjacent cells gets smaller. When the difference is small enough that gradients start being affected you will have convergence problems.

The first thing to do is to use double precision numerics. If that does not work then you should carefully coarsen your mesh. Many people on this forum seem scared of y+>1; do a sensitivity check and find out if it is a problem in your case. In many cases y+>1 will work fine, and run much quicker.
ghorrocks is offline   Reply With Quote

Old   April 6, 2014, 08:50
Default
  #4
Member
 
Join Date: Apr 2011
Posts: 30
Rep Power: 6
MainzerKaiser is on a distinguished road
Thanks for the responses.
I already chose the double precision mode before. Could there be another explanation besides round off errors?

A coarsen grid also gave me better results. I just need an explanation why I not generated meshes with y+=1 for every set of design variables.
MainzerKaiser is offline   Reply With Quote

Old   April 6, 2014, 17:51
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,825
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Round off errors is the main cause. Another possibility is that you probably have too fast a transition from the small elements to the large ones, but this is a problem similar to numerical round off as well. Trust me, numerical round off is the key problem. It is normal to have problems converging to extremely fine meshes, especially heavily graded ones (that is, I expect your near wall mesh is much finer than your largest element size).

I have no idea why you did not generate meshes with y+=1 for all design points - you generated the meshes so you have to answer that. And as for the better results on coarsened grid, as I said, as you appear to be hitting numerical round-off limits so coarsening the mesh and moving away from that will help.
ghorrocks is offline   Reply With Quote

Reply

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
.STL: non-closed manifold surface giulio.topazio OpenFOAM Native Meshers: snappyHexMesh and Others 24 March 3, 2015 05:41
Simulating small features on large models siw CFX 1 February 16, 2012 18:10
[GAMBIT] Meshing multiple 3D regions gascortado ANSYS Meshing & Geometry 2 February 7, 2011 13:12
early stall, poor convergence, and mesh quality everest CFX 2 May 12, 2010 16:27
Convergence in Fluent at small (order 1) Re Sergei Chernyshenko FLUENT 0 January 10, 2008 06:39


All times are GMT -4. The time now is 23:18.