CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > FLUENT

Finer mesh, worse result?

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

LinkBack Thread Tools Search this Thread Display Modes
Old   March 17, 2016, 12:51
Default Finer mesh, worse result?
New Member
Join Date: Jun 2011
Location: Jülich,Germany
Posts: 19
Rep Power: 15
Ryan_Yang is on a distinguished road
Hi, everyone,

I was trying to model a transient Couette flow with FLUENT (cf.Geometry). The walls at Y-direction are defined as translational periodic, the walls at Z-direction are defined as symmetric. Walls at X=H/2 and X=-H/2 started to move at t=0 with U=U_wall. The flow is laminar and calculation was performed for only one time step.

I found that with finer mesh, it is more difficult to obtain the converged result. Take the default convergence criterion 1e-3 for example (cf. Result), velocity profile along the +X-axis gets steeper with finer mesh( higher H/delta_X value), meanwhile it takes more iterations. However, with smaller convergence criterion (depending on how fine is the mesh), the result of finer mesh will eventually approach to the result of coarser mesh.

This blows my mind, does anyone knows why? Does it mean that I have to choose a specific convergence criterion for each mesh size individually?


Attached Images
File Type: jpg Geometry.jpg (15.0 KB, 38 views)
File Type: jpg Result.jpg (39.2 KB, 53 views)
Ryan_Yang is offline   Reply With Quote

Old   March 17, 2016, 14:52
Senior Member
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,685
Rep Power: 66
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
The velocity profile tends to be steeper on finer grids because there's less numerical dissipation/damping. Convergence doesn't mean the solution is accurate.

All else being equal (same problem, same initial guess, all settings equal), increasing the mesh resolution (finer mesh) will take more iterations to converge to the same solution.

It's a result of the implicit discretization schemes which results in a sparse linear system. That is, changes in cell properties only affect their immediate neighbors. Hence, it takes many many iterations for adjustments of the solution to slowly propagate cell by cell throughout the entire domain to reduce the global error.

This behavior can be overcome/accelerated by using a multigrid algorithm to improve the speed at which global errors are reduced, but when you go to a finer grid (you need to make the multigrid method more aggressive). If you don't change these settings in the multigrid solver, your finer grid would still take more iterations (because the coarse grid has more aggressive settings relative to the finer grid). However, I don't recommend changing the AMG parameters unless you are an expert. Merely, this is to explain why the behavior is normal.

Also, I recommend defining convergence criteria based on solution values (like a sane person would) rather than residuals. Residuals do not measure convergence. Residuals are good stopping criteria, but are terribly convergence criteria.

Last edited by LuckyTran; March 18, 2016 at 09:42.
LuckyTran is offline   Reply With Quote

Old   March 18, 2016, 03:48
New Member
Join Date: Jun 2011
Location: Jülich,Germany
Posts: 19
Rep Power: 15
Ryan_Yang is on a distinguished road
Hi, dude,
Thanks for your reply!
I will try to improve my calculation by your suggestion.

Ryan_Yang is offline   Reply With Quote


couette flow, fluent, mesh dependency

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
[snappyHexMesh] Add Mesh Layers doesnt work on the whole surface Kryo OpenFOAM Meshing & Mesh Conversion 13 February 17, 2022 07:34
sliding mesh problem in CFX Saima CFX 46 September 11, 2021 07:38
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 37 July 20, 2020 05:38
Getting coarse mesh from a finer initial mesh chriss85 OpenFOAM Programming & Development 9 May 8, 2017 14:07
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55

All times are GMT -4. The time now is 08:41.