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

early stall, poor convergence, and mesh quality

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 4, 2010, 10:10
Arrow early stall, poor convergence, and mesh quality
  #1
New Member
 
Join Date: May 2010
Location: Tokyo, Japan
Posts: 6
Rep Power: 7
everest is on a distinguished road
Hi everyone
I tried to use cfx12.0.1 to simulate aeroplane landing characteristics with high lift devices deployed. Simulations were carried out at a series of angle of attack(AOA) in order to obtain a plot of lift coefficient versus AOA.

I did a steady-state simulation using tets and prism elements. Residual Target is set to RMS=1E-6. Turbulence model is SST. Time step control is default setting for auto time step.

Now my problem is that the results show a early "stall", about 3 degrees ahead, compared with other's computations and experiences. At earlier AOA, the monitoring force coefficients all achieved to acceptable convergence levels. However, at the "stalling" AOA , The lift coefficient demonstrated a relatively large oscillation (nearly 10%). The average lift coefficient dropped. Attached figures below are coverging process of residuals and monitoring variables. The flow visualization in the CFX-post showed a large separation upon the wing. People with rich engineering experience told me flow separation cannot be that severe and there should be a reasonable converged result at this AOA.

I doubt whether the lift coefficient oscillation and the flow separation are physical. Since I lack experience (about 3 months in total) in CFX and related issues, I try to do some search and research in this forum. Now I still have something quite confusing and hope to get some advices here.

1. larger time step didn't fix my problem.
As suggested by people in this forum, I tried larger physical time step by increasing the time scale factor to 10. The results still oscillated in the end.

I understand larger time step here try to stabilized small transient features due to physical or unphysical reasons to find the final acceptable steady-state solution. Is it right? Since larger time step didn't take effect, does it mean that my problem is due to actual flow separation or poor mesh qualities.

2. Mesh quality issues
2.1. Small time step failed, too.
After a rather long run using a physical time scale, about one quarter of the original auto time scale, I still could not get a converged results.

Buried in CFX help files, I conclude that small time steps can increase numerical accuracies and then improve bad converging behavior resulting from low mesh quality. Is this conclusion right?

2.2 where does the maximum residual lie?
To figure out where the bad grid lies, I toggle on the residual backup. I found the maximum residuals lies right at some critical flow regimes or some small geometry features, but I could not see the obviously bad mesh quality there in naked eyes. I located the maximum aspect ratio or volume ratio as suggested in this forum, and didn't found they reside where the maximum residuals occurred.

I do think mesh quality is where my problem lies.

Some people said the sudden transition from last prism to first tetra could be a source of poor convergence. In ICEM-CFD, I made my prism layers by first extruding one layer with a fixed height, and then splitting single layer into multi-layers, given the ratio and number of layers. Will it cause the volume ratio change problems Could anyone share with me the experience in generating prisms? Are there any general guideline in generating good prisms and tets?

If I found some mesh elements with unexpected qualities, what can I do to fix them other than the time-consuming global smoothing?

Attached Mesh Statistics:

+--------------------------------------------------------------------+
| Mesh Statistics |
+--------------------------------------------------------------------+
| Domain Name | Orthog. Angle | Exp. Factor | Aspect Ratio |
+----------------------+---------------+--------------+--------------+
| | Minimum [deg] | Maximum | Maximum |
+----------------------+---------------+--------------+--------------+
| airplane | 7.2 ! | 7688 ! | 374 ok |
+----------------------+---------------+--------------+--------------+
| | %! %ok %OK | %! %ok %OK | %! %ok %OK |
+----------------------+---------------+--------------+--------------+
| airplane | <1 3 97 | 1 15 84 | 0 4 96 |
+----------------------+---------------+--------------+--------------+

Sorry Again for so many question here for I struggle with convergence for weeks.
Attached Images
File Type: jpg residuals.jpg (43.9 KB, 52 views)
File Type: jpg monitor_points.jpg (42.4 KB, 39 views)
everest is offline   Reply With Quote

Old   May 4, 2010, 18:51
Default
  #2
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
Not sure exactly what the problem is, but I can make a few suggestions:
1) Improving mesh quality will often help in complicated geometries like this, especially when you are looking for subtle effects like stall points. In the region of unphysical separation, can you chop this bit out and do a hex mesh in it? Or maybe do a very deep prism layer such that the prism layer extends way past the separation bubble.

2) The maximum expansion factor of 7688 is a worry and aspect ratio of 374 is not good either. I suspect fixing these very poor elements will help.

3) You might also find improvement with the new high order turbulence numerics. Try activating that.
ghorrocks is offline   Reply With Quote

Old   May 12, 2010, 16:27
Default
  #3
Member
 
Luis Filipe Fabiani
Join Date: Apr 2009
Posts: 43
Rep Power: 8
lffabiani is on a distinguished road
Everest,

I beleive that lowering the time step will improve your soluton, but if you lower the time step too much, the solver will catch some phenomenons that are not steady-state (like vortices, and stuff)

Try changing the mesh as ghorrocks told you (lower the expantion angle), and try again.

ALso, pay atention to the out file, when you end a run the solver will output the location of the maximum residues... I think that will help you refine the mesh.

Best regards
lffabiani 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
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Gambit Mesh quality TOM FLUENT 1 February 8, 2002 08:00
Gambit problems Althea FLUENT 21 February 6, 2001 08:05


All times are GMT -4. The time now is 23:33.