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

error in fluent

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 29, 2009, 07:51
Default error in fluent
  #1
Member
 
sivaramakrishnaiah
Join Date: Mar 2009
Location: india,pondicherry
Posts: 74
Rep Power: 8
sivarama1 is on a distinguished road
Send a message via MSN to sivarama1 Send a message via Yahoo to sivarama1 Send a message via Skype™ to sivarama1
hi all,

whats meaning,
divergence detected in AMG solver: w-swirl ,not converging.
Error Object: ()
__________________
sivaramakrihnaiah
sivarama1 is offline   Reply With Quote

Old   October 29, 2009, 08:57
Lightbulb grid - bc - numerics
  #2
New Member
 
Volker Pawlik
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 8
Volker P. is on a distinguished road
Quote:
Originally Posted by sivarama1 View Post
hi all,

whats meaning,
divergence detected in AMG solver: w-swirl ,not converging.
Error Object: ()
That means that there is s.th. wrong with your case:
1. A problem with the grid (resolution, too big size ratios, too high skewness..)

2. Boundary conditions are posed in a bad way: e.g. you want to model a water flow but you forgot to change the material, or - happens very often - you forgot to scale the model from mm to m...

3. A problem due to numerics:
a) If you use the segregated solver (pressure based) try to reduce your under relaxation parameters (momentum to 0.3 pressure 0.1 k-eps 0.4; energy 0.95 ..) and observe the residuals; maybe go one step further and try to get a "first" solution with 1st order discretization instead of second/third and then switch to 2nd again.

b) If you use the coupled solver (new terminology: density based): try to lower the CFL number (but I think, AMG corresponds to the pressure based solver only..)

w-swirl..: indicates that you're a running a 2d-job? Then try fisrt to reduce w-swirl if it is imposed to the system by you. Increase it parallel to the converging solution.
Volker P. is offline   Reply With Quote

Old   October 29, 2009, 10:10
Default grid - bc - numerics
  #3
Member
 
sivaramakrishnaiah
Join Date: Mar 2009
Location: india,pondicherry
Posts: 74
Rep Power: 8
sivarama1 is on a distinguished road
Send a message via MSN to sivarama1 Send a message via Yahoo to sivarama1 Send a message via Skype™ to sivarama1
Hi volker,
Thankyou for replay

i am simulating Tesla turbine one single blade .
please your mail ID will give,i want send my file,and some clarifications.
Thnakyou
__________________
sivaramakrihnaiah
sivarama1 is offline   Reply With Quote

Old   October 30, 2009, 03:23
Default
  #4
New Member
 
Volker Pawlik
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 8
Volker P. is on a distinguished road
Hi sivirama1,
I regret, but I won't have the time to look closely on your case, since I am completely occupied with my own work. Better is to contact your provider. If you can't then at first try to work through the 3 points I mentioned earlier : 1.grid - 2.boundary conditions - 3.numerics Follow that order!

If you are modelling one blade only, you should have periodic boundary conditions in your model? Are they really periodic? i.e. Did you really choose rotational periodic?? Where did you define the periodicity? Inside fluent or outside in your grid generator? If the latter then try to define them via TUI (Text user interface) /grid/modify-zones/make-periodic (I think in fluent 12 it should be mesh instead of grid; noone except for the Ansys managers knows why they changed it..)
AND: You must define the correct rotation axis. This is done in the cell-zone bc panel where you also define your motion. I am not sure but it might be necessary too to define that zone as a reference zone under report "reference values". The last is at least necessary to postprocess your results relative to your rotation.

I hope this helps a little bit. Unless answer again or contact your key user or provider.
Volker P. 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
Stopping a Fluent batch job AND saving the data! Possible? Volker Pawlik FLUENT 7 May 22, 2014 22:30
Two questions on Fluent UDF Steven Fluent UDF and Scheme Programming 4 September 20, 2013 16:30
Problems in lauching FLUENT Lourival FLUENT 3 January 16, 2008 17:48
FLUENT versions ... Gautam FLUENT 3 November 1, 2007 11:49
Run Fluent in batch mode Shengping LUO FLUENT 2 October 24, 2000 05:42


All times are GMT -4. The time now is 06:47.