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

Diverging wall scale due to large domain size

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 10, 2006, 15:48
Default Diverging wall scale due to large domain size
  #1
Kevin
Guest
 
Posts: n/a
I am modelling a blade profile at a Reynolds number of 700000 in air using the SST turbulence model. My solutions are largely domain size dependent and as such i would like to increase the size of my domain to get a more accurate solution. The problem that i am having is that as i make my domain size larger the solver has a tougher and tougher time solving the wall scale. I am at a stage now where if i make my domain any larger the wall scale function goes to infinity and the solver stops. Any suggestions as to how i can prevent thsi problem??

Thank you in advance Kevin
  Reply With Quote

Old   November 11, 2006, 13:15
Default Re: Diverging wall scale due to large domain size
  #2
Robin
Guest
 
Posts: n/a
Hi Kevin,

The wall scale calculation solves a simple diffusion equation. If it blows up, it is almost invariably due to some bad mesh in your domain. I would check that as you increase your domain size you are not overly distorting the mesh.

Another possiblity, which is easy to check, is if this is due to roundoff error. Try running your case in double precision.

Regards, Robin
  Reply With Quote

Old   November 11, 2006, 13:38
Default Re: Diverging wall scale due to large domain size
  #3
Kevin
Guest
 
Posts: n/a
Thanks for the help Robin. I was wondering how I would go about checking for distortion within my mesh. I have left the meshing technique the same as for previous runs and have only altered the size of the domain. Actually, now that i think of it, i have increased the maximum face spacing in order to maintain a reasonable number of nodal points. Could this be the cause of distortion? My smallest elements at the surface of the blade are approx. .01 mm while at the boundary of the domain they reach a size of approx. 500 mm and I was wondering if this could be causing the complications. Finally, i am not entirely sure how to set the solver to use double precision and i was hopng that you could point me in the right direction.

Thank you again, your support and knowledge is always appreciated.

Kevin
  Reply With Quote

Old   November 12, 2006, 16:48
Default Re: Diverging wall scale due to large domain size
  #4
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

The large range of mesh element sizes is potentially causing a problem with the single precision solver I strongly recommend you try double precision.

You can run the double precision solver by going to the advanced options on the solver manager when you start a run up, or if using the command line you can use the switch -double

Regards, Glenn Horrocks
  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
Domain Imbalance HMR CFX 3 March 6, 2011 21:10
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
Need help with the error cfdproject OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 0 April 14, 2009 15:45
Phase locked average in run time panara OpenFOAM 2 February 20, 2008 15:37
code for large scale fluid induced movement sb Main CFD Forum 0 April 27, 2007 15:42


All times are GMT -4. The time now is 02:10.