CFD Online Logo CFD Online URL
Home > Forums > CFX

visualize the initial and/or boundary conditions

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

LinkBack Thread Tools Display Modes
Old   April 28, 2004, 10:10
Default visualize the initial and/or boundary conditions
Posts: n/a
Dear all, IŽd useful any trick to visualize in post the initial conditions or the BC. In complex geometries it is easy to make mistakes or do not set the right (physically right)ones in corners, for example. How do you do it(if you do)?

thanks pi
  Reply With Quote

Old   April 28, 2004, 12:15
Default Re: visualize the initial and/or boundary conditio
Gloria Gaynor
Posts: n/a
Try to set the following expert parameters:
solve fluids = f solve tke eps = f
This will turn off the equation solver (assuming you're using k-epsilon model). Run for 1 iteration only and you'll be able to see your initial conditions. Take a look at the CFX-5/etc/5.6/RULES file and you'll find the suitable expert parameters to turn off the equations for your specific case.
Good luck, G. G.
  Reply With Quote

Old   April 28, 2004, 18:26
Default Re: visualize the initial and/or boundary conditio
Glenn Horrocks
Posts: n/a

There are other ways of doing it which do not require you to do a dummy simulation. For steady state runs you can, just after starting a run press "Backup Run"; or in CFX-Pre you can set it up to output the initial conditions with output control/backup results and set the iteration list to 0.

For transient runs, in CFX-Pre use Output Control/Transient Results, and set the time list to zero.

Regards, Glenn
  Reply With Quote

Old   April 29, 2004, 00:03
Default Re: visualize the initial and/or boundary conditio
Posts: n/a
To visualize the initial condition for a steady state run use the following expert parameter:

backup file at zero =t

This will create a backup file at 0th iteration! ie before the start of the solution so that you can view the initial guess.

IN cfx-5.7 you can visualize the boundary conditions in Pre itself.. I have not tested out the same for initial conditions!
  Reply With Quote


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
Full pipe 3D using icoFoam cyberbrain OpenFOAM 4 March 16, 2011 10:20
MRFSimpleFOAM goes divergenced! renyun0511 OpenFOAM Running, Solving & CFD 0 November 19, 2009 03:11
Computational time sunnysun OpenFOAM Running, Solving & CFD 5 March 16, 2009 04:32
MRFSimpleFoam amp cyclic patches david OpenFOAM Running, Solving & CFD 36 October 21, 2008 21:55
Unknown error sivakumar OpenFOAM Pre-Processing 9 September 9, 2008 12:53

All times are GMT -4. The time now is 01:51.