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

Y* and really large .dat files

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 4, 2003, 11:27
Default Y* and really large .dat files
  #1
Simon Blakey
Guest
 
Posts: n/a
Dear All,

I have been having some problems getting respectable values for y* in my fluent5 modelling. I'd appreciate your thoughts. I have tried successive grid adaptation, but fluent crashes.

I suspect I am at the limits of what my computer RAM or Fluent5 can handle. My files are pretty big already (.cas file = 80MB and .dat file = 400MB)with at least 500 000 nodes, and I can only get a y* value around say 100.

Can I trust the results from the model? Or should I be looking to get a smaller y*?

Thanks,

Simon
  Reply With Quote

Old   August 4, 2003, 12:38
Default Re: Y* and really large .dat files
  #2
ap
Guest
 
Posts: n/a
Instead of using grid adaption, try to create a new mesh on the same geometry in Gambit.

If you need it, you can also import the solution obtained with the old grid, in the new case file.

Adaption tools usually tends to increase nodes number too much.

You could also try to apply a boundary layer to walls in your system.

If you refer to the manual of FLUENT, wall functions are considered valid only if y+ is between 30 and 60. And it's better to have y+ as close as possible to its lower limit.

Hi

ap
  Reply With Quote

Old   August 7, 2003, 04:51
Default Re: Y* and really large .dat files
  #3
Simon Blakey
Guest
 
Posts: n/a
Thanks for the reply ap.

You mentioned that you could import old .dat files onto new grids (of the same overall geometery I presume). How do you go about doing that? I think that such a feature would be almost revolutionary, for my work at least.

Regards,

Simon
  Reply With Quote

Old   August 8, 2003, 09:34
Default Re: Y* and really large .dat files
  #4
ap
Guest
 
Posts: n/a
You can do it using Grid to Grid interpolation function. To do this, you new grid must have the exact geometry of the first. Only the mesh can change.

1) Open your old case.

2) Go to File -> Interpolate.

3) If you want to export all solution data, select all cell zones and all fields.

4) Click on Write to save the data file.

5) Open the new msh file without closing FLUENT, using the text command:

file->reread-grid

6) read the exported data: File-Interpolate...

If zones in the new grid are different or have different numbers, you should first set up the new case file using the new grid, then import the old data.

See the manual looking for: Interpolation in the index, then click on grid-to-grid.

Hi

ap

  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



All times are GMT -4. The time now is 08:54.