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

New boundary zones ?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 10, 2005, 11:52
Default New boundary zones ?
  #1
largeeedysimulation
Guest
 
Posts: n/a
Is it possible to create new boundary zones in FLUENT ?

Without using Gambit, I'd like to split a wall zone into several smaller wall zones.

  Reply With Quote

Old   August 10, 2005, 12:13
Default Re: New boundary zones ?
  #2
Jason
Guest
 
Posts: n/a
Sure... one way is to "mark" some cells as if you were going to adapt the cells... Adapt->Region... but instead of clicking "adapt" click "mark"... then you can go to Grid->Separate->Faces and split the face by the marked region. Another way is to split by angle... lets say you have two surfaces that come together at an XX° angle but they are defined as a single wall... you can split by XX° in Grid->Separate->Faces (this will find any cells on the chosen BC where the vector normal of faces are XX° or greater between them). There are some other options in there as well, but those are the two common ways of splitting a face within Fluent.

Hope this helps, and good luck, Jason
  Reply With Quote

Old   August 10, 2005, 14:50
Default Re: New boundary zones ?
  #3
largeeedysimulation
Guest
 
Posts: n/a
Thanks Jason.

Some zones are separated based on your comments while this method was not working some other zones with errors.

What other methods could be used for the following error happens? Error: Separate_Face_Thread: zone contain hanging nodes/interface faces
  Reply With Quote

Old   August 10, 2005, 15:36
Default Re: New boundary zones ?
  #4
Jason
Guest
 
Posts: n/a
Well, which do you have, hanging nodes on the face (this can happen when you adapt the mesh) or an interface face that contacts the face you want to split?

If it's hanging nodes, then I'm not sure how to split it... the only thing I can think of is if you saved the case and data just before you adapted the mesh, then you can go back to this and split the face, then adapt it the same way you did... hopefully the adaption creates the same number of cells, so now you can save this new case (with the split face and adapted mesh) and if the mesh was adapted exactly the same way, then you can open the most recent data file into this new case and it should work... if it comes back with an error its because there's a different number of cells created during adaption than previously.

If it's an interface, then what you can try is: save the case and data file. Delete the interface you defined (Define->Grid Interfaces) and redefine the "interface" faces as "walls"... then split your face the way you want... then redefine the "wall" faces as "interface" and re-define your interface (Define->Grid Interfaces). Save the case and data file with a new name just in case something went weird when you deleted the interface. You may even want to consider re-opening the data file you saved earlier into the new case and iterating a little bit to make sure it worked.

Actually, in either case you may want to iterate it at least a few iterations to make sure nothing weird happened.

Hope this helps, and good luck, Jason
  Reply With Quote

Old   August 10, 2005, 18:28
Default Re: New boundary zones ?
  #5
largeeedysimulation
Guest
 
Posts: n/a
The main reason of splitting zones was to visualize and get results from droplets trapped in the zones. My simulation is on the wind-induced-rain-drop-behavior around a building using DPM. After simulation, I realized that the current zones are too large to get details of rain-drop-flow-rates trapped in the surface. So I tried to split the zones into smaller zones. But it was failed due to the hanging nodes.

After mesh adaptations,the new case and data files are saved and old case files are deleted. Unfortunately, I can not go backward. I decided to mesh again using Gambit. I will run Fluent with this new mesh file and will not use hanging grids during mesh adaptations.

Thank you for your answers.
  Reply With Quote

Old   August 11, 2005, 01:36
Default Re: New boundary zones ?
  #6
zxaar
Guest
 
Posts: n/a
well one thing u sure can do, go to file->interpolate

and write the calcuations u have done so far, create the new mesh and read this interpolation data (from file->interpolate), you will start exactly where you left( though when u will start iterating for some iteration fluent will adjust but then it will be okey).
  Reply With Quote

Old   August 11, 2005, 08:19
Default Re: New boundary zones ?
  #7
Jason
Guest
 
Posts: n/a
I agree with zxaar. This will at least recover the time you spent iterating the previous model.

Good luck, Jason
  Reply With Quote

Old   August 11, 2005, 10:43
Default Re: New boundary zones ?
  #8
largeeedysimulation
Guest
 
Posts: n/a
Thank you for your kind answers, Jason and zxaar. Last night I started remeshing the domain and run Fluent (steady state simulation). After 1000 iterations, I got a reasonable converged results. Employing DPM, I found that the rain-droplets are trapped on the surface of a building. I have to calculate LIF (local intensity factor) based on the undisturbed rain amount. Zxaar, I will have a chance to use your method next time. Thanks for your advice.
  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
Implementation of boundary conditions for FVM Tom Main CFD Forum 7 August 26, 2014 05:58
External Radiation Boundary Condition (Two sided wall), Grid Interface CFD XUE FLUENT 0 July 8, 2010 06:49
boundary zones Vinod FLUENT 2 November 16, 2004 06:16
Boundary conditions? Tom Main CFD Forum 0 November 5, 2002 02:54
Boundary Conditions Jan Ramboer Main CFD Forum 11 August 16, 1999 08:59


All times are GMT -4. The time now is 20:30.