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

Help Urgent about changing boundary condition

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 10, 2006, 18:45
Default Help Urgent about changing boundary condition
  #1
Anjum Naveed
Guest
 
Posts: n/a
hi all i want to know that how can i change a boundary condition in fluent i have given the boundary condition of wall when i was meshing in gambit and then run my simulation in fluent now i want to run DPM model on the pre developed flow field. but there are only three option for particle when they strike with wal reflect absorb or split. now my prob is that i want to reflect particles from some area of wall and absorb in some area but fluent consider the whole area as on wall as i had given the boundary condition in first. my question is can i change this one wall into two or three walls in fluent or i have to construct geometry again and there give boundary condition of wall at differnt areas and run simulation again. please help me out thanx Anjum
  Reply With Quote

Old   August 11, 2006, 03:18
Default Re: Help Urgent about changing boundary condition
  #2
Raj Kiran Grandhi
Guest
 
Posts: n/a
Look into Grid->Separate->Faces and Grid->Separate->Cells

Also see the FLUENT user manual on these topics.
  Reply With Quote

Old   August 11, 2006, 07:17
Default Re: Help Urgent about changing boundary condition
  #3
Jason
Guest
 
Posts: n/a
Instead of running the whole simulation from scratch, you could also do file->interpolate and write the solution (make sure to write ALL of the variables) of the current setup. Then re-create the geometry in Gambit (this will give you more control of the walls you want to change) and interpolate the old solution onto the current mesh (file->interpolate). Re-iterate a little (depending on how similar your mesh is it could be a couple dozen or a few hundred) to make sure the solution took onto the new mesh.

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

Old   August 12, 2006, 11:01
Default Re: Help Urgent about changing boundary condition
  #4
ANJUM NAVEED
Guest
 
Posts: n/a
thanks for your help

  Reply With Quote

Old   August 12, 2006, 13:03
Default Re: Help Urgent about changing boundary condition
  #5
ANJUM NAVEED
Guest
 
Posts: n/a
hi i am anjum. thanks for ur advice but can u give some detail how to impliment interpoaltion function because i tried first save file than with new mesh i set every thing and instead of initializing i read interpolation file that i stored before and than start iteration but it did not work. Also separate face did not work Anjum
  Reply With Quote

Old   August 14, 2006, 07:50
Default Re: Help Urgent about changing boundary condition
  #6
Jason
Guest
 
Posts: n/a
About the separate face... what do you mean it didn't work? Are you talking about you redid the geometry in Gambit and didn't get an extra face? Then you didn't define your wall BCs in Gambit, you didn't build your geometry correctly, or you didn't read the correct mesh back into Fluent. What exactly did you do (what steps did you perform), and what were the results (were there any errors).

About interpolating the data... what do you mean it didn't work? What happened when you tried interpolating the data?

Jason
  Reply With Quote

Old   August 14, 2006, 12:13
Default Re: Help Urgent about changing boundary condition
  #7
ANJUM NAVEED
Guest
 
Posts: n/a
hi sorry i mixed it up in my previous mail. separate>face did not work was message for raj kiran. and for interpoaltion i saved my interpolation file . created a new mesh in gambit as i desired. than give all the BC and model to the new mesh but i did not inialize it rather i read my interpolated file at this time. my simualtion (i think) was inialized with this file automatically after ward when i start iteration it gave the message invalid argument[2]: wrong type [not a number] and stopped. any suggestions thanks Anjum
  Reply With Quote

Old   August 14, 2006, 12:25
Default Re: Help Urgent about changing boundary condition
  #8
Jason
Guest
 
Posts: n/a
Well, as for splitting the surface, you have to mark the cells first(Adapt->Region... don't Adapt, instead select "Mark" to mark the cells). Mark the cells in the area you want to split, then you can separate by "mark".

As for the interpolation problem, it could be different things. I forgot to mention to make sure your geometry is in about the same XYZ location and is the same scale. Fluent interpolates the values from the original XYZ locations to the current XYZ locations, and if you've shifted your geometry, then you could be interpolating to completely different areas (if you shift an airfoil forward, all of a sudden the LE stagnation point is at the TE of the airfoil, and the TE stagnation point is out in space). Also, before you read in the interpolation file go to Solve->Initialize and set your initialization values. Make sure you click "Apply" to store the values. You don't have to actually initialize though. What happens is that Fluent will interpolate the old solution onto the new geometry and then any variables that are missing will be filled in using the values you stored in the initialize panel. If you didn't set these values then it could've set the default pressure (0pa) which would've causes a NaN for compressible flow.

Also, make sure you set all the variables in the original interpolation file (Fluent will list each variable as it's being written to or read from an interpolation file).

Another thing that could be a problem is if there's a big difference between the setups you've done. If you make a large change on the BCs for example, this could cause a problem.

Hope this helps, and good luck, Jason
  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
Wind turbine simulation Saturn CFX 34 October 16, 2014 05:27
Mixed/Robin boundary condition aaev OpenFOAM Bugs 2 December 15, 2011 15:03
Changing the name of a boundary condition produces errors jorkolino OpenFOAM Bugs 2 January 6, 2011 04:14
CFX Solver : Sudden crash Hervé CFX 2 June 16, 2008 06:40
How to set boundary condition in Fluent for the fo Peiyong FLUENT 1 November 10, 2006 12:44


All times are GMT -4. The time now is 17:11.