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

how to setting this boundary

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 9, 2008, 23:52
Default how to setting this boundary
  #1
tipakorn
Guest
 
Posts: n/a
I divide my model to 2 parts because it's very big and complex. Can I use part A's result be input to another part? And how to set it to part B. Thanks
  Reply With Quote

Old   January 10, 2008, 16:00
Default Re: how to setting this boundary
  #2
DB
Guest
 
Posts: n/a
I can give you an example:

Suppose you have a long pipe and instead of modeling as a whole you divide pipe into 2 parts such that outlet from one part is inlet to another. Run the first piece of model and write out the velocity,temperature etc at the outlet boundary in a tabular format [x,y,z,velocity/temperature] now this data will be input to second piece. Set the user option in inlet boundary in second piece to "user" and then in the user subroutine read the file to define the boundary values.

  Reply With Quote

Old   January 11, 2008, 09:24
Default Re: how to setting this boundary
  #3
James
Guest
 
Posts: n/a
I think you are looking for PMAP.

One way of doing this is to place a set of shells on the downstream model boundary and write them out. You read these into the upstream model, PMAP the data and write it out.

Then using the data files and the ORIGINAL shell file ( the data from the upstream model and the original shell file will be in the correct order and matched, it does not matter that the upstream shell numbers were different during mapping) you write some code that creates one region per face (it should require ~10 lines toi do this). You then ifile/BREAD the files into the downstream model and run it.

Overlapping the models rather than abutting them is preferred.

This process only works well if there is a good low gradient simple flow zone at which to map. Obviously you cannot have recirculation but you also have the issue that while you map the velocity field you do not map the pressure field or more specifically the pressure gradients that were driving the flow (or vice versa).

One check to see if the mapping is valid is to check the quantity (pressure/velocity) that you did not map between the two models. If they are close it's OK if not the mapping plane was not suitable.

I would suggest you map velocity for the highest chance of success.
  Reply With Quote

Old   January 15, 2008, 23:32
Default Re: how to setting this boundary
  #4
tipakorn
Guest
 
Posts: n/a
What is PMAP? I use Star CD V3.26?
  Reply With Quote

Old   January 16, 2008, 09:19
Default Re: how to setting this boundary
  #5
James
Guest
 
Posts: n/a
Did you try help PMAP ?

It maps volume data onto another set of cells, it is a bit like SMAP except you can do a part of a model and in addition you can map volume data onto shells for use with boundary mapping.
  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
VOF and setting boundary conditions dave00001 FLUENT 0 January 25, 2008 13:37
Can someone help me on setting boundary, continuum Michaelkoay FLUENT 0 January 12, 2008 04:28
Need help setting a boundary condition... HSeldon FLUENT 2 August 28, 2006 14:10
UDF for boundary condition setting Luke FLUENT 0 June 1, 2006 04:33
setting variable boundary Mehdi CD-adapco 3 January 31, 2006 05:33


All times are GMT -4. The time now is 13:36.