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

How to specify a value on a this surface?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 30, 2003, 10:29
Default How to specify a value on a this surface?
  #1
windhair1
Guest
 
Posts: n/a
I'd likt to specify some value on a thin surface inside a flow domain, hope it is possible. For example, temperature on the thin surface is fixed. I urgent need your guys help. Thanks

windhair1
  Reply With Quote

Old   September 30, 2003, 15:44
Default Re: How to specify a value on a this surface?
  #2
fly
Guest
 
Posts: n/a
define where you want to put data
  Reply With Quote

Old   October 1, 2003, 04:40
Default Re: How to specify a value on a this surface?
  #3
windhair1
Guest
 
Posts: n/a
The command file is like

>>CREATE PATC PATCH TYPE 'THIN SURFACE' PATCH NAME 'INTERWALL' BLOCK NAME 'FUELBLOCK' HIGH I PATCH LOCATION 17 17 1 40 1 1 END

Add in USRSRC

CALL IPALL('INTERWALL', '*', ......)

DO 100 I = 1, NPT

INODE = IPT(I)

VARBCS(ISCA2, IPHASE, INODE) = 1.0 100 CONTINUE

But the results show zero value of scalar2 in whole fluid domain.

How to deal with it?

Thanks
  Reply With Quote

Old   October 9, 2003, 21:18
Default Re: How to specify a value on a this surface?
  #4
Jeff
Guest
 
Posts: n/a
First of all, you need to use USRBCS to access the VARBCS array (USRSRC is for setting SU and SP). If you are actually in USRBCS, you have to set the IUBCSF flag (see top of routine) to indicate whether the condition is constant, changing with iteration, or changing with timestep.

Secondly, how are you defining ISCA2? Accessing the scalar arrays is a bit tricky. Try something like:

CALL GETVAR('USRBCS','SCAL ',ISCAL)

CALL GETSCA('USER SCALAR2',IS2,CWORK)

ISCA2 = ISCAL + IS2 - 1

CALL IPALL('INTERWALL', '*','PATCH',

+ 'CENTERS',IPT,NPT,CWORK,IWORK)

DO I = 1, NPT

INODE = IPT(I)

VARBCS(ISCA2, IPHASE, INODE) = 1.0

ENDDO

Note that scalar 1 is in the 0th position, which is why we subtract 1. Also note the two spaces in the 'SCAL ' string used by GETVAR. All var names in GETVAR are exactly 6 characters padded with spaces.

If this is confusing, call the Pittsburgh CFX support line for a very detailed technical note on CFX-4 User FORTRAN written by some guy named Jeff.

Hope this helps, Jeff
  Reply With Quote

Old   October 10, 2003, 05:44
Default Re: How to specify a value on a this surface?
  #5
windhair1
Guest
 
Posts: n/a
Thanks, It works now. But I still need further help on this topic, refer to the following post.

http://www.cfd-online.com/Forum/cfx.cgi?read=6087
  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
[ICEM] Problems with coedge curves and surfaces tommymoose ANSYS Meshing & Geometry 0 August 5, 2011 16:02
boundaries with gmshToFoam‏ ouafa Open Source Meshers: Gmsh, Netgen, CGNS, ... 7 May 21, 2010 12:43
Error : Self intersecting surface mesh, computing intersections & Error : Impossible velan Open Source Meshers: Gmsh, Netgen, CGNS, ... 0 June 29, 2009 00:48
Problem with Gmsh nishant_hull Open Source Meshers: Gmsh, Netgen, CGNS, ... 17 December 7, 2007 02:33
CFX4.3 -build analysis form Chie Min CFX 5 July 12, 2001 23:19


All times are GMT -4. The time now is 06:45.