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

CFX, 2 dimensional flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 21, 2003, 19:12
Default CFX, 2 dimensional flow
  #1
Beno
Guest
 
Posts: n/a
Hi!

I have an assignment to simulate flow in two dimensions. Is that possible with CFX 5.5.1, and how do you do it?

Thx!
  Reply With Quote

Old   December 22, 2003, 06:18
Default Re: CFX, 2 dimensional flow
  #2
Bob
Guest
 
Posts: n/a
Hi Beno, Yes it is possible, but it depends upon your geometry as to how best to approach the problem. If the geometry is nice and simple (assuming you do not have lots of meshing experience), I'd use a structured mesh which can easily be defined as 1 cell deep. On the boundaries of the 3rd dimension you have to specify symetry planes. Now if your geometry is more complex then you may well have to use the unstructured mesher. But that will give you 3D cells. So to get a truely 2D mesh you need to create a 3D mesh, define GGI boundaries rather than a symetry planes on your 3rd dimension, and then invoke an enviroment variable to tell the solver to extrude one of the GGI surface mesh's through to the other boundary.

Unfortunately, I can't remember which enviroment variable it is, plus I'm not 100% sure that the GGI is the correct definition, it may be a periodic pair ? sorry. But the long and short of it is that you can do 2D runs. May be some one else can clarify the last points for you. Have you done a search on the CFX comunity site, as I'm sure there is help there either in an FAQ or just a regular querrie.

Good Luck

Bob
  Reply With Quote

Old   December 22, 2003, 09:43
Default Re: CFX, 2 dimensional flow
  #3
Bob
Guest
 
Posts: n/a
Hi Beno, the enviroment variable is: CFX5_2D_MESH set this to be TRUE.

To return to 3D meshing you will need to rempove this variable. The boundary condition you need to apply is a periodic pair. This should then create a 2D mesh when the def file is created.

Hope this is a little more clear now ? Bob
  Reply With Quote

Old   December 25, 2003, 03:01
Default Re: CFX, 2 dimensional flow
  #4
Jeff
Guest
 
Posts: n/a
If it's truely 2D (no flow in the third direction) you don't need the GGI. Simply use the symmetry planes.

If there's rotational flow (2D axysymmetric) then you can still do this without a GGI. Use the paver option for meshing and pave quads over your 2D face. Then sweep these elements 1 cell thick in the Z direction. This gives hexes which match up on the high and low Z faces and can be set as symmetry planes.

Jeff
  Reply With Quote

Old   December 30, 2003, 17:00
Default Re: CFX, 2 dimensional flow
  #5
Ron
Guest
 
Posts: n/a
CFX is point based. Aren't two cells required for the thickness? (i.e. points in the middle)

With one cell thick, there are only points on the symmetry planes.

Not sure.

-Ron
  Reply With Quote

Old   January 4, 2004, 18:26
Default Re: CFX, 2 dimensional flow
  #6
Glenn Horrocks
Guest
 
Posts: n/a
Hi Ron,

The 2D simulations work fine with just one cell in the thickness. Done it many times.

Glenn
  Reply With Quote

Old   January 5, 2004, 11:29
Default Re: CFX, 2 dimensional flow
  #7
Ron
Guest
 
Posts: n/a
Thanks Glenn!
  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
Flow Analysis tilting Pad thrust bearing using CFX julien CFX 5 April 9, 2014 08:38
[HELP] Slip flow boundary condtion in CFX jeffwmb CFX 20 March 13, 2013 17:21
Ansys 11.0 CFX - solving electric potentials and multiphase flow cfd_multiphyiscs CFX 2 March 10, 2010 14:43
Different flow pattern between OpenFOAM and CFX AirS OpenFOAM 0 January 12, 2010 08:08
demo free flow blunt body in cfx ansys 11 jan CFX 1 July 31, 2007 19:44


All times are GMT -4. The time now is 13:50.