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

CFX-solver problem??

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 14, 2006, 09:34
Default CFX-solver problem??
  #1
Jesper Sørensen
Guest
 
Posts: n/a
Hey! I have a 2D problem (simulated by a thin 3D problem) were i have got the following error in CFX-solver! But since i have no "free slip" bounderies, can anyone tell me what the problem could be?? The mesh is generated in Icem!

Jesper

"ERROR #002100048 has occurred in subroutine SU_BNEXT. Message: All vertices for a fluid domain lie on a boundary. The solver considers this to be a fatal error because control volume gradients cannot be calculated, leading to serious discretization error. | | This error may arise for two-dimensional simulations when a free slip boundary condition is applied to the end planes. In this situation a symmetry condition should be applied to the end planes instead. Execution is terminating. This error message can be bypassed by setting the expert parameter 'boundary vertex check = f'."
  Reply With Quote

Old   November 14, 2006, 11:25
Default Re: CFX-solver problem??
  #2
Bian
Guest
 
Posts: n/a
Did you set both end planes as symmetry condition?
  Reply With Quote

Old   November 15, 2006, 02:20
Default Re: CFX-solver problem??
  #3
Jesper Sørensen
Guest
 
Posts: n/a
No i did not! I have 3 inlet (top, buttom and front) and an outled at the end, and the sides are set as walls as same as the body! Why should that create the problem?? But you are right - If i set the sides as symmetri the solver has no errors!

Jesper
  Reply With Quote

Old   November 15, 2006, 02:55
Default Re: CFX-solver problem??
  #4
zxaar
Guest
 
Posts: n/a
Execution is terminating. This error message can be bypassed by setting the expert parameter 'boundary vertex check = f'."

this sounds funny to me, if the execution is terminated in next step, what is the use of bypassing the warning. Anyway the solver will come out.

  Reply With Quote

Old   November 15, 2006, 13:58
Default Re: CFX-solver problem??
  #5
Bian
Guest
 
Posts: n/a
If you put wall boundary on the side planes, this is not a 2-D approximation.
  Reply With Quote

Old   November 15, 2006, 21:18
Default Re: CFX-solver problem??
  #6
Robin
Guest
 
Posts: n/a
You can bypass the warning if you set the problem up this way intentionally. Clearly the he did not.
  Reply With Quote

Old   November 15, 2006, 21:19
Default Re: CFX-solver problem??
  #7
Robin
Guest
 
Posts: n/a
Hi Jesper,

If you specify the side walls as "No Slip", there is nowhere for the fluid to go. A two dimensional problem is either symmetric or periodic in the 3rd dimension and requires boundary conditions accordingly.

Regards, Robin
  Reply With Quote

Old   November 16, 2006, 04:57
Default Re: CFX-solver problem??
  #8
zxaar
Guest
 
Posts: n/a
I think the warning means that if you bypass than the solver will not exit, and will try to continue. Then it makes sense, what do you think.
  Reply With Quote

Old   November 17, 2006, 02:32
Default Re: CFX-solver problem??
  #9
HekLeR
Guest
 
Posts: n/a
This can also happen if all the vertices are on boundary conditions like inlets/outlets. I would think this is implied by the first sentence: "All vertices for a fluid domain lie on a boundary".

The example is just a common setup error.

  Reply With Quote

Old   November 17, 2006, 11:05
Default Re: CFX-solver problem??
  #10
Robin
Guest
 
Posts: n/a
Bypassing the warning only makes sense if you had intentionally set the problem up in this manner. Based on what has been stated, the user forgot to specify symmetry planes or periodic interfaces on the side walls. If he fixes this, there will be no warning and no need to bypass it.
  Reply With Quote

Old   November 24, 2006, 00:17
Default my easy way to solve it
  #11
Kiddosuper
Guest
 
Posts: n/a
You can just use local parallel run to cover this problem, I don't know why this will run properly without any warning message by local parallel run.
  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
ERROR #002100056 CFX FSI problem Hongdao CFX 0 November 10, 2010 04:58
CFX Solver Memory Error mike CFX 1 March 19, 2008 08:22
Urgent Problem with Hypermesh and CFX Luk CFX 5 March 14, 2008 05:59
CFX new user, problem with solver and PRE settings Vijesh Joshi CFX 1 March 13, 2006 23:42
CFX 4.4 installation problem Pandu Sattvika CFX 1 December 1, 2001 05:07


All times are GMT -4. The time now is 21:11.