CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] CGNS mesh failing in CFX

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 17, 2011, 15:26
Default [ICEM] CGNS mesh failing in CFX
  #1
siw
Senior Member
 
Join Date: Jul 2009
Posts: 444
Rep Power: 14
siw will become famous soon enough
Hi,

I'm not sure if this is an ICEM or a CFX problem.

I downloaded the ANSYS ICEM Hexa mesh of an aircraft in CGNS format from ftp://cmb24.larc.nasa.gov/outgoing/DPW4/ and tried to run a simulation in CFX but I got this error:

+--------------------------------------------------------------------+
| ERROR #002100013 has occurred in subroutine Chk_Splane. |
| Message: |
| The symmetry boundary condition requires that the boundary patch |
| mesh faces form a plane or axis. However, face set 3 in the |
| symmetry boundary patch |
| |
| symm |
| |
| is not in a strict plane, which means that at least one of its |
| faces is not parallel to the others. To make the solver run |
| you can do one of the following: |
| |
| (1) Make sure that this symmetry boundary patch is in a plane or |
| axis by checking and regenerating the mesh. |
| (2) If the symmetry boundary patch is an axis rather than a |
| plane, change the tolerance of the degeneracy check by |
| increasing the value of the Solver Expert Parameter |
| 'degeneracy check tolerance' (the default value is 1.e-4). |
| (3) Increase the value of the Solver Expert Parameter |
| 'vector parallel tolerance' (the default value is 1 deg.). |
| Note that the accuracy of the symmetry condition may decrease |
| as the tolerance is increased. This is because the tolerance |
| is the number of degrees that a mesh face normal is allowed |
| to deviate from the average normal for the entire face set. |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+

Clearly something needs to happen to the mesh. But I would have thought it okay since ANSYS made it for the public to download.

I noticed when I was setting up the CFX boundary conditions that each surface that BoCos are set at was listed twice (see image) but that's not case when viewing the mesh in ICEM.

What needs to be done to get this mesh to work?

Thanks
Attached Images
File Type: jpg 1.jpg (38.3 KB, 30 views)
siw is offline   Reply With Quote

Old   February 23, 2011, 10:08
Default
  #2
New Member
 
Join Date: Mar 2009
Posts: 9
Rep Power: 8
CycLone is on a distinguished road
Follow step number 3 recommended in the solver output.
CycLone is offline   Reply With Quote

Old   February 23, 2011, 11:56
Default
  #3
Member
 
Ludvik Lanicek
Join Date: Apr 2009
Location: Czech Republic
Posts: 52
Rep Power: 9
Ludvik is on a distinguished road
The symmetry plane isn't planar exactly. Check positon of nodes on this plane (is it very, very small deviation).
Ludvik is offline   Reply With Quote

Old   March 14, 2011, 14:52
Default Move Nodes => Exact => Position
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Yes, this can happen some times, usually because the geometry isn't quite planar or for other reasons due to mesh parameters, etc. You may be able to figure out why the mesher is not creating a planar mesh on the symmetry plane and then fix and remesh...

For a mesh editing solution, we usually sort this out by using Edit Mesh (tab) => Move Nodes => Exact => Position.

If it is looking for a reference location, then clear the command.

Choose to modify the dimension that is the problem (for an XY symmetry Plane, you would modify Z) and set it equal to the correct value (Z=0 might be right).

Then select the shell elements that need to be moved into the correct plane. For instance, you might use the "select items in a part" option from the selection tool box and then select the symmetry part.

Then apply. All the nodes of the selected elements will have their X,Y and/or Z values adjusted to the numbers you set (probably Z values adjusted to 0).

I will see if we can make a "planar" check (like the periodicity check) that can detect and solve this problem for you.
PSYMN is offline   Reply With Quote

Old   March 14, 2011, 14:53
Default Dez
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Oops, I forgot to attach this...
Attached Images
File Type: jpg MoveNodes_Exact_Position.jpg (43.6 KB, 46 views)
PSYMN is offline   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] Negative volume error in hybrid mesh siw ANSYS Meshing & Geometry 4 September 3, 2014 05:25
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Create moving mesh without simulating (CFX) spatialtime ANSYS 2 July 22, 2010 10:30
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09
Mesh from ICEM CFD to CFX ! Error ! Why ? Thanks ! Vu Trinh Tuan CFX 11 March 28, 2005 19:04


All times are GMT -4. The time now is 06:02.