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

Symmetry conditon Error in CFX with hex mesh generated by ICEM CFD

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

Like Tree3Likes
  • 1 Post By Thomas MADELEINE
  • 1 Post By RicochetJ
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   October 22, 2014, 21:25
Default Symmetry conditon Error in CFX with hex mesh generated by ICEM CFD
  #1
New Member
 
Mason
Join Date: Sep 2014
Posts: 16
Rep Power: 2
Mason liu is on a distinguished road
Hi,

I encountered a error when start simulation with CFX. This error's description said that 'the mesh face set to a symmetry condition should be a plane or a axis, but my mesh face is not in a plane.'

This is really confused me, the mesh is generated by ICEM CFD with block method, all hex bricks. But how can the mesh on a certain face is not in a plane?

Can you help me with this? Please give any comments or whatever about this, thanks a lot.
Mason liu is offline   Reply With Quote

Old   October 23, 2014, 03:35
Default
  #2
Senior Member
 
Thomas MADELEINE
Join Date: Oct 2014
Posts: 122
Rep Power: 2
Thomas MADELEINE is on a distinguished road
Hi,
when you define a block you usually need a geometry to be glued to it. then you need to move the verticle to the extremity of your geometric plane...
But even with all this some mistakes can occur during the meshing step if your mesh is a little to coarse...

The best thing to do is to specify a larger tolerance inside CFX-Pre by
right-click on solver
insert => expert parameter
Discretization panel (the first one)
activate vector parallel tolerance and set a value of 5 (for instance)
(you can check in CFX Help to have more explanation of this parameter)
re-run your case

it will decrease the tolerance of CFX to consider some surface as a plane
Mason liu likes this.
Thomas MADELEINE is offline   Reply With Quote

Old   October 23, 2014, 05:30
Default
  #3
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 289
Rep Power: 6
RicochetJ is on a distinguished road
Quote:
Originally Posted by Thomas MADELEINE View Post
Hi,
when you define a block you usually need a geometry to be glued to it. then you need to move the verticle to the extremity of your geometric plane...
But even with all this some mistakes can occur during the meshing step if your mesh is a little to coarse...

The best thing to do is to specify a larger tolerance inside CFX-Pre by
right-click on solver
insert => expert parameter
Discretization panel (the first one)
activate vector parallel tolerance and set a value of 5 (for instance)
(you can check in CFX Help to have more explanation of this parameter)
re-run your case

it will decrease the tolerance of CFX to consider some surface as a plane


I wouldn't do this. Instead I would invest time tidying your mesh.

A good quality mesh, with edges appropriately assigned to curves, faces to surfaces etc can really enhance your mesh, and hence solution.

You should use expert parameters as a last resort. Fixing your mesh is the first resort.

Your mesh issues your having can be signs of other underlying mesh issues.
Mason liu likes this.
RicochetJ is offline   Reply With Quote

Old   October 23, 2014, 07:08
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
+1 for Mr CFD.

Don't patch over the problem by allowing a larger tolerance - the tolerance is there for a reason. It is bound to cause other errors as well. Fix the root cause as Mr CFD says.
Mason liu likes this.
ghorrocks is offline   Reply With Quote

Old   October 24, 2014, 04:53
Default
  #5
New Member
 
Mason
Join Date: Sep 2014
Posts: 16
Rep Power: 2
Mason liu is on a distinguished road
Thanks a lot, you all, really appreciate your comments all.

I have assigned all edges to curves from memory, but maybe there are still some other lines, faces or vertexes not been well associated. I'll have a good check in ICEM CFD.

And can I find this mesh problem in ICEM CFD? with some certain mesh check method? Because I want to find this problem early, not to find this until do CFX simulation. I do mesh at home and then do simulation in my office ,so I want find this at home, then to modify.\

Thank you all.
Mason liu is offline   Reply With Quote

Old   October 24, 2014, 05:33
Default
  #6
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 289
Rep Power: 6
RicochetJ is on a distinguished road
Yes, in ICEM go to:
1) Edit Mesh tab
2) Check Mesh icon (it's the green box with a tick)
3) Check your mesh for all errors and possible problems.

The best thing to do is ask in the ICEM forums. They're more knowledgeable about these things than I am.

Make sure you associate your vertices to points, edges to curves, faces to surfaces etc. If you then snap project vertices and then update sizes in pre-mesh params then I think you should be fine.
RicochetJ is offline   Reply With Quote

Old   October 28, 2014, 03:55
Default
  #7
New Member
 
Mason
Join Date: Sep 2014
Posts: 16
Rep Power: 2
Mason liu is on a distinguished road
Thanks a lot for your all help.

End up with that I involved 2 face into 1 symmetry condition before, that's the problem, obviously the mesh face not lie in one single plane.
Because I was used to deal with symmetry boundary condition in CFX with mesh from internal mesh module, there is no problem when 2 face in one symmetry condition, BCZ CFX knows that the two faces are symmetry face respectively.

Thank you all.
Mason
Mason liu is offline   Reply With Quote

Old   May 22, 2015, 06:54
Default
  #8
Member
 
Join Date: Dec 2012
Posts: 59
Rep Power: 4
pizzaspinate is on a distinguished road
Hey Mason,

I am facing the same issue as you did. How did you figure out that you assigned faces wrong?

Thank you
pizzaspinate is offline   Reply With Quote

Old   May 29, 2015, 09:53
Default
  #9
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 470
Rep Power: 10
singer1812 is on a distinguished road
Simple to fix in ICEM.

From CFX you should know the plane that is giving you trouble. Go back into ICEM and into "Edit Mesh"

Move nodes on your sym plane. You can snap them to a uniform plane location.

I am assuming you dont have gross errors in your mesh build and this is just a result of a small offset of node(s) on the offending plane(s).
singer1812 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
--> FOAM FATAL ERROR: Trying to specify a boundary face A.A. OpenFOAM Native Meshers: blockMesh 26 November 26, 2014 11:38
This mesh contains patches of type empty but is not 1D or 2D oric OpenFOAM Running, Solving & CFD 35 March 8, 2014 19:37
[ANSYS Meshing] Question about ICEM mesh output to CFX lnk ANSYS Meshing & Geometry 0 July 27, 2012 15:39
How to create a mesh use ICEM in CFX? little stone CFX 3 July 17, 2012 19:33
Transport mesh from ICEM CFD, to Fluent, to Sysnoise Wieland FLUENT 2 April 15, 2012 06:28


All times are GMT -4. The time now is 12:09.