# Symmetry plane error in solver

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 January 29, 2007, 19:32 Symmetry plane error in solver #1 Santiago Orrego. Guest   Posts: n/a Hello Guys. Im analysin a 3D wing. In first place, I created the mesh in ICEM CFD with a spacing=1 in the wing zone. Then I run the Pre, then the solver and no problem. It runs ok. But then I reduced the spacing to =0.1 and Im having problems with the solver. I load the mesh in PRE and all the BC and Pre conditions normal, but when the solver starts it show an 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 1 in the | | symmetry boundary patch | | | | TAPER WING Default | | | | 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. Any idea to solve this? Thanks a lot Santiago

 January 29, 2007, 22:05 Re: Symmetry plane error in solver #2 Johnny Guest   Posts: n/a Have you tried the three suggestions provided to you by the solver? One of them will likely work.

 January 30, 2007, 00:34 Re: Symmetry plane error in solver #3 Paul Guest   Posts: n/a Hi Santiago, I encountered this problem once. As Johnny said try with the suggestions in the users manual. for me it worked fine when i defined separate parts for different symmetry faces instead of clubbing all of them under a single part name in ICEM. Do let us know what resolved your problem Regards Paul

 January 30, 2007, 02:29 Re: Symmetry plane error in solver #4 Daniel Guest   Posts: n/a Dear Santiago! I also had similar problems. The solution was to check the mesh at the symmetry planes. It is likely that there are nodes which are not exactely located in the symmetry plane. When you find these nodes, they can be projected back into the symmetry plane in icem under the edit mesh tab. Good Luck Daniel

 January 30, 2007, 08:06 Re: Symmetry plane error in solver #5 Santiago Orrego. Guest   Posts: n/a Johnny, Paul, Daniel, thanks a lot for the answer. I solved the problem. In ICEM, i made right click under Pre-Mesh (in the tree), and click "NO projection" and it worked OK. Thanks a lot. Santiago TrII4d likes this.

 January 30, 2007, 23:14 Re: Symmetry plane error in solver #6 eric Guest   Posts: n/a I also trapped by this problem. Rebulid some faces in ICEM, select tolerance 0.00001, that will be OK.

 January 31, 2007, 08:09 Re: Symmetry plane error in solver #7 Santiago Orrego. Guest   Posts: n/a Ok discover another way, and was changing the SYMMETRY condition to a FREE WALL.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post flyingk ANSYS Meshing & Geometry 2 August 16, 2011 06:41 TWaung CFX 2 February 16, 2010 09:11 Matt CFX 2 February 25, 2009 06:41 Roland CFX 3 September 13, 2006 08:38 Roland CFX 7 May 31, 2006 13:34

All times are GMT -4. The time now is 06:16.

 Contact Us - CFD Online - Top