CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] CGNS mesh failing in CFX (http://www.cfd-online.com/Forums/ansys-meshing/85119-icem-cgns-mesh-failing-cfx.html)

siw February 17, 2011 15:26

[ICEM] CGNS mesh failing in CFX
 
1 Attachment(s)
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

CycLone February 23, 2011 10:08

Follow step number 3 recommended in the solver output.

Ludvik February 23, 2011 11:56

The symmetry plane isn't planar exactly. Check positon of nodes on this plane (is it very, very small deviation).

PSYMN March 14, 2011 14:52

Move Nodes => Exact => Position
 
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 March 14, 2011 14:53

Dez
 
1 Attachment(s)
Oops, I forgot to attach this...


All times are GMT -4. The time now is 15:39.