CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   ERROR #002100013 has occurred in subroutine Chk_Sp (https://www.cfd-online.com/Forums/cfx/21792-error-002100013-has-occurred-subroutine-chk_sp.html)

Forrest November 3, 2005 08:28

ERROR #002100013 has occurred in subroutine Chk_Sp
 
Hi all,

I am using cfx5.7.1 to do a two modelling. I used symmetry boundaries. Because I don't want more cells on the third direction so the physical distance on the third direction is very small (smaller than the larger cell dimension). Ideally, when I was using structured mesh, only one cell along the third direction and now I have to use unstructured mesh due to the geometry reasons.

There was no problem when I was generating the mesh using ICEM and set the boundary conditions in cfx-pre, only when I run it I got this error (see below). I tried to refine the mesh and used the expert parameters it suggested, but it keeps telling me this.

Does this mean I do need more cells on the third direction in order to make the plane to be a 'strict plane'? If there are more cells in the third direction, am I going to have 3D effects for the calculation? I mean, parameters in the third direction won't be uniform as it is assumed to be.

Thanks for your help

Regards Yingchun

Followed the error message:

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 14 in the symmetry boundary patch

SymFluid111

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.


Ivnev555 March 15, 2016 07:33

Hello,
did you fix the problem?

ghorrocks March 15, 2016 08:14

The error this post is about is a simple one. You have to make sure a symmetry plane is actually a plane. The error usually comes about because:
1) You have put multiple symettry planes in one boundary. You need to put them each in their own symmetry plane
2) You have defined a curved surface to be a symmetry plane - you can't do this
or
3) A meshing error has put a few stray elements into a symmetry plane. THis can happen in ICEM with the way it meshes, the fix is to manually check and fix the symmetry plane elements.

Mengjiezhao August 2, 2017 13:55

same problem about symmetry
 
I'm keeping get the following error every time I try to refine the mesh. This time I just increase the Prismen layer number from 6 to 7, and with 6 the solver has worked. I#m wondering if it's because of the thickness of the Domain, i'm calculating a 1,2mx2.85m rectangular Domain with airfoil in it. The thickness of the Domain is only 0.01m. But it also worked for 6 Prismen layer?

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

Symmetry

| 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:

I met this probelm really frequently, not only for the structured mesh but also for the unstructred mesh: I can't see many mesh in wrong boudary surfaces and thus don't know how to fix it manuelly.

Did you fix your Problem now? and how?

ghorrocks August 2, 2017 18:59

Load your model in CFD-Post (or if it did not generate an output file, in your mesher) and find the faces in the symmetry face which are off the plane. It is a very simple error, but it can take some hunting to find the problem elements.


All times are GMT -4. The time now is 15:25.