CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... (
-   -   Ccm26tofoam problems (

knabhishek June 26, 2007 10:51

Hi I am trying to import

I am trying to import the ccm++ mesh containing 1.7 million cells.

When i run the check mesh following errors

1. bool primitiveMesh::checkFacePyramids(const bool, const scalar, labelHashSet*) const: face 4891768 points the wrong way.
Pyramid volume: -2.68463e-11 Face 4(13595581 13598892 12444508 11638869) area: 6.5171e-06 Owner cell: 842458
Owner cell vertex labels:

How can i check this cell in starccm is it the number corresponding to Owner cell: 842458 or is it possible in paraview/parafoam

2.bool primitiveMesh::checkUpperTriangular(const bool, labelHashSet*) const :
face 232123 out of position. Markup label: 232122. All subsequent faces will also be out of position. Please check the mesh manually.
--> FOAM Serious Error :
From function bool primitiveMesh::checkUpperTriangular(const bool, labelHashSet*) const
in file meshes/primitiveMesh/primitiveMeshCheck.C at line 1354
Error in face ordering: faces not in upper triangular order!
Writing 1 unordered faces to set upperTriangularFace

what is this error


mattijs June 26, 2007 14:46

1. The converter should write
1. The converter should write a volScalarField "cellType" which gives the ccm cell id. The two should be the same for a compacted mesh.

You could use the 'setSet' application to look at a single cell. E.g.

cellSet c0 new labelToCell (842458)

2. Upper-triangular : discussed on this board before. The error itself should not be there since ccm26ToFoam sorts the faces before writing. If you can generate a small case (<50k cells) that has the same behaviour I don't mind having a look at it.

knabhishek June 27, 2007 04:42

Hi Mattijs The format for c
Hi Mattijs

The format for cellset command is

Usage: cellSet <root> <case> [-parallel]

Command cellSet c0 new labelToCell (842458) is not working.


olesen June 27, 2007 04:49

Re: Upper-triangle error messa
Re: Upper-triangle error message.
I've seen this problem before.
Since the faces are correctly sorted (in ccm26ToFoam), the error indidates something else.

When a cell joins to its neighbour across TWO faces instead of one (eg, when a concave polyhedral cell connects to its neighbour), it messes up the face order checking, but is not a problem.

Of course, if the polyhedra were all correctly convex, or at least not concave, this error would not be reported.

knabhishek June 28, 2007 06:19

Hi Mattijis I used setSet
Hi Mattijis

I used setSet command. It wrote some file in directory VTK and Consatant.
Noe how to look that cell, using ParaFoam.


knabhishek June 29, 2007 02:50

Hi Mattijis Thank you...
Hi Mattijis

Thank you...

I was able to view the cells in parafoam

I will look into Upper-triangular stuff using smaller mesh size


olesen June 29, 2007 08:45

As I mentioned, the upper-tria
As I mentioned, the upper-triangle check might be tripped by concave poly cells.

Here a small mesh subset that illustrates it: concaveCase.tar.gz

With a corresponding screenshot:

knabhishek July 6, 2007 11:34

HI Is it possible to do som

Is it possible to do some mesh cleaning in OF. Like deleting highly skewed faces, smoothing warped faces or rectifying highly non orthogonal faces.

Is it possible to use cell Set command to carry out this kind of operation or may be some other command.

What is basis for non orthogonal corrector range from 0 to 20.

assert April 15, 2014 08:37


2. Upper-triangular : discussed on this board before.

All times are GMT -4. The time now is 15:13.