CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...

Ccm26tofoam problems

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 26, 2007, 10:51
Default Hi I am trying to import
  #1
New Member
 
abhishek k n
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 16
Rep Power: 9
knabhishek is on a distinguished road
Hi

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:
16
(
13595581
13598892
12444508
11638869
13324323
11638873
13601768
11638874
11638868
13551335
12466029
679059
11638876
679057
12466028
13600671

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

Bye,
abhishek
knabhishek is offline   Reply With Quote

Old   June 26, 2007, 14:46
Default 1. The converter should write
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 17
mattijs is on a distinguished road
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.
mattijs is offline   Reply With Quote

Old   June 27, 2007, 04:42
Default Hi Mattijs The format for c
  #3
New Member
 
abhishek k n
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 16
Rep Power: 9
knabhishek is on a distinguished road
Hi Mattijs

The format for cellset command is

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

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

Bye,
abhishek
knabhishek is offline   Reply With Quote

Old   June 27, 2007, 04:49
Default Re: Upper-triangle error messa
  #4
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 779
Rep Power: 19
olesen will become famous soon enough
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.
olesen is offline   Reply With Quote

Old   June 28, 2007, 06:19
Default Hi Mattijis I used setSet
  #5
New Member
 
abhishek k n
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 16
Rep Power: 9
knabhishek is on a distinguished road
Hi Mattijis

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

Bye,
abhishek
knabhishek is offline   Reply With Quote

Old   June 29, 2007, 02:50
Default Hi Mattijis Thank you...
  #6
New Member
 
abhishek k n
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 16
Rep Power: 9
knabhishek is on a distinguished road
Hi Mattijis

Thank you...

I was able to view the cells in parafoam

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

bye
abhishek
knabhishek is offline   Reply With Quote

Old   June 29, 2007, 08:45
Default As I mentioned, the upper-tria
  #7
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 779
Rep Power: 19
olesen will become famous soon enough
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:

olesen is offline   Reply With Quote

Old   July 6, 2007, 11:34
Default HI Is it possible to do som
  #8
New Member
 
abhishek k n
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 16
Rep Power: 9
knabhishek is on a distinguished road
HI

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.
knabhishek is offline   Reply With Quote

Old   April 15, 2014, 08:37
Default
  #9
New Member
 
Richel Bilderbeek
Join Date: Nov 2013
Posts: 14
Rep Power: 4
assert is on a distinguished road
Quote:
2. Upper-triangular : discussed on this board before.
Here: Upper triangular face order
__________________
I will never accept a 'Friend' request, I will always accept beer
assert 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
OF15 libccmio and thus ccm26ToFoam do not compile henry OpenFOAM Bugs 29 July 21, 2011 17:23
Wmake ccm26ToFoam compilation problem under Ubuntu x64 810 kprzysowagmailcom OpenFOAM Installation 7 November 6, 2009 05:33
Problems with Fluent on simple 1D problems agg FLUENT 3 November 21, 2008 12:55
Problems in CFX 5.5.1 Sulviyanti CFX 6 February 7, 2003 17:46
Vr problems Mark Phoenics 3 June 18, 2002 09:31


All times are GMT -4. The time now is 04:22.