|
[Sponsors] |
Star4ToFoam import boundaries in polyhedral mesh |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
April 5, 2007, 04:15 |
Hi all,
I would like to conve
|
#1 |
Member
|
Hi all,
I would like to convert into Foam a pro-Star4 format mesh. I have done this procedure many times without problems, the peculiarity is that this time the mesh is composed by polyhedral elements. Being a test the chosen mesh is very simple: a single cylinder with inlet, outlet and wall. I found some errors in importing the boundary conditions set up with pro-Star4. The geometry is exactly converted but boundary polymesh fails to be created. Two types of error come out: ... There are 2554 faces to be patched and 237 specified - collect missed boundaries to final patch meshReader::createPolyBoundary(): Problem with face: 6(11916 17960 17961 17962 17963 11917) Probably trying to define a boundary face on a previously matched internal face. Internal face: 6(11916 17960 17961 17962 17963 11917) ... and ... meshReader::createPolyBoundary() : problem with face 1278: addressed 1 times (should be 2!). Face: 6(2011 2012 2013 2014 2015 2016) ... Is there anyone that already found this errors? How did you solve it? Thanks a lot for the help Cosimo
__________________
Cosimo Bianchini Ergon Research s.r.l. Via Panciatichi, 92 50127 Florence - ITALY Tel: +39 055 0763716 Mob: +39 320 9460153 e-mail: cosimo.bianchini@ergonresearch.it URL: www.ergonresearch.it |
|
April 5, 2007, 05:03 |
Hi Cosimo,
Assuming that yo
|
#2 |
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,679
Rep Power: 40 |
Hi Cosimo,
Assuming that you are using the last patch posted here (13 Nov 2006), the following mini-patch should help solve the problem. The culprit is the incorrect lookup in "mapToFoamCellId_" (typical cut/paste error) that is around line 461 of starMeshReader.C else if (shapeId == 255) { // poly cell - create cell faces directly label nFaces = starLabels[0] - 1; // record original cell number and lookup origCellId_[cellI] = starCellId; mapToFoamCellId_[starCellId] = cellI; The version that you have likely has the obviously wrong mapToFoamCellId_[starCellId] = starCellId; After OpenFOAM v1.4 is released, I'll be able to post a more recent version that also handles defined, but unused vertices and various other improvements. |
|
April 5, 2007, 05:48 |
Thank you very much Mark for t
|
#3 |
Member
|
Thank you very much Mark for the quick and effective reply. Following your suggestion, everything works now.
Thanks a lot again Cosimo
__________________
Cosimo Bianchini Ergon Research s.r.l. Via Panciatichi, 92 50127 Florence - ITALY Tel: +39 055 0763716 Mob: +39 320 9460153 e-mail: cosimo.bianchini@ergonresearch.it URL: www.ergonresearch.it |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Polyhedral Mesh | Diego Flores | FLUENT | 17 | August 21, 2020 14:52 |
CGNS import in fluent - periodic boundaries. | Bjarne Børresen | FLUENT | 2 | April 25, 2013 12:12 |
[Commercial meshers] Import error Gambit msh file with Cell Type 7 polyhedral cells | philippose | OpenFOAM Meshing & Mesh Conversion | 1 | June 1, 2007 03:58 |
polyhedral mesh | guang ai | Siemens | 3 | May 28, 2006 02:02 |
CGNS mesh import and boundaries | Barbaros | CFX | 0 | May 6, 2004 17:34 |