CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Star4ToFoam import boundaries in polyhedral mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 5, 2007, 03:15
Default Hi all, I would like to conve
  #1
Member
 
cosimo bianchini
Join Date: Mar 2009
Location: Florence, Tuscany, Italy
Posts: 88
Rep Power: 8
cosimobianchini is on a distinguished road
Send a message via Skype™ to cosimobianchini
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

Energy Engineering Department "S. Stecco"
University of Florence
Via di S.Marta, 3
50139 Florence - ITALY
Tel: +39 055 4796575
Fax: +39 055 4796342
Mob: +39 320 9460153
e-mail: cosimo.bianchini@htc.de.unifi.it
URL: www.htc.de.unifi.it
cosimobianchini is offline   Reply With Quote

Old   April 5, 2007, 04:03
Default Hi Cosimo, Assuming that yo
  #2
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
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.
olesen is offline   Reply With Quote

Old   April 5, 2007, 04:48
Default Thank you very much Mark for t
  #3
Member
 
cosimo bianchini
Join Date: Mar 2009
Location: Florence, Tuscany, Italy
Posts: 88
Rep Power: 8
cosimobianchini is on a distinguished road
Send a message via Skype™ to cosimobianchini
Thank you very much Mark for the quick and effective reply. Following your suggestion, everything works now.

Thanks a lot again

Cosimo
__________________
Cosimo Bianchini

Energy Engineering Department "S. Stecco"
University of Florence
Via di S.Marta, 3
50139 Florence - ITALY
Tel: +39 055 4796575
Fax: +39 055 4796342
Mob: +39 320 9460153
e-mail: cosimo.bianchini@htc.de.unifi.it
URL: www.htc.de.unifi.it
cosimobianchini 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
CGNS import in fluent - periodic boundaries. Bjarne Børresen FLUENT 2 April 25, 2013 11:12
Polyhedral Mesh Diego Flores FLUENT 15 November 29, 2011 18:30
Import error Gambit msh file with Cell Type 7 polyhedral cells philippose OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 June 1, 2007 09:14
polyhedral mesh guang ai CD-adapco 3 May 28, 2006 01:02
CGNS mesh import and boundaries Barbaros CFX 0 May 6, 2004 16:34


All times are GMT -4. The time now is 03:46.