CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Bugs

IdeasUnvToFoam Bug amp Fix

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 24, 2007, 07:33
Default Hi, I tryied to mesh prisms
  #21
New Member
 
maitre touf
Join Date: Mar 2009
Posts: 6
Rep Power: 8
touf is on a distinguished road
Hi,
I tryied to mesh prisms in salome, in order to do a pseudo-2D simulaiton around an airfoil. When trying to convert to OF, with the last version of ideasUnvTofoam, i recieve the mesage:

Cell type 112 not supported
Read 0 cells and 4130 boundary faces.

and convertion stopped.
Any help please?
touf is offline   Reply With Quote

Old   November 26, 2007, 05:52
Default For fix in ideasUnvToFoam (sup
  #22
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8
mkraposhin is on a distinguished road
For fix in ideasUnvToFoam (support to cell type 112, prisms) email to mkraposhin@inbox.ru (I don't know how to post file here)
mkraposhin is offline   Reply With Quote

Old   November 26, 2007, 09:41
Default 2 RENAUD Guillaume Do you use
  #23
Member
 
Ruben I. Mukhamadeev
Join Date: Mar 2009
Location: Obninsk, Kaluga reg., Russian Federation
Posts: 69
Rep Power: 8
benru is on a distinguished road
2 RENAUD Guillaume
Do you use standard (which present in distr OF-1.4.1) ideasUnvToFoam or one from this forum (21.08.2007 by Mattijs Janssens) ? It seems to me, that this version works coorrectly.
benru is offline   Reply With Quote

Old   November 27, 2007, 14:51
Default Here's my latest. Should handl
  #24
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Here's my latest. Should handle 112. Can you get back to me if it doesn't?
ideasUnvToFoam.C
mattijs is offline   Reply With Quote

Old   November 27, 2007, 15:56
Default Hi, Thank you Mattijs, this
  #25
New Member
 
maitre touf
Join Date: Mar 2009
Posts: 6
Rep Power: 8
touf is on a distinguished road
Hi,

Thank you Mattijs, this new version works fine
previously I used the one of 21.08.2007, and it was not handling cells 112
touf is offline   Reply With Quote

Old   January 15, 2008, 04:58
Default Hi Mattijs, I've taken you
  #26
Member
 
Francesco Boschetto
Join Date: Mar 2009
Location: Italy
Posts: 56
Rep Power: 8
francesco_b is on a distinguished road
Hi Mattijs,

I've taken your ideasUnvToFoam.C file, then i put it in $HOME/applications/utilities/mesh/conversion/ideasUnvToFoam
on a shell I typed:

wmake

but I got some errors during the compilation, is there something I've missed?

Thank you in advance

Francesco
francesco_b is offline   Reply With Quote

Old   January 15, 2008, 14:14
Default No that is all that is necessa
  #27
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
No that is all that is necessary. Perhaps do a 'wclean' before 'wmake'?

- Can you compile anything at all? Try compiling one of the other 1.4.1 utilities. If that does works post the errors.
mattijs is offline   Reply With Quote

Old   January 23, 2008, 10:22
Default Hi Mattijs, I've tried to r
  #28
Member
 
Francesco Boschetto
Join Date: Mar 2009
Location: Italy
Posts: 56
Rep Power: 8
francesco_b is on a distinguished road
Hi Mattijs,

I've tried to recompile icoFoam: from the directory ~/OpenFOAM/OpenFOAM-1.4.1/applications/solvers/incompressible/icoFoam$

I typed:

wclean

wmake

and I've got lots of errors, so I think there something wrong with my installation.

Errors are too much, so I report some of them, they are like this:

/home/area3/OpenFOAM/linux/gcc-4.2.1/bin/../lib/gcc/i686-pc-linux-gnu/4.2.1/../. ./../../include/c++/4.2.1/cstdlib:106: error: '::div_t' has not been declared
/home/area3/OpenFOAM/linux/gcc-4.2.1/bin/../lib/gcc/i686-pc-linux-gnu/4.2.1/../. ./../../include/c++/4.2.1/cstdlib:107: error: '::ldiv_t' has not been declared
/home/area3/OpenFOAM/linux/gcc-4.2.1/bin/../lib/gcc/i686-pc-linux-gnu/4.2.1/../. ./../../include/c++/4.2.1/cstdlib:109: error: '::abort' has not been declared
/home/area3/OpenFOAM/linux/gcc-4.2.1/bin/../lib/gcc/i686-pc-linux-gnu/4.2.1/../. ./../../include/c++/4.2.1/cstdlib:110: error: '::abs' has not been declared
/home/area3/OpenFOAM/linux/gcc-4.2.1/bin/../lib/gcc/i686-pc-linux-gnu/4.2.1/../. ./../../include/c++/4.2.1/cstdlib:111: error: '::atexit' has not been declared

I think there could be something stupid I've missed, I'm trying to understand what

Thanks in advance

Francesco
francesco_b is offline   Reply With Quote

Old   January 23, 2008, 10:42
Default Hi Mattijs, It was a proble
  #29
Member
 
Francesco Boschetto
Join Date: Mar 2009
Location: Italy
Posts: 56
Rep Power: 8
francesco_b is on a distinguished road
Hi Mattijs,

It was a problem of Gcc 4.2.1, I didn't install all the packages, but only the base, I'm sorry for my stupid mistakes,

Regards

Francesco
francesco_b is offline   Reply With Quote

Old   February 25, 2008, 12:01
Default I have build a tetraeder mesh
  #30
New Member
 
Michael Wessels
Join Date: Mar 2009
Posts: 8
Rep Power: 8
miwesse is on a distinguished road
I have build a tetraeder mesh with salome3.2.6 and exported the mesh as *.unv file.
When I used ideasUnvToFoam to convert the mesh I got the following error:
Exec : ideasUnvToFoam . Mesh_moderate Mesh3D_Moderate.unv
Date : Feb 25 2008
Time : 16:57:13
Host : linux-b5l3
PID : 13858
Root : /home/lxuser/OpenFOAM/lxuser-1.4.1/run/AFC_Actuator/Geometry
Case : Mesh_moderate
Nprocs : 1
Create time

Processing tag:2411
Starting reading points at line 3.
Read 146916 points.

Processing tag:2412
Starting reading cells at line 293838.
First occurrence of element type 22 for cell 1 at line 293839
--> FOAM Warning :
From function readCells(IFstream&, label&)
in file ideasUnvToFoam.C at line 387
Reading "Mesh3D_Moderate.unv" at line 293839
Cell type 22 not supported


--> FOAM FATAL IO ERROR : Attempt to get back from bad stream

file: IStringStream.sourceFile at line 0.

From function void Istream::getBack(token& t)
in file db/IOstreams/IOstreams/Istream.C at line 44.

FOAM exiting

How can I solve the problem ?

Michael
miwesse is offline   Reply With Quote

Old   February 25, 2008, 13:56
Default Report a bug with a testcase a
  #31
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Report a bug with a testcase and I'll fix it.
mattijs is offline   Reply With Quote

Old   February 26, 2008, 08:28
Default Hi has anyone fixed this bug.
  #32
New Member
 
OpenFOAM Newbie
Join Date: Mar 2009
Posts: 20
Rep Power: 8
lofty is on a distinguished road
Hi has anyone fixed this bug. I need to use this software very soon and i dont have much time to fix the problem.
lofty is offline   Reply With Quote

Old   February 26, 2008, 15:30
Default I have made a mistake. I have
  #33
New Member
 
Michael Wessels
Join Date: Mar 2009
Posts: 8
Rep Power: 8
miwesse is on a distinguished road
I have made a mistake. I have build in salome3.2.6 the mesh with second order elements. These are of course not supported by the ideasUnvToFoam converter. I have no problems with linear elements.
Sorry!

Michael
miwesse is offline   Reply With Quote

Old   February 27, 2008, 07:18
Default I was able to export my mesh w
  #34
New Member
 
OpenFOAM Newbie
Join Date: Mar 2009
Posts: 20
Rep Power: 8
lofty is on a distinguished road
I was able to export my mesh with no problems as well. However, i was really worried that i am gone get same error message as you.
lofty is offline   Reply With Quote

Old   April 21, 2008, 15:42
Default Hi Stefan Thanks for your c
  #35
New Member
 
Humberto Peredo
Join Date: Mar 2009
Location: Queretaro, Queretaro, MExico
Posts: 2
Rep Power: 0
hperedo is on a distinguished road
Hi Stefan

Thanks for your comments

However the log that I sent you was for a test in order to see whats going on

I am appending the log for the unv that I am trying to import to OF

I will review in detail your comments in the manual

Let me know any comments

humberto@linux:~/OpenFOAM/humberto-1.4.1/run/tutorials/interFoam/assy> ideasUnvToFoam /home/humberto/OpenFOAM/humberto-1.4.1/run/tutorials/interFoam assy assy.unv
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4.1 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : ideasUnvToFoam /home/humberto/OpenFOAM/humberto-1.4.1/run/tutorials/interFoam assy assy.unv
Date : Apr 19 2008
Time : 16:01:47
Host : linux
PID : 8090
Root : /home/humberto/OpenFOAM/humberto-1.4.1/run/tutorials/interFoam
Case : assy
Nprocs : 1
Create time

Processing tag:151
"C:FEMAP93ExamplesAssemblydone.MOD
"C:FEMAP93ExamplesAssemblydone.MOD
"Femap with NX Nastran
" 14-Apr-08 21:45:54 9 30 0
" Never Never
"Femap with NX Nastran
" 14-Apr-08 21:45:54 9 30 10 0 0

Processing tag:180
Skipping tag 180 on line 13
Skipping section at line 13.

Processing tag:164
Starting reading units at line 116.
l:7
units:"Inch (pound f) "
unitType:2
Unit factors:
Length scale : 39.3701
Force scale : 0.224809
Temperature scale : 1.8
Temperature offset : 459.67


Processing tag:1710
Skipping tag 1710 on line 122
Skipping section at line 122.

Processing tag:2420
Skipping tag 2420 on line 376
Skipping section at line 376.

Processing tag:2411
Starting reading points at line 411.
--> FOAM Warning :
From function readPoints(IFstream&, label&, DynamicList<point>, DynamicList<label>&)
in file ideasUnvToFoam.C at line 215
Points not in order starting at point 2 at line 412
Read 16786 points.

Processing tag:2431
Skipping tag 2431 on line 33986
Skipping section at line 33986.

Processing tag:2437
Skipping tag 2437 on line 33989
Skipping section at line 33989.

Processing tag:776
Skipping tag 776 on line 33994
Skipping section at line 33994.

Processing tag:2412
Starting reading cells at line 33997.
--> FOAM Warning :
From function readCells(IFstream&, label&)
in file ideasUnvToFoam.C at line 335
Reading "assy.unv" at line 33998
Cell type 118 not supported


--> FOAM FATAL IO ERROR : Attempt to get back from bad stream

file: IStringStream.sourceFile at line 0.

From function void Istream::getBack(token& t)
in file db/IOstreams/IOstreams/Istream.C at line 44.

FOAM exiting
hperedo is offline   Reply With Quote

Old   April 22, 2008, 03:58
Default Cell type 118 is parabolic tet
  #36
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Cell type 118 is parabolic tet. See remark above about 2nd order elements not supported. Also your points are not output in consecutive order but this should not cause problems.



11 Rod
21 Linear beam
22 Tapered beam
23 Curved beam
24 Parabolic beam
31 Straight pipe
32 Curved pipe
41 Plane Stress Linear Triangle
42 Plane Stress Parabolic Triangle
43 Plane Stress Cubic Triangle
44 Plane Stress Linear Quadrilateral
45 Plane Stress Parabolic Quadrilateral
46 Plane Strain Cubic Quadrilateral
51 Plane Strain Linear Triangle
52 Plane Strain Parabolic Triangle
53 Plane Strain Cubic Triangle
54 Plane Strain Linear Quadrilateral
55 Plane Strain Parabolic Quadrilateral
56 Plane Strain Cubic Quadrilateral
61 Plate Linear Triangle
62 Plate Parabolic Triangle
63 Plate Cubic Triangle
64 Plate Linear Quadrilateral
65 Plate Parabolic Quadrilateral
66 Plate Cubic Quadrilateral
71 Membrane Linear Quadrilateral
72 Membrane Parabolic Triangle
73 Membrane Cubic Triangle
74 Membrane Linear Triangle
75 Membrane Parabolic Quadrilateral
76 Membrane Cubic Quadrilateral
81 Axisymetric Solid Linear Triangle
82 Axisymetric Solid Parabolic Triangle
84 Axisymetric Solid Linear Quadrilateral
85 Axisymetric Solid Parabolic Quadrilateral
91 Thin Shell Linear Triangle
92 Thin Shell Parabolic Triangle
93 Thin Shell Cubic Triangle
94 Thin Shell Linear Quadrilateral
95 Thin Shell Parabolic Quadrilateral
96 Thin Shell Cubic Quadrilateral
101 Thick Shell Linear Wedge
102 Thick Shell Parabolic Wedge
103 Thick Shell Cubic Wedge
104 Thick Shell Linear Brick
105 Thick Shell Parabolic Brick
106 Thick Shell Cubic Brick
111 Solid Linear Tetrahedron
112 Solid Linear Wedge
113 Solid Parabolic Wedge
114 Solid Cubic Wedge
115 Solid Linear Brick
116 Solid Parabolic Brick
117 Solid Cubic Brick
118 Solid Parabolic Tetrahedron
121 Rigid Bar
122 Rigid Element
136 Node To Node Translational Spring
137 Node To Node Rotational Spring
138 Node To Ground Translational Spring
139 Node To Ground Rotational Spring
141 Node To Node Damper
142 Node To Gound Damper
151 Node To Node Gap
152 Node To Ground Gap
161 Lumped Mass
171 Axisymetric Linear Shell
172 Axisymetric Parabolic Shell
181 Constraint
191 Plastic Cold Runner
192 Plastic Hot Runner
193 Plastic Water Line
194 Plastic Fountain
195 Plastic Baffle
196 Plastic Rod Heater
201 Linear node-to-node interface
202 Linear edge-to-edge interface
203 Parabolic edge-to-edge interface
204 Linear face-to-face interface
208 Parabolic face-to-face interface
212 Linear axisymmetric interface
213 Parabolic axisymmetric interface
221 Linear rigid surface
222 Parabolic rigin surface
231 Axisymetric linear rigid surface
232 Axisymentric parabolic rigid surface
mattijs is offline   Reply With Quote

Old   May 1, 2008, 19:03
Default Mattijs Thanks it works I j
  #37
New Member
 
Humberto Peredo
Join Date: Mar 2009
Location: Queretaro, Queretaro, MExico
Posts: 2
Rep Power: 0
hperedo is on a distinguished road
Mattijs

Thanks it works I just uncheck midside nodes

HP
hperedo is offline   Reply With Quote

Old   May 8, 2008, 16:00
Default Hello Foamers/ Mattijs, I u
  #38
Senior Member
 
Mark Couwenberg
Join Date: Mar 2009
Location: Netherlands
Posts: 130
Rep Power: 8
markc is on a distinguished road
Hello Foamers/ Mattijs,

I used ideasUnvToFoam with the prism possiblity (type 112). The utility seems to work without errors. However, checkMesh returns errors with respect to faces with incorrect edgeFaces and nonManifoldPoints. The mesh domain is a one-layer axisymmetric domain. Problems seems to occur neer the axis, where some prisms exist. The incorrect edges seem to be diagonal edges running over 4-nodes surfaces.
Snapshot.pdf
The attachment shows a snapshot from paraview, showing wireframe of the model and two of the erroneous patches. Diagonal edges are visible.Inspecting the unv mesh in either Femap (where I modelled and made the mesh) and in Salome does not show any of those features.
checkmeshlog
Attached the checkmesh log.
I tried to remove the erronuous faces using faceset and removeface but without succes.
I suspect this is a bug in the Unv converter. However there is of course also a possiblity that there is something wrong with my mesh. I am eager to send you my mesh.

Awaiting any comments,

Mark
markc is offline   Reply With Quote

Old   May 8, 2008, 18:47
Default Looks like something is wrong
  #39
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Looks like something is wrong with your mesh. The converter expects a properly connected mesh. You might have two triangles (from one cell) on top of a quad (from a neighbouring cell) which is not handled. Load the duplicate faces into paraview and switch on point display.
mattijs is offline   Reply With Quote

Old   May 9, 2008, 08:30
Default It seems you're right. One fac
  #40
Senior Member
 
Mark Couwenberg
Join Date: Mar 2009
Location: Netherlands
Posts: 130
Rep Power: 8
markc is on a distinguished road
It seems you're right. One face of a hex is shared by two faces of two neighbouring tets, causing the diagonal. Thanks for your hint.
Mark
markc 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
Ideasunvtofoam and FoamX micpage18 OpenFOAM Mesh Utilities 0 June 20, 2007 10:17


All times are GMT -4. The time now is 12:00.