to Maintainers : ideasUnvToFoa
to Maintainers : ideasUnvToFoam utility has a serious bug - it couldn't correctly read complicated tet mesh, saved as unv-files, generated with Cubit (dont know about used mesh generator), SALOME (Netgen-4.5) and, perhaps, other CAD+meshing programs, and coudn't read grouped surfaces for BC patch from it. Topic was discussed here : http://www.cfd-online.com/OpenFOAM_D...tml?1186384437
Stefan Radl fixed problem of tet mesh reading, we fixed problem of correct reading generated patch for BC, now ideasUnvToFoam can read these big complicated mesh files. What is the way of posting source of new ideasUnvToFoam ? with a best regards ruben |
The best way is to post it hea
The best way is to post it hear using the attach command.
|
Take a look at the formatting
Take a look at the formatting section of the documentation of the forum software which you will see on the left hand side of your browser window. In there you will see a description of how to attach files.
|
Many Big Thanks, Henry - i was
Many Big Thanks, Henry - i was too harried, sorry 8-).
So, archieve with short test is placed here : http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif ideasUnvCSToFoam.tar.gz To try and use : 1. It should be unpacked to OF/OF-1.4/applications/utilities/mesh/conversion 2. cd OF/OF-1.4/applications/utilities/mesh/conversion/ideasUnvCSToFoam and wmake FoamX will find it, or it would be used from command line. |
I've checked it on as simple b
I've checked it on as simple box with groups inlet, outlet & walls, as tet mesh, created with SALOME-3.2.6 & their NETGEN-4.5 plugin, grouped faces for patching.
with a best regards Ruben |
I have tried ideasUnvCSToFoam
I have tried ideasUnvCSToFoam for a simple box with ~ 3000 hexaelements a two groups for inlet and outlet. The grid was generated with salome-3.2.6 .I got the following error
............... ................ reading face (faceI==)286; reading face (faceI==)288; reading face (faceI==)290; reading face (faceI==)292; reading face (faceI==)294; reading face (faceI==)296; reading face (faceI==)298; Sorting boundary faces according to group (patch) --> FOAM FATAL ERROR : 223 not found in table. Valid entries are 0() From function HashTable<t,>::operator[](const Key&) in file /home/miwesse/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/HashTableI.H at line 74. FOAM exiting What is the problem? Michael |
Hi Michael,
does the 1.4.1
Hi Michael,
does the 1.4.1 ideasUnvToFoam work? It contains some of the fixes from Ruben's version. If not, can you attach (50K limit) or mail me the file that gives problems? Mattijs |
Hi Mattijs,
the 1.4.1 ideas
Hi Mattijs,
the 1.4.1 ideasUnvToFoam also doesn't work. Therefore I attach .Thank you for your help. Michael |
Hi Mattijs,
the 1.4.1 ideas
Hi Mattijs,
the 1.4.1 ideasUnvToFoam also doesn't work. Therefore I will send you the file(< 50 k) by mail .Thank you for your help. Michael |
Added cell type 44. Works on y
Added cell type 44. Works on your file. Compile under 1.4.1
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif ideasUnvToFoam.C |
Thank you, Mattijs. Stefan & i
Thank you, Mattijs. Stefan & i didn't serve problem for hex geom. It would be great to combine advantages both convertors into one.
ruben |
Hi Ruben,
I put in your fix
Hi Ruben,
I put in your fix for patch face reading. Can you test this one? http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif ideasUnvToFoam.C |
Hi Mattijs,
I have tested i
Hi Mattijs,
I have tested ideasUnvToFoam and it works wll till now. Thanks Michael |
Thank You, Mattijs, my tet mes
Thank You, Mattijs, my tet mesh (46M) with BC converted correctly !
With Best Regards, ruben |
Hi Mattijs,
I have again a
Hi Mattijs,
I have again a problem with ideasUnvToFoam. I ahve now a grid with pentaeders and got the following error: ........ Processing tag:2411 Starting reading points at line 3. Read 28104 points. Processing tag:2412 Starting reading cells at line 56214. --> FOAM Warning : From function readCells(IFstream&, label&) in file ideasUnvToFoam.C at line 335 Reading "Pent_Mesh_1.unv" at line 75163 Cell type 112 not supported Read 0 cells and 19384 boundary faces. Can you again correct ideasUnvToFoam for this celltype 112 ? I will send you the example by e-mail. Thanks Michael |
Hi
I have tried ideasUnvCS
Hi
I have tried ideasUnvCSToFoam but got error for patchs v /*---------------------------------------------------------------------------*\ | ========= | | | \ / 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/gui/ test /home/gui/test/simple&wall.unv Date : Oct 18 2007 Time : 14:21:49 Host : gui-desktop PID : 19079 Root : /home/gui/ Case : test Nprocs : 1 Create time Processing tag:2411 Starting reading points at line 3. Read 892 points. Processing tag:2412 Starting reading cells at line 1790. Read 2746 cells and 1654 boundary faces. Processing tag:2467 Starting reading patches at line 10971. For facegroup 0 named stator trying to read 1027 patch face indices. --> 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 someone can help me ? thanks guillaume |
Does the standard 1.4.1 ideasU
Does the standard 1.4.1 ideasUnvToFoam work?
|
May be problem with your mesh.
May be problem with your mesh. Yesterday I got the same error, and it was concerned with non-correct building of complicated mesh with SALOME-NETGEN. I'd generated new mesh (with more number of nodes) - and solved problem.
|
It should be noted, that you n
It should be noted, that you need to use ideasUnvToFoam, posted at this topic 21.08.2007 - some problems of standard version (including 1.4.1) were patched there.
|
thanks
i have changed my mesh
thanks
i have changed my mesh,generated new (with less number of nodes) and it work. i think, like Rubben said ,it was concerned with non-correct building of complicated mesh with SALOME-NETGEN. best regards guillaume |
Hi,
I tryied to mesh prisms
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? |
For fix in ideasUnvToFoam (sup
For fix in ideasUnvToFoam (support to cell type 112, prisms) email to mkraposhin@inbox.ru (I don't know how to post file here)
|
2 RENAUD Guillaume
Do you use
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. |
Here's my latest. Should handl
Here's my latest. Should handle 112. Can you get back to me if it doesn't?
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif ideasUnvToFoam.C |
Hi,
Thank you Mattijs, this
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 |
Hi Mattijs,
I've taken you
Hi Mattijs,
I've taken your ideasUnvToFoam.C file, then i put it in $HOME/applications/utilities/mesh/conversion/ideasUnvToFoam on a shell I typed: wmake but I got some errors during the compilation, is there something I've missed? Thank you in advance Francesco |
No that is all that is necessa
No that is all that is necessary. Perhaps do a 'wclean' before 'wmake'?
- Can you compile anything at all? Try compiling one of the other 1.4.1 utilities. If that does works post the errors. |
Hi Mattijs,
I've tried to r
Hi Mattijs,
I've tried to recompile icoFoam: from the directory ~/OpenFOAM/OpenFOAM-1.4.1/applications/solvers/incompressible/icoFoam$ 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 |
Hi Mattijs,
It was a proble
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 |
I have build a tetraeder mesh
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 |
Report a bug with a testcase a
Report a bug with a testcase and I'll fix it.
|
Hi has anyone fixed this bug.
Hi has anyone fixed this bug. I need to use this software very soon and i dont have much time to fix the problem.
|
I have made a mistake. I have
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 |
I was able to export my mesh w
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.
|
Hi Stefan
Thanks for your c
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 |
Cell type 118 is parabolic tet
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
Thanks it works I j
Mattijs
Thanks it works I just uncheck midside nodes HP |
Hello Foamers/ Mattijs,
I u
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. http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif 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. http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif 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 |
Looks like something is wrong
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.
|
It seems you're right. One fac
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 |
All times are GMT -4. The time now is 09:57. |