[victorbelenense]

Hi everyone,


I've been learning how to use openFoam for couple of months and recently I have started to study a simple airfoil case. I have done the mesh with Gmsh and followed the steps to produce the .msh file but when I finally try to import the .msh file to openFoam format with the command gmshToFoam I get the following message:

--> FOAM FATAL IO ERROR:
wrong token type - expected word, found on line 0 the label 99

file: IStringStream.sourceFile at line 0.

From function Foam::Istream& Foam:perator>>(Foam::Istream&, Foam::word&)
in file primitives/strings/word/wordIO.C at line 74.

FOAM exiting


Here is the .geo file:


//+
Point(1) = {0.08436612, 0.1027103, 0, 1.0};
//+
Point(2) = {0.08467859, 0.1005296, 0, 1.0};
//+
Point(3) = {0.08499106, 0.1053271, 0, 1.0};
//+
Point(4) = {0.08561599, 0.09834891, 0, 1.0};
//+
Point(5) = {0.08608469, 0.1075078, 0, 1.0};
//+
Point(6) = {0.08717833, 0.09660436, 0, 1.0};
//+
Point(7) = {0.08764703, 0.1092523, 0, 1.0};
//+
Point(8) = {0.08905313, 0.09529595, 0, 1.0};
//+
Point(9) = {0.0893656, 0.1107788, 0, 1.0};
//+
Point(10) = {0.09139663, 0.09420561, 0, 1.0};
//+
Point(11) = {0.09155287, 0.1118692, 0, 1.0};
//+
Point(12) = {0.0935839, 0.09333333, 0, 1.0};
//+
Point(13) = {0.09374014, 0.1129595, 0, 1.0};
//+
Point(14) = {0.09655234, 0.1140498, 0, 1.0};
//+
Point(15) = {0.09670857, 0.09246106, 0, 1.0};
//+
Point(16) = {0.09936454, 0.09202492, 0, 1.0};
//+
Point(17) = {0.09967701, 0.1149221, 0, 1.0};
//+
Point(18) = {0.1040516, 0.09158879, 0, 1.0};
//+
Point(19) = {0.104989, 0.1157944, 0, 1.0};
//+
Point(20) = {0.1081136, 0.09137072, 0, 1.0};
//+
Point(21) = {0.1098322, 0.1162305, 0, 1.0};
//+
Point(22) = {0.1131131, 0.09115265, 0, 1.0};
//+
Point(23) = {0.114363, 0.1164486, 0, 1.0};
//+
Point(24) = {0.1188937, 0.09115265, 0, 1.0};
//+
Point(25) = {0.1198311, 0.1162305, 0, 1.0};
//+
Point(26) = {0.1243619, 0.09115265, 0, 1.0};
//+
Point(27) = {0.1252993, 0.1155763, 0, 1.0};
//+
Point(28) = {0.1301426, 0.09115265, 0, 1.0};
//+
Point(29) = {0.13108, 0.114486, 0, 1.0};
//+
Point(30) = {0.1359232, 0.09115265, 0, 1.0};
//+
Point(31) = {0.1370168, 0.1133956, 0, 1.0};
//+
Point(32) = {0.1402977, 0.09093458, 0, 1.0};
//+
Point(33) = {0.1418601, 0.1123053, 0, 1.0};
//+
Point(34) = {0.1462346, 0.09093458, 0, 1.0};
//+
Point(35) = {0.1476407, 0.1105607, 0, 1.0};
//+
Point(36) = {0.1527964, 0.09049844, 0, 1.0};
//+
Point(37) = {0.1537338, 0.1085981, 0, 1.0};
//+
Point(38) = {0.1588895, 0.09006231, 0, 1.0};
//+
Point(39) = {0.1606081, 0.1059813, 0, 1.0};
//+
Point(40) = {0.1654513, 0.08919003, 0, 1.0};
//+
Point(41) = {0.1670137, 0.1033645, 0, 1.0};
//+
Point(42) = {0.1726381, 0.08809969, 0, 1.0};
//+
Point(43) = {0.173888, 0.1003115, 0, 1.0};
//+
Point(44) = {0.1813872, 0.08613707, 0, 1.0};
//+
Point(45) = {0.1823246, 0.09595016, 0, 1.0};
//+
Point(46) = {0.1891988, 0.08417445, 0, 1.0};
//+
Point(47) = {0.1902925, 0.09115265, 0, 1.0};
//+
Point(48) = {0.197323, 0.08133956, 0, 1.0};
//+
Point(49) = {0.1982604, 0.08657321, 0, 1.0};
//+
Point(50) = {0.204666, 0.0782866, 0, 1.0};
//+
Point(51) = {0.2054471, 0.08199377, 0, 1.0};
//+
Point(52) = {0.2127901, 0.07436137, 0, 1.0};
//+
Point(53) = {0.2132588, 0.07676012, 0, 1.0};
//+
Point(54) = {0.2198206, 0.07021807, 0, 1.0};
//+
Point(55) = {0.2204456, 0.07196262, 0, 1.0};
//+
Point(56) = {0.2259137, 0.06629283, 0, 1.0};
//+
Point(57) = {0.2263824, 0.06760125, 0, 1.0};
//+
Point(58) = {0.2296633, 0.06433022, 0, 1.0};
//+
Point(59) = {-1, -1, 0, 1.0};
//+
Point(60) = {-1, 1, 0, 1.0};
//+
Point(61) = {1, 1, 0, 1.0};
//+
Point(62) = {1, -1, 0, 1.0};
//+
Point(63) = {1, -1, 0, 1.0};
//+
Line(1) = {5, 3};
//+
Line(2) = {3, 1};
//+
Line(3) = {1, 2};
//+
Line(4) = {2, 2};
//+
Line(5) = {4, 2};
//+
Line(6) = {4, 6};
//+
Line(7) = {6, 8};
//+
Line(8) = {8, 10};
//+
Line(9) = {10, 12};
//+
Line(10) = {12, 15};
//+
Line(11) = {15, 16};
//+
Line(12) = {16, 18};
//+
Line(13) = {18, 20};
//+
Line(14) = {20, 22};
//+
Line(15) = {22, 24};
//+
Line(16) = {24, 26};
//+
Line(17) = {26, 28};
//+
Line(18) = {28, 30};
//+
Line(19) = {30, 32};
//+
Line(20) = {32, 34};
//+
Line(21) = {34, 36};
//+
Line(22) = {36, 38};
//+
Line(23) = {38, 40};
//+
Line(24) = {40, 42};
//+
Line(25) = {42, 44};
//+
Line(26) = {44, 46};
//+
Line(27) = {46, 48};
//+
Line(28) = {48, 50};
//+
Line(29) = {50, 52};
//+
Line(30) = {52, 54};
//+
Line(31) = {54, 56};
//+
Line(32) = {56, 58};
//+
Line(33) = {58, 57};
//+
Line(34) = {57, 55};
//+
Line(35) = {55, 53};
//+
Line(36) = {53, 51};
//+
Line(37) = {51, 49};
//+
Line(38) = {49, 47};
//+
Line(39) = {47, 45};
//+
Line(40) = {45, 43};
//+
Line(41) = {43, 41};
//+
Line(42) = {41, 39};
//+
Line(43) = {39, 37};
//+
Line(44) = {37, 35};
//+
Line(45) = {35, 33};
//+
Line(46) = {33, 31};
//+
Line(47) = {31, 29};
//+
Line(48) = {29, 27};
//+
Line(49) = {27, 25};
//+
Line(50) = {25, 23};
//+
Line(51) = {23, 21};
//+
Line(52) = {21, 19};
//+
Line(53) = {19, 17};
//+
Line(54) = {17, 14};
//+
Line(55) = {14, 13};
//+
Line(56) = {13, 11};
//+
Line(57) = {11, 9};
//+
Line(58) = {9, 7};
//+
Line(59) = {7, 5};
//+
Line(60) = {60, 59};
//+
Line(61) = {59, 62};
//+
Line(62) = {62, 61};
//+
Line(63) = {61, 60};
//+
Line Loop(1) = {63, 60, 61, 62};
//+
Line Loop(2) = {53, 54, 55, 56, 57, 58, 59, 1, 2, 3, -5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15, 16, 17, 18, 19, 20, 21, 22, 23, 24, 25, 26, 27, 28, 29, 30, 31, 32, 33, 34, 35, 36, 37, 38, 39, 40, 41, 42, 43, 44, 45, 46, 47, 48, 49, 50, 51, 52};
//+
Plane Surface(1) = {1, 2};
//+
Physical Volume("internal") = {1};
Extrude {0,0,0.05}
{
Surface{1};
Layers{1};
Recombine;
}
//+
Physical Surface("walls") = {150, 146, 374, 370, 366, 362, 1, 358, 354, 350, 346, 342, 338, 334, 330, 326, 322, 318, 314, 310, 306, 302, 298, 294, 290, 286, 282, 278, 274, 270, 266, 262, 258, 254, 250, 246, 242, 238, 234, 230, 226, 222, 375, 218, 214, 210, 206, 202, 198, 194, 190, 186, 182, 178, 174, 170, 166, 162, 158, 154};

//+
Physical Surface("inlet") = {130,134,138};
//+
Physical Surface("frontAndBack") = {375, 1};
//+
Physical Surface("outlet") = {142};
//+
Characteristic Length {60, 59, 62, 61} = 0.1;
//+
Characteristic Length {17, 14, 13, 11, 9, 7, 5, 3, 1, 2, 4, 6, 8, 10, 12, 15} = 0.01;





I already read several tutorials and I am still stuck at the same issue.
I humbly ask for some help.

[mzzmrt]

I have tested your "x.geo" script with gmsh 3.0.6, made a 3D "x.msh" with it and imported to OpenFOAM (4.1) as "gmshToFoam x.geo"


Well, it is working as expected.



If you are on windows this may be a reason....

[victorbelenense]

Hi mzzmrt,

Thank you for the reply. I am using Ubuntu 16.04, Gmsh 4.0.0 and OpenFoam 5.
I got a new error message now when using gmshToFoam:

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

file: IStringStream.sourceFile at line 0.

From function bool Foam::Istream::getBack(Foam::token&)


I have no idea why it is not working for me. Could you show me the .msh file?

[mzzmrt]

I got it. The default *.msh format of the latest gmsh (4.0) has been updated to v4 but gmshToFoam needs v2.


So while exporting the mesh from gmsh use >file>export>*.msh and choose v2 ascii. Then it will work.


Second line in the *.msh also shows the version...

[victorbelenense]

It worked! It was the v2 ascii format as you said.

Thank you mzzmrt!

[jaggonz]

THANK YOU!! I wasted a tremendous amount of time trying to figure out the problem. Selecting v2 ASCII solved it!!!

[Talder]

I'm running OpenFoam v1812+ on Fedora 28, with gmsh 4.0.7 (all recent versions)
My gmsh file>export> doesn't allow me to indicate V2 ASCII or something like that.

However, looking at the header of the saved testmesh (4 connected cubes), that seems OK, it's version 2.2 ASCII, but gmshToFoam still gives me a 'bad token' error.



Any suggestion what else I can try, apart from editing the .msh file ?



(this used to work properly with GMSH 2 and OpenFoam 2.x versions)


$MeshFormat
2.2 0 8
$EndMeshFormat
$PhysicalNames
10
2 1 "inlet"
2 2 "outlet"
2 3 "leftwall"
2 4 "rightwall"
2 5 "top"
2 6 "bottom"
3 7 "V1"
3 8 "V2"
3 9 "V3"
3 10 "V4"
$EndPhysicalNames
$Nodes
7381
1 -0 -0 0
2 1 -0 0
3 0 0.5 0






[tom@localhost meshtest]$ gmshToFoam test2.msh
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v1812 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : v1812 OPENFOAM=1812
Arch : "LSB;label=32;scalar=64"
Exec : gmshToFoam test2.msh
Date : Feb 08 2019
Time : 17:54:19
Host : localhost.localdomain
PID : 9194
I/O : uncollated
Case : /home/tom/OpenFOAM/tom-v1812/run/meshtest
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Starting to read mesh format at line 2
Read format version 2.2 ascii 0

Starting to read physical names at line 5
Physical names:10
Surface 1 inlet
Surface 2 outlet
Surface 3 leftwall
Surface 4 rightwall
Surface 5 top
Surface 6 bottom
Volume 7 V1
Volume 8 V2
Volume 9 V3
Volume 10 V4

Starting to read points at line 18
Vertices to be read:7381
Vertices read:7381

Starting to read cells at line 7402
Cells to be read:8600

Mapping region 3 to Foam patch 0
Mapping region 6 to Foam patch 1
Mapping region 5 to Foam patch 2
Mapping region 1 to Foam patch 3
Mapping region 4 to Foam patch 4
Mapping region 2 to Foam patch 5
Mapping region 7 to Foam cellZone 0
Mapping region 8 to Foam cellZone 1
Mapping region 9 to Foam cellZone 2
Mapping region 10 to Foam cellZone 3
Cells:
total:6000
hex :6000
prism:0
pyr :0
tet :0

CellZones:
Zone Size
0 2000
1 1000
2 1000
3 2000



--> FOAM FATAL IO ERROR:
Bad token - could not get word

file: input at line 0.

From function Foam::Istream& Foam:perator>>(Foam::Istream&, Foam::word&)
in file primitives/strings/word/wordIO.C at line 45.

FOAM exiting

[Talder]

I made a really simple gmsh testcube.geo in 3D. (4 x 4 x 4 ) 64-cell volume.

The file>export> *.msh V2 ASCII is OK.
Since the foam error wants a word, I just added "$end" at the end of the msh file.
Now gmshToFoam makes a polymesh. I do see the cube in paraFoam, but the internal mesh is missing.



So it is clear that gmshToFoam expects some more definition about 3D-internal mesh, not sure what else you can save after generating the 3D mesh in gmsh.


Hope someone sees what's missing
Tom.



Below is a view of the testcube.geo and testcube in paraFoam result. (and geo file)


testcube.geo:


//+
dim=1.0;

hz=1.0;
gridx=5;
gridy=5;
gridz=5;

Point(1) = {0.0, 0.0, 0.0, dim};
Point(2) = {0.0, 1.0, 0.0, dim};
Point(3) = {1.0, 1.0, 0.0, dim};
Point(4) = {1.0, 0.0, 0.0, dim};
Point(5) = {0.0, 0.0, hz, dim};
Point(6) = {0.0, 1.0, hz, dim};
Point(7) = {1.0, 1.0, hz, dim};
Point(8) = {1.0, 0.0, hz, dim};

Line(1) = {1,2};
Line(2) = {2,3};
Line(3) = {3,4};
Line(4) = {4,1};
Line(5) = {5,6};
Line(6) = {6,7};
Line(7) = {7,8};
Line(8) = {8,5};
Line(9) = {1,5};
Line(10) = {2,6};
Line(11) = {3,7};
Line(12) = {4,8};

// inlet box 1 surface loops
Line Loop(201) = {1,2,3,4};
Line Loop(202) = {5,6,7,8};
Line Loop(203) = {1,10,-5,-9};
Line Loop(204) = {2,11,-6,-10};
Line Loop(205) = {3,12,-7,-11};
Line Loop(206) = {4,9,-8,-12};

// define surface inlet box 1
Plane Surface(201) = {201};
Plane Surface(202) = {202};
Plane Surface(203) = {203};
Plane Surface(204) = {204};
Plane Surface(205) = {205};
Plane Surface(206) = {206};

//Make surfaces structured. Box 1
Transfinite Line{2,-4,6,-8} = gridx;
Transfinite Line{1,-3,5,-7} = gridy;
Transfinite Line{9,10,11,12} = gridz;

// define surface loops box1
Surface Loop(301) = {201,202,203,204,205,206};

Volume(301) = {301};

Transfinite Surface "*";
Recombine Surface "*";
Transfinite Volume "*";

//+
Physical Surface("inlet") = {203};
Physical Surface("outlet") = {205};
Physical Surface("walls") = {204, 206};
Physical Surface("top") = {202};
Physical Surface("bottom") = {201};

//+
Physical Volume("internalvolume") = {301};

//+

[Talder]

Problem resolved, if useful for others.
The cube problem above is OK, paraFoam doesn't show internal wireframe cells.


The weird point is that gmshToFoam expects another word at the end of the .msh file.
If I add 1 line with "$end" to any old or new msh file from gmsh, it converts properly.



Tom.

[segelpaul]

$End


works for me as well... Thank!!!