CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Meshing & Mesh Conversion (https://www.cfd-online.com/Forums/openfoam-meshing/)
-   -   [Gmsh] "Perhaps you have not exported the 3D elements?" (https://www.cfd-online.com/Forums/openfoam-meshing/185021-perhaps-you-have-not-exported-3d-elements.html)

j_moulton March 17, 2017 00:16

"Perhaps you have not exported the 3D elements?"
 
Hi,

I'm trying to mesh a *.msh file in OF and I receive the following error:

Code:

--> FOAM FATAL IO ERROR:
No cells read from file "pipe2.msh"
Does your file specify any 3D elements (hex=5, prism=6, pyramid=7, tet=4)?
Perhaps you have not exported the 3D elements?

Been digging around on this site trying to figure out a solution, but everything I see is never explained or is a dead end. Please help. My .geo file is:

Code:

Point(1) = {0, 0, 0, 1.0};
//+
Point(2) = {1, 0, 0, 1.0};
//+
Point(3) = {0, 1, 0, 1.0};
//+
Point(4) = {-1, 0, 0, 1.0};
//+
Point(5) = {0, -1, 0, 1.0};
//+
Circle(1) = {2, 1, 3};
//+
Circle(2) = {3, 1, 4};
//+
Circle(3) = {4, 1, 5};
//+
Circle(4) = {5, 1, 2};
//+
Line Loop(5) = {1, 2, 3, 4};
//+
Plane Surface(6) = {5};
//+
Extrude {0, 0, 10} {
  Surface{6};
  Layers{10};
}
//+
Surface Loop(29) = {6, 15, 19, 23, 27, 28};
//+
Volume(30) = {29};
//+
Physical Surface("inlet") = {6};
//+
Physical Surface("outlet") = {28};
//+
Physical Surface("wall") = {27, 15, 19, 23};
//+
Physical Volume("fluid") = {30};


CFD-Lover March 20, 2017 11:00

Hi Jeremy,

I have looked through your code and was able to recreate it for you. Here is the code;

Code:

Point(1) = {0, 0, 0, 0};
Point(2) = {10, 0, 0, 0};
Point(3) = {0, 1, 0, 0};
Point(4) = {10, 1, 0, 0};
Line(1) = {4, 2};
Line(2) = {2, 1};
Line(3) = {1, 3};
Line(4) = {3, 4};

Line Loop(5) = {4, 1, 2, 3};
Plane Surface(6) = {5};
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{6};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{23};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{40};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{57};
}
Surface Loop(74) = {18, 15, 22, 6, 23};
Volume(75) = {74};
Surface Loop(76) = {69, 66, 73, 6, 57};
Volume(77) = {76};
Surface Loop(78) = {52, 49, 56, 40, 57};
Volume(79) = {78};
Surface Loop(80) = {23, 32, 35, 39, 40};
Volume(81) = {80};
d1 = 1;
d2 = 1;
d3 = 1.;//1.171;
N1 = 50;
N2 = 50;
N3 = 18;
Transfinite Line {4, 42, 25, 8, 2} = N1 Using Progression d1;
Transfinite Line {3, 45, 28, 11, 1, 43, 26, 9} = N2 Using Progression d2;
Transfinite Line {64, 47, 30, 13, 14, 65, 48, 31} = N3 Using Progression d3;
Transfinite Surface "*";
Transfinite Volume "*";
Recombine Surface "*";
Coherence;
Physical Surface("inlet") = {73, 22, 39, 56};
Physical Surface("outlet") = {69, 18, 35, 52};
Physical Surface("walls") = {15, 66, 49, 32};
Physical Volume("internal") = {3, 2, 1, 4};

Let me know how it goes with you.

Cheers,

j_moulton March 20, 2017 14:28

Quote:

Originally Posted by CFD-Lover (Post 641477)
Hi Jeremy,

I have looked through your code and was able to recreate it for you. Here is the code;
Let me know how it goes with you.

Cheers,

Hi, thank you! This looks fantastic. Could you provide some insight into what I was not doing properly, or why you made the geometry and the subsequent mesh the way that you did?

tareqkh March 20, 2017 14:34

Hi Jeremy,

In your case, you were not using volume surface. You defined a plane surface only but since you have a volume i.e. 3D you need to define volume surface to be able to use structured me of the 3D.

Best,

j_moulton March 20, 2017 14:39

Quote:

Originally Posted by tareqkh (Post 641506)
Hi Jeremy,

In your case, you were not using volume surface. You defined a plane surface only but since you have a volume i.e. 3D you need to define volume surface to be able to use structured me of the 3D.

Best,

Thank you. I thought in fact I had defined all of the volumes properly. I appreciate the insight!

tareqkh March 20, 2017 14:45

You are welcomed. Let me know if you need more help.

Best,

j_moulton March 24, 2017 00:48

Quote:

Originally Posted by tareqkh (Post 641508)
You are welcomed. Let me know if you need more help.

Best,

I do need some more help. I followed CFD-Lovers's file and extended it for the case that I actually need to model -- a pipe with a bulb/sac on the end to model an alveolar sac. I am getting the following errors from Gmsh:

Code:

Info    : Finalized high order topology of periodic connections
Info    : Meshing 3D...
Info    : Meshing volume 1 (transfinite)
Error  : Incompatible surface 26 in transfinite volume 1
Info    : Meshing volume 2 (transfinite)
Error  : Incompatible surface 43 in transfinite volume 2
Info    : Meshing volume 3 (transfinite)
Error  : Incompatible surface 60 in transfinite volume 3
Info    : Meshing volume 4 (transfinite)
Error  : Incompatible surface 77 in transfinite volume 4
Info    : Meshing volume 5 (transfinite)
Error  : Transfinite algorithm only available for 5- and 6-face volumes
Info    : Meshing volume 6 (transfinite)
Error  : Transfinite algorithm only available for 5- and 6-face volumes
Info    : Meshing volume 7 (transfinite)
Error  : Transfinite algorithm only available for 5- and 6-face volumes
Info    : Meshing volume 8 (transfinite)
Error  : Transfinite algorithm only available for 5- and 6-face volumes
Info    : Meshing volume 122 (transfinite)
Error  : Incompatible surface 26 in transfinite volume 122
Info    : Meshing volume 124 (transfinite)
Error  : Incompatible surface 77 in transfinite volume 124
Info    : Meshing volume 126 (transfinite)
Error  : Incompatible surface 60 in transfinite volume 126
Info    : Meshing volume 128 (transfinite)
Error  : Incompatible surface 43 in transfinite volume 128
Info    : Meshing volume 130 (transfinite)
Error  : Transfinite algorithm only available for 5- and 6-face volumes
Info    : Meshing volume 132 (transfinite)
Error  : Transfinite algorithm only available for 5- and 6-face volumes
Info    : Meshing volume 134 (transfinite)
Error  : Transfinite algorithm only available for 5- and 6-face volumes
Info    : Meshing volume 136 (transfinite)
Error  : Transfinite algorithm only available for 5- and 6-face volumes

and then
Code:

Error  : Cannot build pyramids on non manifold faces
about 1500 times. I've read that (some of) these errors are produced because transfinite surface/volume requires the lines, surfaces, & volumes to be listed in a certain order. I thought I was following that order. Can you help clarify? Here is my .geo file:

Code:

// Gmsh project created on Thu Mar 23 16:06:33 2017
Point(1) = {0, 0, 0, 0};
Point(2) = {10, 0, 0, 0};
Point(3) = {0, 1, 0, 0};
Point(4) = {10, 1, 0, 0};
Point(5) = {14, 0, 0, 0};
Point(6) = {11.9, 0.1, 0, 1.0};
Line(1) = {4,2};
Line(2) = {2,1};
Line(3) = {1,3};
Line(4) = {3,4};
Line(5) = {2,5};
Circle(6) = {5, 6, 4};
Line Loop(7) = {4, 1, 2, 3};
Plane Surface(8) = {7};
Line Loop(9) = {6, 5, 1};
//+
Plane Surface(10) = {9};
//+
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{8};
}
//+
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{27};
}
//+
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{44};
}
//+
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{61};
}
//+
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{10};
}
//+
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{89};
}
//+
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{101};
}
//+
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{113};
}
Surface Loop(121) = {22, 19, 26, 8, 27};
Volume(122) = {121};
Surface Loop(123) = {73, 70, 77, 8, 61};
Volume(124) = {123};
Surface Loop(125) = {53, 56, 60, 44, 61};
Volume(126) = {125};
Surface Loop(127) = {27, 36, 39, 43, 44};
Volume(128) = {127};
Surface Loop(129) = {84, 10, 89};
Volume(130) = {129};
Surface Loop(131) = {120, 73, 113};
Volume(132) = {131};
Surface Loop(133) = {108, 101, 113};
Volume(134) = {133};
Surface Loop(135) = {96, 101, 89};
Volume(136) = {135};

d1 = 1;
d2 = 1;
d3 = 1;
d4 = 1;
n1 = 10;
n2 = 10;
n3 = 10;
n4 = 10;
Transfinite Line {2, 46, 29, 12, 4} = n1 Using Progression d1;
Transfinite Line {1, 49, 32, 15, 3, 47, 30, 13} = n2 Using Progression d2;
Transfinite Line {68, 51, 34, 17, 18, 69, 52, 35} = n3 Using Progression d3;
Transfinite Line {6, 103, 91, 79} = n4 Using Progression d4;
Transfinite Surface "*";
Transfinite Volume "*";
Recombine Surface "*";
Coherence;
Physical Surface("inlet") = {77, 26, 43, 60};
Physical Surface("gate") = {73, 56, 39, 22};
Physical Surface("walls") = {19, 70, 53, 36};
Physical Surface("sac") = {84, 120, 108, 96};
Physical Volume("fluidPipe") = {3, 2, 1, 4};
Physical Volume("fluidSac") = {7, 6, 5, 8};


tareqkh March 25, 2017 14:59

1 Attachment(s)
Hi,

I have spent sometime on your weird pipe mesh and here is the code as well as a 3D picture of it;

Code:

Point(1) = {0, 0.1, 0, 0};
Point(2) = {10, 0.1, 0, 0};
Point(3) = {0, 1, 0, 0};
Point(4) = {10, 1, 0, 0};
Point(5) = {14, 0.1, 0, 0};
Point(6) = {11.9, 0.1, 0, 0.0};
Line(1) = {4,2};
Line(2) = {2,1};
Line(3) = {1,3};
Line(4) = {3,4};
Point(7) = {11.9, 2.2, 0, 0.0};
Circle(5) = {5, 6, 7};
Circle(6) = {7, 6, 4};
Line(7) = {5, 2};

Line Loop(8) = {4, 1, 2, 3};
Plane Surface(9) = {8};
Line Loop(10) = {6, 1, -7, 5};
Plane Surface(11) = {10};
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{9, 11};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{55, 33};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{77, 99};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{121, 143};
}
Surface Loop(186) = {20, 32, 28, 9, 33, 24};
Volume(187) = {186};
Surface Loop(188) = {33, 86, 98, 94, 99, 68};
Volume(189) = {188};
Surface Loop(190) = {9, 173, 185, 181, 143, 156};
Volume(191) = {190};
Surface Loop(192) = {143, 99, 142, 130, 138, 112};
Volume(193) = {192};
Surface Loop(194) = {11, 42, 54, 50, 24, 55};
Volume(195) = {194};
Surface Loop(196) = {55, 77, 64, 76, 72, 68};
Volume(197) = {196};
Surface Loop(198) = {11, 121, 152, 164, 160, 156};
Volume(199) = {198};
Surface Loop(200) = {121, 77, 120, 108, 116, 112};
Volume(201) = {200};
d1 = 1;
d2 = 1;
n1 = 30;
n2 = 30;
Transfinite Line {2, 15, 125, 81, 4, 123, 79, 13} = n1 Using Progression d1;
Transfinite Line {3, 126, 82, 16, 3, 1, 102, 58, 14} = n2 Using Progression d2;
Transfinite Line {7, 103, 37, 59, 6, 5, 101, 104, 57, 60, 35, 38} = n1 Using Progression d1;
Transfinite Line {171, 18, 84, 128, 180, 27, 93, 137, 19, 151, 107, 63, 23, 155, 111, 67} = 18 Using Progression 1;
Transfinite Line {40, 150, 62, 106, 49, 159, 115, 71} = 18 Using Progression 1;
Transfinite Surface "*";
Transfinite Volume "*";
Recombine Surface "*";
Coherence;

Attachment 54902

Let me know how it goes with you.

Cheers,

Khamlaj

j_moulton March 25, 2017 15:31

Quote:

Originally Posted by tareqkh (Post 642272)
Hi,

I have spent sometime on your weird pipe mesh and here is the code as well as a 3D picture of it;

Let me know how it goes with you.

Cheers,

Khamlaj

Thank you for doing that Khamlaj. I was hoping to get some clarification on my original question, though. Also, I think you misunderstood my model... I just need a pipe with a bulb on the end. I'm not sure where the idea for a smaller pipe inside came from.

j_moulton March 25, 2017 15:38

Quote:

Originally Posted by CFD-Lover (Post 641477)
Hi Jeremy,

I have looked through your code and was able to recreate it for you. Here is the code;
Cheers,

Hi, thank you. There is an issue. When I use this mesh in OpenFOAM, there is actually some object (a 1D wall?) down the center line (see below). How can I eliminate this?

https://photos-5.dropbox.com/t/2/AAB...36&size_mode=3

tareqkh March 25, 2017 16:34

Can you show it?

tareqkh March 25, 2017 17:50

1 Attachment(s)
Here is the new mesh without the inner pipe;

Code:

Point(1) = {0, 0.0, 0, 0};
Point(2) = {10, 0.0, 0, 0};
Point(3) = {0, 0.9, 0, 0};
Point(4) = {10, 0.9, 0, 0};
Line(1) = {4, 2};
Line(2) = {2, 1};
Line(3) = {1, 3};
Line(4) = {3, 4};
Point(5) = {14, 0.0, 0, 0};
Point(6) = {11.9, 0.0, 0, 0.0};
Point(7) = {11.9, 2.1, 0, 0.0};
Circle(5) = {5, 6, 7};
Circle(6) = {7, 6, 4};
Line(7) = {5, 2};
Line Loop(8) = {4, 1, 2, 3};
Plane Surface(9) = {8};
Line Loop(10) = {6, 1, -7, 5};
Plane Surface(11) = {10};
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{9, 11};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{28, 45};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{62, 79};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{96, 113};
}
Surface Loop(146) = {20, 27, 9, 28, 23};
Volume(147) = {146};
Surface Loop(148) = {28, 62, 54, 61, 57};
Volume(149) = {148};
Surface Loop(150) = {9, 122, 129, 96, 125};
Volume(151) = {150};
Surface Loop(152) = {96, 88, 95, 62, 91};
Volume(153) = {152};
Surface Loop(154) = {11, 37, 44, 45, 23};
Volume(155) = {154};
Surface Loop(156) = {45, 79, 78, 71, 57};
Volume(157) = {156};
Surface Loop(158) = {11, 113, 138, 145, 125};
Volume(159) = {158};
Surface Loop(160) = {113, 79, 105, 112, 91};
Volume(161) = {160};
d1 = 1;
d2 = 1;
d3 = 1;
d4 = 1;
n1 = 30;
n2 = 30;
n3 = 18;
Transfinite Line {2, 4, 81, 47, 13, 7, 6, 5, 98, 101, 64, 67, 30, 33} = n1 Using Progression d1;
Transfinite Line {3, 84, 50, 16, 1, 82, 48, 14} = n2 Using Progression d2;
Transfinite Line {120, 18, 52, 86, 121, 19, 53, 87, 136, 35, 69, 103} = n3 Using Progression d3;
Transfinite Surface "*";
Transfinite Volume "*";
Recombine Surface "*";

Attachment 54903

Now, it is your job to complete the rest.

Cheers,

j_moulton April 3, 2017 21:17

Quote:

Originally Posted by tareqkh (Post 642288)
Here is the new mesh without the inner pipe;

Now, it is your job to complete the rest.

Cheers,

Thank you, but this didn't actually work with gmshToFoam:

Code:

--> FOAM Warning : Not using gmsh face 4(16055 823 6 155) since zero vertex is not on boundary of polyMesh

FaceZones:
Zone        Size
    0        16588

Writing zone 0 to cellZone cellZone_0 and cellSet
Writing zone 0 to faceZone faceZone_0 and faceSet
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigSegv::sigHandler(int) at ??:?
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  ? at ??:?
#4  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#5  ? at ??:?
Segmentation fault


cksanjay December 26, 2020 00:43

Quote:

Originally Posted by tareqkh (Post 642288)
Here is the new mesh without the inner pipe;

Code:

Point(1) = {0, 0.0, 0, 0};
Point(2) = {10, 0.0, 0, 0};
Point(3) = {0, 0.9, 0, 0};
Point(4) = {10, 0.9, 0, 0};
Line(1) = {4, 2};
Line(2) = {2, 1};
Line(3) = {1, 3};
Line(4) = {3, 4};
Point(5) = {14, 0.0, 0, 0};
Point(6) = {11.9, 0.0, 0, 0.0};
Point(7) = {11.9, 2.1, 0, 0.0};
Circle(5) = {5, 6, 7};
Circle(6) = {7, 6, 4};
Line(7) = {5, 2};
Line Loop(8) = {4, 1, 2, 3};
Plane Surface(9) = {8};
Line Loop(10) = {6, 1, -7, 5};
Plane Surface(11) = {10};
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{9, 11};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{28, 45};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{62, 79};
}
Extrude {{1, 0, 0}, {0, 0, 0}, Pi/2} {
  Surface{96, 113};
}
Surface Loop(146) = {20, 27, 9, 28, 23};
Volume(147) = {146};
Surface Loop(148) = {28, 62, 54, 61, 57};
Volume(149) = {148};
Surface Loop(150) = {9, 122, 129, 96, 125};
Volume(151) = {150};
Surface Loop(152) = {96, 88, 95, 62, 91};
Volume(153) = {152};
Surface Loop(154) = {11, 37, 44, 45, 23};
Volume(155) = {154};
Surface Loop(156) = {45, 79, 78, 71, 57};
Volume(157) = {156};
Surface Loop(158) = {11, 113, 138, 145, 125};
Volume(159) = {158};
Surface Loop(160) = {113, 79, 105, 112, 91};
Volume(161) = {160};
d1 = 1;
d2 = 1;
d3 = 1;
d4 = 1;
n1 = 30;
n2 = 30;
n3 = 18;
Transfinite Line {2, 4, 81, 47, 13, 7, 6, 5, 98, 101, 64, 67, 30, 33} = n1 Using Progression d1;
Transfinite Line {3, 84, 50, 16, 1, 82, 48, 14} = n2 Using Progression d2;
Transfinite Line {120, 18, 52, 86, 121, 19, 53, 87, 136, 35, 69, 103} = n3 Using Progression d3;
Transfinite Surface "*";
Transfinite Volume "*";
Recombine Surface "*";

Attachment 54903

Now, it is your job to complete the rest.

Cheers,

Hi ,
I am running with the similar issue while converting from gmsh to Foam , can you help me resolve this issue. Its a case of a cube obstacle in a sqaure domain.my error is as below,


--> FOAM FATAL IO ERROR:
No cells read from file "demo2.msh"
Does your file specify any 3D elements (hex=5, prism=6, pyramid=7, tet=4)?
Perhaps you have not exported the 3D elements?

file: demo2.msh at line 5711.

From function void readCells(Foam::scalar, bool, const pointField&, const Foam::Map<int>&, Foam::IFstream&, Foam::cellShapeList&, Foam::labelList&, Foam::List<Foam::DynamicList<Foam::face> >&, Foam::labelList&, Foam::List<Foam::DynamicList<int> >&)
in file gmshToFoam.C at line 726.

FOAM exiting




I also attach my .geo file here below for your reference.Thanks in advance



// Gmsh project created on Thu Dec 24 12:46:26 2020
SetFactory("OpenCASCADE");
//+
Point(1) = {0, 0, 0, 1.0};
//+
Point(4) = {30, 0, 0, 1.0};
//+
Point(5) = {40, 0, 0, 1.0};
//+
Point(6) = {40, 30, 0, 1.0};
//+
Point(7) = {30, 30, 0, 1.0};
//+
Point(8) = {0, 30, 0, 1.0};
//+
//square obstacle
Point(9) = {10, 20, 0, 1.0};
//+
Point(10) = {10, 10, 0, 1.0};
//+
Point(11) = {20, 10, 0, 1.0};
//+
Point(12) = {20, 20, 0, 1.0};
//boundary lines
//+
Line(1) = {8, 7};Transfinite Curve {1} = 11 Using Progression 1;
//+
Line(2) = {7, 6};Transfinite Curve {2} = 11 Using Progression 1;
//+
Line(3) = {6, 5}; //outlet line
//+
Line(4) = {5, 4};Transfinite Curve {4} = 11 Using Progression 1;
//+
Line(5) = {4, 1};Transfinite Curve {5} = 11 Using Progression 1;
//+
Line(6) = {1, 8};//inlet line
//+


//square obstacle
Line(7) = {9, 12};
//+
Line(8) = {12, 11};
//+
Line(9) = {11, 10};
//+
Line(10) = {10, 9};


//obstacle connection
//+
Line(11) = {8, 9};
//+
Line(12) = {7, 12};
//+
Line(13) = {7, 4};//boundary connection
//+
Line(14) = {4, 11};
//+
Line(15) = {1, 10};

//Surfaces
//+
Curve Loop(1) = {11, 7, -12, -1};
//+
Plane Surface(1) = {1};
//+
Curve Loop(2) = {12, 8, -14, -13};
//+
Plane Surface(2) = {2};
//+
Curve Loop(3) = {14, 9, -15, -5};
//+
Plane Surface(3) = {3};
//+
Curve Loop(4) = {15, 10, -11, -6};
//+
Plane Surface(4) = {4};
//+
Curve Loop(5) = {2, 3, 4, -13};
//+
Plane Surface(5) = {5};
//+
Recombine Surface {4};
//+
Recombine Surface {1};
//+
Recombine Surface {2};
//+
Recombine Surface {3};
//+
Extrude {0, 0, 1} {
Surface{1}; Surface{2}; Surface{3}; Surface{4}; Surface{5};
Layers{1};
Recombine;
}



//boundary conditions
//+
Physical Surface("inlet") = {20};
//+
Physical Surface("outlet") = {23};
//+
Physical Surface("bottom wall") = {9, 22};
//+
Physical Surface("top wall") = {24, 17};
//+
Physical Surface("obstacle wall") = {19, 15, 11, 7};
//+
Physical Surface("front and back") = {18, 21, 10, 14, 25, 5, 3, 4, 1, 2};


All times are GMT -4. The time now is 01:32.