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};

chrisyang October 6, 2022 21:58
Hi,

I think you also miss adding the physical volume for your geometry, like the posts discussed above in this thread, since OpenFOAM only take care of the 3D mesh.


All times are GMT -4. The time now is 00:23.