CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

This mesh contains patches of type empty but is not 1D or 2D

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 9, 2009, 09:45
Default
  #21
tgj
New Member
 
Join Date: Dec 2009
Posts: 3
Rep Power: 7
tgj is on a distinguished road
ok, tried that... (simply set the boundary to patch in the boundary file generated by blockMesh)
it requires me to set the boundary conditions for p... when i set them to zeroGradient, i get
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading field p

Programme terminated with errors: exit code 3, status 0.

with no further explanation... when i set it to fixedValue and value 0, it works, but, of course, shows the same problems for the other variables (U, epsilon, NuTilda, R, k): won't work with zeroGradient, but does with fixedValue 0... but when i set all of them to fixedValue 0, i get

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

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon

Starting time loop

Time = 1

Programme terminated with errors: exit code 3, status 0.


again without explanation... really don't know what to do (the simulation worked fine before i put the "obstacle" into it)
tgj is offline   Reply With Quote

Old   March 10, 2010, 10:54
Default
  #22
Member
 
Nick Gardiner
Join Date: Apr 2009
Location: Chichester, UK
Posts: 93
Rep Power: 8
NickG is on a distinguished road
Hi

bobby - your mesh is 3D in case you hadn't found out yet. i.e you have more than two different z values

I'm having a similar problem re

This mesh contains patches of type empty but is not 1D or 2D
by virtue of the fact that the number of faces of this
empty patch is not divisible by the number of cells...

I've merged two meshes in order to be able to rotate one of them inside the other. They work individually as empty meshes, and merged when described as symmetryPlane, but I'd like to be able to use the empty BC for the combined mesh.

Any suggestions anyone?

Thanks

Nick
NickG is offline   Reply With Quote

Old   June 3, 2010, 08:37
Default The mes contains patches of type empty
  #23
New Member
 
Gaurav
Join Date: Jun 2010
Location: Bangalore, India
Posts: 12
Rep Power: 6
PaGgiE is on a distinguished road
Hi,
I am trying to run a 2D fluid flow with an obstacle in its path and it is able to creat the mesh proprly but when i run icoFoam its giving the error as:




Create time

Create mesh for time = 0

Reading transportProperties

Reading field p

Reading field U

Reading/calculating face flux field phi


Starting time loop

Time = 0.005

Courant Number mean: 0 max: 7.5


This mesh contains patches of type empty but is not 1D or 2D
by virtue of the fact that the number of faces of this
empty patch is not divisible by the number of cells.

From function emptyFvPatchField<Type>::updateCoeffs()
in file fields/fvPatchFields/constraint/empty/emptyFvPatchField.C at line 148.

FOAM exiting



Can anyone suggest what is the problem?
Do i need to use any other solver than icoFoam?
or is there any problem with the mesh as while running blockMesh, i got a warning as
:


Creating blockCorners

Creating curved edges

Creating blocks

Creating patches

Creating block mesh topology

Default patch type set to empty
--> FOAM Warning :
From function polyMesh:olyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 577
Found 8 undefined faces in mesh; adding to default patch.

Check block mesh topology

Basic statistics
Number of internal faces : 0
Number of boundary faces : 24
Number of defined boundary faces : 24
Number of undefined boundary faces : 0

Checking patch -> block consistency

Creating block offsets

Creating merge list .

Creating points with scale 1

Creating cells

Creating patches

Creating mesh from block mesh

Default patch type set to empty

Writing polyMesh

End



The blockMesh code is as follows:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
(0 0 0)
(0.4 0 0)
(0.6 0 0)
(1 0 0)
(0.4 0.2 0)
(0.6 0.2 0)
(0.4 0.4 0)
(0.6 0.4 0)
(0 0.6 0)
(0.4 0.6 0)
(0.6 0.6 0)
(1 0.6 0)
(0 0 0.1)
(0.4 0 0.1)
(0.6 0 0.1)
(1 0 0.1)
(0.4 0.2 0.1)
(0.6 0.2 0.1)
(0.4 0.4 0.1)
(0.6 0.4 0.1)
(0 0.6 0.1)
(0.4 0.6 0.1)
(0.6 0.6 0.1)
(1 0.6 0.1)
);

blocks
(
hex (0 1 9 8 12 13 21 20) (30 45 1) simpleGrading (1 1 1)
hex (1 2 5 4 13 14 17 16) (15 15 1) simpleGrading (1 1 1)
hex (2 3 11 10 14 15 23 22) (30 45 1) simpleGrading (1 1 1)
hex (6 7 10 9 18 19 22 21) (15 15 1) simpleGrading (1 1 1)

);

edges
(
);

patches
(
patch
inlet
(
(0 8 20 12)
)

patch
outlet
(
(11 3 15 23)
)

wall upperWalls
(
(8 9 21 20)
(10 11 23 22)
(6 7 19 18)
(9 10 22 21)
)

wall lowerWalls
(
(1 0 12 13)
(3 2 14 15)
(5 4 16 17)
(2 1 13 14)
)

empty frontAndBack
(
(9 8 0 1)
(10 9 6 7)
(5 4 1 2)
(11 10 2 3)
(20 21 13 12)
(21 22 19 18)
(16 17 14 13)
(22 23 15 14)
)
);

mergePatchPairs
(
);

// ************************************************** *********************** //
PaGgiE is offline   Reply With Quote

Old   June 3, 2010, 08:49
Default
  #24
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,571
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
You need to create the mesh using 8 blocks instead those 4 you have used. Two neighbouring blocks need to have a one-to-one match. Read the manual if in doubt.

Best regards,

Niels
ngj is offline   Reply With Quote

Old   June 3, 2010, 09:16
Default blockMesh warning || mesh contains patches of type empty
  #25
New Member
 
Gaurav
Join Date: Jun 2010
Location: Bangalore, India
Posts: 12
Rep Power: 6
PaGgiE is on a distinguished road
Thank you for reply Niels.
I've converted it into 8 blocks...but still this error is there while running icoFoam :

This mesh contains patches of type empty but is not 1D or 2D
by virtue of the fact that the number of faces of this
empty patch is not divisible by the number of cells.

From function emptyFvPatchField<Type>::updateCoeffs()
in file fields/fvPatchFields/constraint/empty/emptyFvPatchField.C at line 148.

FOAM exiting


But while running blockMesh, now the warning is only for 2 faces. I'm not getting which 2 faces are left?


Create time


Creating block mesh from
"/home/gaurav/OpenFOAM/gaurav-1.6/run/tutorials/incompressible/icoFoam/obstacle/constant/polyMesh/blockMeshDict"


Creating blockCorners

Creating curved edges

Creating blocks

Creating patches

Creating block mesh topology

Default patch type set to empty
--> FOAM Warning :
From function polyMesh:olyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 577
Found 2 undefined faces in mesh; adding to default patch.

Check block mesh topology

Basic statistics
Number of internal faces : 8
Number of boundary faces : 32
Number of defined boundary faces : 32
Number of undefined boundary faces : 0

Checking patch -> block consistency

Creating block offsets

Creating merge list .

Creating points with scale 1

Creating cells

Creating patches

Creating mesh from block mesh

Default patch type set to empty

Writing polyMesh

End


The blockMeshDict code is is as follows:


/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
(0 0 0)
(0.4 0 0)
(0.6 0 0)
(1 0 0)
(0 0.2 0)
(0.4 0.2 0)
(0.6 0.2 0)
(1 0.2 0)
(0 0.4 0)
(0.4 0.4 0)
(0.6 0.4 0)
(1 0.4 0)
(0 0.6 0)
(0.4 0.6 0)
(0.6 0.6 0)
(1 0.6 0)
(0 0 0.1)
(0.4 0 0.1)
(0.6 0 0.1)
(1 0 0.1)
(0 0.2 0.1)
(0.4 0.2 0.1)
(0.6 0.2 0.1)
(1 0.2 0.1)
(0 0.4 0.1)
(0.4 0.4 0.1)
(0.6 0.4 0.1)
(1 0.4 0.1)
(0 0.6 0.1)
(0.4 0.6 0.1)
(0.6 0.6 0.1)
(1 0.6 0.1)
);

blocks
(
hex (0 1 5 4 16 17 21 20) (30 15 1) simpleGrading (1 1 1)
hex (1 2 6 5 17 18 22 21) (15 15 1) simpleGrading (1 1 1)
hex (2 3 7 6 18 19 23 22) (30 15 1) simpleGrading (1 1 1)
hex (4 5 9 8 20 21 25 24) (30 15 1) simpleGrading (1 1 1)
hex (6 7 11 10 22 23 27 26) (30 15 1) simpleGrading (1 1 1)
hex (8 9 13 12 24 25 29 28) (30 15 1) simpleGrading (1 1 1)
hex (9 10 14 13 25 26 30 29) (15 15 1) simpleGrading (1 1 1)
hex (10 11 15 14 26 27 31 30) (30 15 1) simpleGrading (1 1 1)

);

edges
(
);

patches
(
patch
inlet
(
(0 4 20 16)
(4 8 24 20)
(8 12 28 24)
)

patch
outlet
(
(3 19 23 7)
(7 23 27 11)
(11 27 31 15)
)

wall upperWalls
(
(12 13 29 28)
(14 15 31 30)
(13 14 30 29)
(9 10 26 25)
)

wall lowerWalls
(
(1 0 16 17)
(3 2 18 19)
(2 1 17 18)
(5 6 22 21)
)

empty frontAndBack
(
(0 1 5 4)
(1 2 6 5)
(2 3 7 6)
(4 5 9 8)
(6 7 11 10)
(8 9 13 12)
(9 10 14 13)
(10 11 15 14)
(20 21 17 16)
(21 22 18 17)
(22 23 19 18)
(24 25 21 20)
(26 27 23 22)
(28 29 25 24)
(29 30 26 25)
(30 31 27 26)
)
);

mergePatchPairs
(
);

// ************************************************** *********************** //
PaGgiE is offline   Reply With Quote

Old   June 3, 2010, 09:50
Default
  #26
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,571
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Try the vertical walls inside the square.

Best regards,

Niels
ngj is offline   Reply With Quote

Old   June 3, 2010, 10:22
Default mesh contains patches of type empty
  #27
New Member
 
Gaurav
Join Date: Jun 2010
Location: Bangalore, India
Posts: 12
Rep Power: 6
PaGgiE is on a distinguished road
Thank you Niels for your reply.
I've included those 2 faces and now its working properly
PaGgiE is offline   Reply With Quote

Old   June 3, 2010, 10:31
Default
  #28
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,571
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Good.

In the future you can benefit from looking at the mesh in paraFoam before asking questions on the Forum.

Best regards,

Niels
ngj is offline   Reply With Quote

Old   June 26, 2010, 08:23
Default merged meshes
  #29
Member
 
Nick Gardiner
Join Date: Apr 2009
Location: Chichester, UK
Posts: 93
Rep Power: 8
NickG is on a distinguished road
Hi - those with this problem that have merged meshes or more than one empty patch

I've just found that if you merge meshes with empty BCs on more than one of the previously separate meshes then they won't work unless you create a new single patch that includes the multiple patches. That is unless they have an equal quantity of faces whereby you won't get this division by number of cells problem.

The only problem with this is that they need to be numerically sequential in the merged mesh to be able to rewrite the number of faces in /boundary (as the sum the previously separate empty nFaces).

e.g.

zSymT
{
type empty;
nFaces 15438;
startFace 66386;
}
ASymR
{
type empty;
nFaces 69208;
startFace 81824;
}

becomes:

Sym
{
type empty;
nFaces 84646;
startFace 66386;
}

Hope that helps others
NickG is offline   Reply With Quote

Old   July 26, 2010, 22:12
Default Undefined and unconsistent
  #30
Member
 
Join Date: Dec 2009
Posts: 39
Rep Power: 7
marval is on a distinguished road
This is my blockMesh file some text in swedish:

Quote:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: http://www.openfoam.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "";
case "";
instance "";
local "";

class dictionary;
object blockMeshDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Vinklad Kanal
convertToMeters 0.001;

vertices
( // y = 0
(0 0 10) // 0
(480 0 10)
(490 0 10)
(500 0 10)

(0 0 20) // 4
(480 0 20)
(490 0 20)
(500 0 20)

(0 0 30) // 8
(480 0 30)
(490 0 30)
(500 0 30)

(0 0 35) // 12
(480 0 35)
(490 0 35)
(500 0 35)

(0 0 45) // 16
(480 0 45)
(490 0 45)
(500 0 45)

(0 0 55) // 20
(480 0 55)
(490 0 55)
(500 0 55)

// y = 8
(0 8 5) // 24
(480 8 5)
(490 8 5)
(500 8 5)

(0 8 10) // 28
(480 8 10)
(490 8 10)
(500 8 10)

(0 8 20) // 32
(480 8 20)
(490 8 20)
(500 8 20)

(0 8 30) // 36
(480 8 30)
(490 8 30)
(500 8 30)

(0 8 35) // 40
(480 8 35)
(490 8 35)
(500 8 35)

(0 8 45) // 44
(480 8 45)
(490 8 45)
(500 8 45)

(0 8 55) // 48
(480 8 55)
(490 8 55)
(500 8 55)

// y = 16
(0 16 0) // 52
(480 16 0)
(490 16 0)
(500 16 0)

(0 16 5) // 56
(480 16 5)
(490 16 5)
(500 16 5)

(0 16 10) // 60
(480 16 10)
(490 16 10)
(500 16 10)

(0 16 20) // 64
(480 16 20)
(490 16 20)
(500 16 20)

(0 16 30) // 68
(480 16 30)
(490 16 30)
(500 16 30)

(0 16 35) // 72
(480 16 35)
(490 16 35)
(500 16 35)

(0 16 45) // 76
(480 16 45)
(490 16 45)
(500 16 45)

(0 16 55) // 80
(480 16 55)
(490 16 55)
(500 16 55)
);

blocks
( // hex (24 25 1 0 24 25 29 28)
// hex (25 26 2 1 25 26 30 29)
// hex (26 27 3 2 26 27 31 30)

// Undre delen
hex (0 1 25 24 0 1 29 28) (480 8 5) simpleGrading (1 1 1) //(0.1 10 10) //0
hex (1 2 26 25 1 2 30 29) (10 8 5) simpleGrading (1 1 1) //(10 10 10)
hex (2 3 27 26 2 3 31 30) (10 8 5) simpleGrading (1 1 1) //(0.1 10 10)

hex (0 1 29 28 4 5 33 32) (480 8 10) simpleGrading (1 1 1) //(0.1 10 10)
hex (1 2 30 29 5 6 34 33) (10 8 10) simpleGrading (1 1 1) //(10 10 10) //4
hex (2 3 31 30 6 7 35 34) (10 8 10) simpleGrading (1 1 1) //(0.1 10 10)

hex (4 5 33 32 8 9 37 36) (480 8 10) simpleGrading (1 1 1) //(0.1 10 0.1)
hex (5 6 34 33 9 10 38 37) (10 8 10) simpleGrading (1 1 1) //(10 10 0.1)
hex (6 7 35 34 10 11 39 38) (10 8 10) simpleGrading (1 1 1) //(0.1 10 0.1) //8

hex (9 10 38 37 13 14 42 41) (10 8 5) simpleGrading (1 1 1) //(10 10 1)
hex (10 11 39 38 14 15 43 42) (10 8 5) simpleGrading (1 1 1) //(0.1 10 1)

hex (12 13 41 40 16 17 45 44) (480 8 10) simpleGrading (1 1 1) //(0.1 10 10)
hex (13 14 42 41 17 18 46 45) (10 8 10) simpleGrading (1 1 1) //(10 10 10) //12
hex (14 15 43 42 18 19 47 46) (10 8 10) simpleGrading (1 1 1) //(0.1 10 10)

hex (16 17 45 44 20 21 49 48) (480 8 10) simpleGrading (1 1 1) //(0.1 10 0.1)
hex (17 18 46 45 21 22 50 49) (10 8 10) simpleGrading (1 1 1) //(10 10 0.1)
hex (18 19 47 46 22 23 51 50) (10 8 10) simpleGrading (1 1 1) //(0.1 10 0.1) //16

// hex (52 53 25 24 52 53 57 56)
// hex (53 54 26 25 53 54 58 57)
// hex (54 55 27 26 54 55 59 58)

// Övre delen
hex (24 25 53 52 24 25 57 56) (480 8 5) simpleGrading (1 1 1) //(0.1 0.1 10)
hex (25 26 54 53 25 26 58 57) (10 8 5) simpleGrading (1 1 1) //(10 0.1 10)
hex (26 27 55 54 26 27 59 58) (10 8 5) simpleGrading (1 1 1) //(0.1 0.1 10)

hex (24 25 57 56 28 29 61 60) (480 8 10) simpleGrading (1 1 1) //(0.1 0.1 10) //20
hex (25 26 58 57 29 30 62 61) (10 8 10) simpleGrading (1 1 1) //(10 0.1 10)
hex (26 27 59 58 30 31 63 62) (10 8 10) simpleGrading (1 1 1) //(0.1 0.1 10)

hex (28 29 61 60 32 33 65 64) (480 8 10) simpleGrading (1 1 1) //(0.1 0.1 10)
hex (29 30 62 61 33 34 66 65) (100 8 10) simpleGrading (1 1 1) //(10 0.1 10) //24
hex (30 31 63 62 34 35 67 66) (100 8 10) simpleGrading (1 1 1) //(0.1 0.1 10)

hex (32 33 65 64 36 37 69 68) (480 8 10) simpleGrading (1 1 1) //(0.1 0.1 0.1)
hex (33 34 66 65 37 38 70 69) (10 8 10) simpleGrading (1 1 1) //(10 0.1 0.1)
hex (34 35 67 66 38 39 71 70) (10 8 10) simpleGrading (1 1 1) //(0.1 0.1 0.1) //28

hex (37 38 70 69 41 42 74 73) (10 8 5) simpleGrading (1 1 1) //(10 0.1 1)
hex (38 39 71 70 42 43 75 74) (10 8 5) simpleGrading (1 1 1) //(0.1 0.1 1)

hex (40 41 73 72 44 45 77 76) (480 8 10) simpleGrading (1 1 1) //(0.1 0.1 10)
hex (41 42 74 73 45 46 78 77) (10 8 10) simpleGrading (1 1 1) //(10 0.1 10) //32
hex (42 43 75 74 46 47 79 78) (10 8 10) simpleGrading (1 1 1) //(0.1 0.1 10)

hex (44 45 77 76 48 49 81 80) (480 8 10) simpleGrading (1 1 1) //(0.1 0.1 0.1)
hex (45 46 78 77 49 50 82 81) (10 8 10) simpleGrading (1 1 1) //(10 0.1 0.1)
hex (46 47 79 78 50 51 83 82) (10 8 10) simpleGrading (1 1 1) //(0.1 0.1 0.1) //36

);

edges
(
);

patches
(

wall cellWall
(
(56 57 53 52) // Cellyta //0
(57 58 54 53)
(58 59 55 54)

(60 61 57 56)
(61 62 58 57) //4
(62 63 59 58)

(64 65 61 60)
(65 66 62 61)
(66 67 63 62) //8

(68 69 65 64)
(69 70 66 65)
(70 71 67 66)

(73 74 70 69) //12
(74 75 71 70)

(76 77 73 72)
(77 78 74 73)
(78 79 75 74) //16

(80 81 77 76)
(81 82 78 77)
(82 83 79 78)
)

wall walls
( // Omslutande
(1 0 24 25) // Undre delen //20
(2 1 25 26)
(3 2 26 27)
(3 27 31 3) // Triangulär väggdel
(7 3 31 35) //24
(11 7 35 39)
(15 11 39 43)
(19 15 43 47)
(23 19 47 51) //28
(22 23 51 50)
(21 22 50 49)
(20 21 49 48)

(25 24 52 53) // Övre delen //32
(26 25 53 54)
(27 26 54 55)
(27 55 59 27) // Triangulär väggdel
(31 27 59 63) //36
(35 31 63 67)
(39 35 67 71)
(43 39 71 75)
(47 43 75 79) //40
(51 47 79 83)
(50 51 83 82)
(49 50 82 81)
(48 49 81 80) //44

//Inre kanalvägg
(8 9 37 36) // Undre delen
(9 13 41 37)
(13 12 40 41)

(36 37 69 68) // Övre delen //48
(37 41 73 69)
(41 40 72 73)

(0 1 5 4) // Golvet
(1 2 6 5) //52
(2 3 7 6)

(4 5 9 8)
(5 6 10 9)
(6 7 11 10) //56

(9 10 14 13)
(10 11 15 14)

(12 13 17 16)
(13 14 18 17) //60
(14 15 19 18)

(16 17 21 20)
(17 18 22 21)
(18 19 23 22) //64
)

patch inlet
( // Undre delen
(0 28 24 0) // Triangulär
(0 4 32 28)
(4 8 36 32)

// Övre delen
(24 56 52 24) // Triangulär //68
(24 28 60 56)
(28 32 64 60)
(32 36 68 64)
)

patch outlet
( // Undre delen
(12 16 44 40) //72
(16 20 48 44)
// Övre delen
(40 44 76 72)
(44 48 80 76)
)

);

mergePatchPairs
(
);

// ************************************************** *********************** //
But when I try blockMesh i get the following:

Quote:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.6.x-7ed1455df0ff
Exec : blockMesh
Date : Jul 27 2010
Time : 03:57:01
Host : marco-laptop
PID : 24010
Case : /home/marco/OpenFOAM/marco-1.6.x/run/run/vinkladHeatChannel
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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


Creating block mesh from
"/home/marco/OpenFOAM/marco-1.6.x/run/run/vinkladHeatChannel/constant/polyMesh/blockMeshDict"


Creating blockCorners

Creating curved edges

Creating blocks

Creating patches

Creating block mesh topology

Default patch type set to empty
--> FOAM Warning :
From function polyMesh:olyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 577
Found 6 undefined faces in mesh; adding to default patch.

Check block mesh topology

Basic statistics
Number of internal faces : 70
Number of boundary faces : 82
Number of defined boundary faces : 82
Number of undefined boundary faces : 0

Checking patch -> block consistency

Creating block offsets

Creating merge list

--> FOAM FATAL ERROR:
Inconsistent number of faces between block pair 0 and 20

From function blockMesh::createMergeList()
in file createMergeList.C at line 196.

FOAM exiting
I don't see how they are inconsistent. :/

And btw, how to find the 6 undefined faces?

Thanks in advance!

Regards
Marco
marval is offline   Reply With Quote

Old   August 30, 2010, 04:53
Default
  #31
New Member
 
David
Join Date: Aug 2010
Location: North Ossetia, Vladikavkaz
Posts: 27
Rep Power: 6
davidmd is on a distinguished road
Send a message via ICQ to davidmd
i'm trying to generate mesh for axisymmetric.
this is my blockMesh:

convertToMeters 0.1;

vertices
(
(0 0 0)
(10 0 0)
(9.988 0.491 0)
(0 0 10)
(10 0 10)
(9.988 0.491 10)
);

blocks
(
hex (0 1 2 3 4 5) (5 5 5) simpleGrading (1 1 1)
);

edges
(
arc 2 3 (0.9997 0.0245 0)
arc 6 7 (0.9997 0.0245 1)
);

patches

(
patch movingWall
(
(0 1 2 0)
)
wall fixedWalls
(
(3 3 4 5)
(1 4 5 2)
)
symmetryPlane axis
(
(0 3 3 0)
)
wedge front
(
(0 3 4 1)
)
wedge back
(
(0 3 5 2)
)
);

mergePatchPairs
(
);

And this is my error:

Create time


Creating block mesh from
"/home/david/OpenFOAM/david-1.7.0/run/tutorials/incompressible/icoFoam/cavmod/constant/polyMesh/blockMeshDict"


Creating blockCorners

Creating curved edges

Creating blocks
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam170/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/opt/openfoam170/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3
in "/opt/openfoam170/applications/bin/linuxGccDPOpt/blockMesh"
#4
in "/opt/openfoam170/applications/bin/linuxGccDPOpt/blockMesh"
#5
in "/opt/openfoam170/applications/bin/linuxGccDPOpt/blockMesh"
#6
in "/opt/openfoam170/applications/bin/linuxGccDPOpt/blockMesh"
#7
in "/opt/openfoam170/applications/bin/linuxGccDPOpt/blockMesh"
#8 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#9
in "/opt/openfoam170/applications/bin/linuxGccDPOpt/blockMesh"
sigmentation error.

Maybe someone can help?
:/

davidmd is offline   Reply With Quote

Old   May 28, 2013, 04:02
Default help
  #32
Member
 
Join Date: Oct 2012
Posts: 47
Rep Power: 4
sh.d is on a distinguished road
i want to create 2d mesh a round airfoil but when use checkMesh is this error:Number of edges not aligned with or perpendicular to non-empty directions
can you help me please?
the surface of airfoil not snap!
sh.d is offline   Reply With Quote

Old   May 28, 2013, 05:58
Default
  #33
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,571
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Hi SH,

Please read the following wiki-page and then come back and rephrase your question:

http://openfoamwiki.net/index.php/Ho..._Message_Board

Kind regards

Niels
ngj is offline   Reply With Quote

Old   May 28, 2013, 09:16
Smile
  #34
Member
 
Join Date: Oct 2012
Posts: 47
Rep Power: 4
sh.d is on a distinguished road
hi
i want to create 2d mesh around airfoil
but when i use checkMesh is this error: ***Max skewness = 5.87721, 2 highly skew faces detected which may impair the quality of the results
<<Writing 2 skew faces to set skewFaces

and the surface of airfoil not snap
is it right:?
1:run blockMesh
2:snappyhexMeshDict -overwite
3:extrudeMesh
Attached Files
File Type: gz checkMesh.tar.gz (1.4 KB, 2 views)
sh.d is offline   Reply With Quote

Old   May 28, 2013, 09:42
Default
  #35
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,571
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Hi SH,

The first error seems to have been resolved. The error you mention is probably related to the settings in snappyHexDict, so I would recommend you to search the forum in the related threads. E.g.:

Code:
http://www.cfd-online.com/Forums/openfoam-meshing-snappyhexmesh/
Kind regards,

Niels
ngj is offline   Reply With Quote

Old   March 8, 2014, 19:37
Default I Need Help
  #36
New Member
 
Join Date: Mar 2014
Posts: 5
Rep Power: 3
Majed is on a distinguished road
Hello all,

I have a question about blockMesh in OpenFOAM. in my geometry there are some faces that are shared between two blocks. How should I define such faces? As far as I know, we can not duplicate the vertices in blockMesh. On the other hand, when the shared face is defined in one of the blocks, the user receives a message as "trying to identify a boundary patch to the..."

Tnx for your help!
Majed 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
C type mesh ivan_cozza OpenFOAM Native Meshers: blockMesh 13 November 28, 2008 05:38
Empty cells in mesh Nikolaos FLOW-3D 2 October 21, 2008 23:17
Moving mesh forces on patches and turbulence solver jackdaniels83 OpenFOAM Running, Solving & CFD 3 May 31, 2007 10:29
First steps w moving mesh FOAM FATAL ERROR solver table is empty tehache OpenFOAM Running, Solving & CFD 2 May 14, 2007 04:59
Mesh Type rakib FLUENT 0 September 17, 2000 07:28


All times are GMT -4. The time now is 13:21.