CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   This mesh contains patches of type empty but is not 1D or 2D (https://www.cfd-online.com/Forums/openfoam-solving/60059-mesh-contains-patches-type-empty-but-not-1d-2d.html)

 oric August 22, 2006 09:46

Hi, I tried to remove a wa

Hi,

I tried to remove a wall from the cavity case (tutorial/icoFoam/cavity) so I changed the blockMeshDict by moving a patch from fixedWall to frontAndBack in the boundary conditions :

wall fixedWalls
(
(2 6 5 1)
(1 5 4 0)
)
empty frontAndBack
(
(0 4 7 3)
(0 3 2 1)
(4 5 6 7)
)

Then I run blockMesh without problem but when I run icoFoam I get :

--> FOAM FATAL ERROR : 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 agree, the mesh is not 1D or 2D, but the cavity example neither and it works with "empty" patches !

What should I do ? My goal is to run a NS simulation in a open space over a ground with obstacles.

TIA

Olivier.

 mattijs August 23, 2006 03:57

empty patches are not included

empty patches are not included in any calculation. They are really only useful for front and back of a pure 2D simulation. This also means your domain should be only one celllayer thick (since otherwise you'd still have internal faces in the cross direction)

The cavity tutorial is a 2D simulation (no cross flow, no gradients in cross direction apart from truncation errors)

 oric August 23, 2006 08:17

ok, so I used patch in

ok, so I used

patch in
(
(0 4 7 3)
)
patch out
(
(2 6 5 1)
)

and the right B.C. in 0/p and 0/U and it is ok.

Thanks,

Olivier.

 mahaputra May 15, 2009 20:21

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

Dear All

since I am a beginner, i try to make a 2D mesh by manual n blockMesh

like shown below :

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1e-3;

vertices
(
(250 0 0)
(300 0 0)
(250 100 0)
(300 100 0)

(100 100 0)
(250 100 0)
(300 100 0)

(0 175 0)
(100 175 0)
(100 175 0)
(250 175 0)
(300 175 0)

(0 225 0)
(100 225 0)
(100 225 0)
(250 225 0)
(300 225 0)

(100 550 0)
(250 550 0)
(300 550 0)
(300 550 0)
(400 550 0)

(100 600 0)
(250 600 0)
(300 600 0)
(300 600 0)
(400 600 0)

(250 0 1)
(300 0 1)
(250 100 1)
(300 100 1)

(100 100 1)
(250 100 1)
(300 100 1)

(0 175 1)
(100 175 1)
(100 175 1)
(250 175 1)
(300 175 1)

(0 225 1)
(100 225 1)
(100 225 1)
(250 225 1)
(300 225 1)

(100 550 1)
(250 550 1)
(300 550 1)
(300 550 1)
(400 550 1)

(100 600 1)
(250 600 1)
(300 600 1)
(300 600 1)
(400 600 1)
);

blocks
(
hex (0 1 3 2 27 28 30 29) (10 20 1) simpleGrading (1 1 1)
hex (4 5 10 9 31 32 37 36) (30 15 1) simpleGrading (1 1 1)
hex (5 6 11 10 32 33 38 37) (10 15 1) simpleGrading (1 1 1)
hex (7 8 13 12 34 35 40 39) (20 10 1) simpleGrading (1 1 1)
hex (9 10 15 14 36 37 42 41) (30 10 1) simpleGrading (1 1 1)
hex (10 11 16 15 37 38 43 42) (10 10 1) simpleGrading (1 1 1)
hex (14 15 18 17 41 42 45 44) (30 65 1) simpleGrading (1 1 1)
hex (15 16 19 18 42 43 46 45) (10 65 1) simpleGrading (1 1 1)
hex (17 18 23 22 44 45 50 49) (30 10 1) simpleGrading (1 1 1)
hex (18 19 24 23 45 46 51 50) (10 10 1) simpleGrading (1 1 1)
hex (20 21 26 25 47 48 53 52) (20 10 1) simpleGrading (1 1 1)
);

edges
(
);

patches
(
wall walls
(
(0 2 29 27)
(1 3 30 28)
(4 5 32 31)
(4 9 36 31)
(6 11 38 33)
(7 8 35 34)
(11 16 43 38)
(12 13 40 39)
(14 17 44 41)
(16 19 46 43)
(17 22 49 44)
(20 21 48 47)
(22 23 50 49)
(23 24 51 50)
(25 26 53 52)
)
patch inlet
(
(7 12 39 34)
)
patch outletBottom
(
(0 1 28 27)
)
patch outletTop
(
(21 26 53 48)
)

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

(27 28 30 29)
(31 32 37 36)
(32 33 38 37)
(36 37 42 41)
(37 38 43 42)
(41 42 45 44)
(42 43 46 45)
(44 45 50 49)
(45 46 51 50)
(34 35 40 39)
(47 48 53 52)
)

);

mergePatchPairs
(
);

// ************************************************** *********************** //

i run checkMesh, and it said :

Mesh OK.

but, i got this following error message when tried to run my case (im using dieselFoam) :

Creating field DpDt

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

anybody can help me please

really really need help :(

many thanks

 ngj May 16, 2009 05:42

Hi Nugroho

I do not know if it is the source of all your problems, however you have multiple defined points, e.g.:

(300 100 0)

(100 100 0)
(250 100 0)
(300 100 0)

and if you do not use the same points to define two blocks with common boundary, it will not automatically be merged. Remove all duplicate points and try again. By the way, the blockMesh do tell you that something is wrong by:

Default patch type set to empty
--> FOAM Warning :
From function polyMesh::polyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 576
Found 6 undefined faces in mesh; adding to default patch.

This is a valuable warning, because you have manually made the front and back patches.

Good luck,

Niels

 mahaputra May 16, 2009 06:09

Quote:
 Originally Posted by ngj (Post 216350) Hi Nugroho I do not know if it is the source of all your problems, however you have multiple defined points, e.g.: (300 100 0) (100 100 0) (250 100 0) (300 100 0) and if you do not use the same points to define two blocks with common boundary, it will not automatically be merged. Remove all duplicate points and try again. By the way, the blockMesh do tell you that something is wrong by: Default patch type set to empty --> FOAM Warning : From function polyMesh::polyMesh(... construct from shapes...) in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 576 Found 6 undefined faces in mesh; adding to default patch. This is a valuable warning, because you have manually made the front and back patches. Good luck, Niels
Ok

i will remove the duplicate point

but, what do you mean with ''I have multiple defined points'' ? i still didnt understand :(

Thanks Niels :)

 ngj May 16, 2009 06:56

The point (300 100 0) is among others defined in the vertices-list more than once.

 mahaputra May 16, 2009 08:22

Quote:
 Originally Posted by ngj (Post 216356) The point (300 100 0) is among others defined in the vertices-list more than once.
Dear Niels

i have removed the duplicate points

like shown below :

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1e-3;

vertices
(
(250 0 0) //0
(300 0 0) //1
(300 100 0) //2
(250 100 0) //3

(100 100 0) //4
(0 175 0) //5
(100 175 0) //6
(250 175 0) //7
(300 175 0) //8
(300 225 0) //9
(250 225 0) //10
(100 225 0) //11
(0 225 0) //12
(100 550 0) //13
(250 550 0) //14
(300 550 0) //15
(400 550 0) //16
(400 600 0) //17
(300 600 0) //18
(250 600 0) //19
(100 600 0) //20

(250 0 1) //21
(300 0 1) //22
(300 100 1) //23
(250 100 1) //24

(100 100 1) //25
(0 175 1) //26
(100 175 1) //27
(250 175 1) //28
(300 175 1) //29
(300 225 1) //30
(250 225 1) //31
(100 225 1) //32
(0 225 1) //33
(100 550 1) //34
(250 550 1) //35
(300 550 1) //36
(400 550 1) //37
(400 600 1) //38
(300 600 1) //39
(250 600 1) //40
(100 600 1) //41

);

blocks
(
hex (0 1 3 2 21 22 23 24) (10 20 1) simpleGrading (1 1 1)
hex (4 3 7 6 25 24 28 27) (30 15 1) simpleGrading (1 1 1)
hex (3 2 8 7 24 23 29 28) (10 15 1) simpleGrading (1 1 1)
hex (5 6 11 12 26 27 32 33) (20 10 1) simpleGrading (1 1 1)
hex (6 7 10 11 27 28 31 32) (30 10 1) simpleGrading (1 1 1)
hex (7 8 9 10 28 29 30 31) (10 10 1) simpleGrading (1 1 1)
hex (11 10 14 13 32 31 35 34) (30 65 1) simpleGrading (1 1 1)
hex (10 9 15 14 31 30 36 35) (10 65 1) simpleGrading (1 1 1)
hex (13 14 19 20 34 35 40 41) (30 10 1) simpleGrading (1 1 1)
hex (14 15 18 19 35 36 39 40) (10 10 1) simpleGrading (1 1 1)
hex (15 16 17 18 36 37 38 39) (20 10 1) simpleGrading (1 1 1)
);

edges
(
);

patches
(
wall walls
(
(0 3 24 21)
(1 2 23 22)
(4 3 24 25)
(4 6 27 25)
(2 8 29 23)
(5 6 27 26)
(8 9 30 29)
(12 11 32 33)
(11 13 34 32)
(9 15 36 30)
(13 20 41 34)
(15 16 37 36)
(20 19 40 41)
(19 18 39 40)
(18 17 38 39)
)
patch inlet
(
(5 12 33 26)
)
patch outletBottom
(
(0 1 22 21)
)
patch outletTop
(
(16 17 38 37)
)

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

(21 22 23 24)
(25 24 28 27)
(24 23 29 28)
(27 28 31 32)
(28 29 30 31)
(32 31 35 34)
(31 30 36 35)
(34 35 40 41)
(35 36 39 40)
(26 27 32 33)
(36 37 38 39)
)

);

mergePatchPairs
(
);

// ************************************************** *********************** //

but i got this error message when i tried run blockMesh :

face 0 in patch 0 does not have neighbour cell face: 4(0 3 24 21)#0 Foam::error::printStack(Foam::Ostream&) in "/home/user/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/user/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::Ostream& Foam::operator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/home/user/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/blockMesh"
#3 Foam::polyMesh::facePatchFaceCells(Foam::List<Foam ::face> const&, Foam::List<Foam::List<int> > const&, Foam::List<Foam::List<Foam::face> > const&, int) const in "/home/user/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 Foam::polyMesh::polyMesh(Foam::IOobject const&, Foam::Field<Foam::Vector<double> > const&, Foam::List<Foam::cellShape> const&, Foam::List<Foam::List<Foam::face> > const&, Foam::List<Foam::word> const&, Foam::List<Foam::word> const&, Foam::word const&, Foam::word const&, Foam::List<Foam::word> const&, bool) in "/home/user/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#5 Foam::blockMesh::createTopology(Foam::IOdictionary &) in "/home/user/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/blockMesh"
#6 Foam::blockMesh::blockMesh(Foam::IOdictionary&) in "/home/user/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/blockMesh"
#7 main in "/home/user/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/blockMesh"
#8 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#9 __gxx_personality_v0 in "/home/user/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/blockMesh"

From function polyMesh::facePatchFaceCells(const faceList& patchFaces,const labelListList& pointCells,const faceListList& cellsFaceShapes,const label patchID)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 125.

FOAM aborting

Aborted

i dont understand why this error message came? since i checked, for the face 0 in patch 0 (wall) it has neighbour cell .

so why this error came ? :(

 ngj May 16, 2009 09:45

The block

hex (0 1 3 2 21 22 23 24) (10 20 1) simpleGrading (1 1 1)

is ill-defined. I suppose it needs to be:

hex (0 1 2 3 21 22 23 24) (10 20 1) simpleGrading (1 1 1)

Best regards,

Niels

 mahaputra May 16, 2009 09:52

oh my God!

i didnt see it. Thanks Niels.

now my simulation is running :D

 hamsadhwani8 July 10, 2009 14:52

Hello,

I am trying to run a 3D case in interFoam. I am able to run a case with just 1 cell in the z-direction. However, when I try to increase the number of cells in this direction i get the following error while running the interfoam case. There is no problem with the mesh as checkMesh indicates. Can someone comment on this please? Below is the error i get at execution, followed by my blockMesh file. Thanks

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

Create mesh for time = 0

--> FOAM Warning :
From function Field<Type>::Field(const word& keyword, const dictionary& dict, const label s)
in file /Network/Servers/controller.cluster/Homedir/stsriniv/OpenFOAM/OpenFOAM-1.5/src/OpenFOAM/lnInclude/Field.C at line 252
Reading "/Homedir/stsriniv/OpenFOAM/stsriniv-1.5/run/tutorials/interFoam/dropletShear_inletU/0/pd::outlet" from line 34 to line 35
expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Calculating field g.h

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

-------------------------

My blockMesh file is:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1.0;//0.01; //0.146;

vertices
(
(-5.0 -1.5 -2.5)
(5.0 -1.5 -2.5)
(5.0 0 -2.5)
(-5.0 0 -2.5)
(5.0 1.5 -2.5)
(-5.0 1.5 -2.5)
(-5.0 -1.5 2.5)
(5.0 -1.5 2.5)
(5.0 0 2.5)
(-5.0 0 2.5)
(5.0 1.5 2.5)
(-5.0 1.5 2.5)
);

blocks
(
hex (0 1 2 3 6 7 8 9) (200 30 4) simpleGrading (1 1 1)
hex (3 2 4 5 9 8 10 11) (200 30 4) simpleGrading (1 1 1)
// hex (0 1 2 3 6 7 8 9) (15 100 1) simpleGrading (1 1 1)
// hex (3 2 4 5 9 8 10 11) (15 100 1) simpleGrading (1 1 1)
// hex (5 4 6 7 15 14 16 17) (15 100 1) simpleGrading (1 1 1)
// hex (7 6 8 9 17 16 18 19) (35 100 1) simpleGrading (1 1 1)
);

edges
(
);
patches
(
patch inlet1
(
(1 2 8 7)
)
patch inlet2
(
(3 5 11 9)
)
patch outlet
(
(2 4 10 8)
(0 3 9 6)
)
patch movingwall1 //atmosphere
(
(4 5 11 10)
// (0 6 7 1)
)
patch movingwall2 //atmosphere
(
// (4 5 11 10)
(0 6 7 1)
)
);

mergePatchPairs
(
);

// ************************************************** *********************** //

 ngj July 10, 2009 15:54

Quote:
 Originally Posted by hamsadhwani8 (Post 222308) 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. //
The above is the answer you seek.

Best regards

Miels

 hamsadhwani8 July 10, 2009 16:11

Hi Niels,

Thanks for the quick reply. However, I did not understand that error. All the patches are either inlets/outlets or walls. What is this empty patch? Is it referring to the the front and back surfaces? I have used the exact same blockMesh file for a 2D case by simply changing the block thickness in the z direction and setting the number of cells to 1. If you could throw more light on this.

Thanks,
S

 ngj July 13, 2009 03:39

Hi Sechasai

The only thing I can come up with, is that sometimes I have experienced that the constant/polyMesh/boundary file is not updated.
Try deleting it and re-blockMesh, then it should be the correct file, and hopefully it will solve your problem.

Best regards,

Niels

 bobby August 4, 2009 15:16

Hi,
I have the same problem. I am trying to simulate the rising of bubble on a plate.
I already used InterFoam (with the same mesh and without errors) but I need to compare my results using InterDyMFoam.

The same message as above appears :

Selected 176 cells for refinement out of 146800.
Refined from 146800 to 148032 cells.
Selected 0 split points out of a possible 176.
Execution time for mesh.update() = 2.96 s

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

Here, is my blockMeshDict,

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.4 |
| \\ / A nd | Web: http://www.openfoam.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
root "";
case "";
instance "";
local "";
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;
vertices
(
(0 0 0)
(0.004 0 0)
(0.070 0 0)
(0.08 0 0)
(0 0 0.013)
(0.004 0 0.013)
(0.070 0 0.013)
(0.08 0 0.013)
(0 0 0.015)
(0.004 0 0.015)
(0.070 0 0.015)
(0.08 0 0.015)
(0 0 0.02)
(0.004 0 0.02)
(0.070 0 0.02)
(0.08 0 0.02)
(0 0.02 0)
(0.004 0.02 0)
(0.070 0.02 0)
(0.08 0.02 0)
(0 0.02 0.013)
(0.004 0.02 0.013)
(0.070 0.02 0.013)
(0.08 0.02 0.013)
(0 0.02 0.015)
(0.004 0.02 0.015)
(0.070 0.02 0.015)
(0.08 0.02 0.015)
(0 0.02 0.02)
(0.004 0.02 0.02)
(0.070 0.02 0.02)
(0.08 0.02 0.02)
);
blocks
(
hex (0 1 17 16 4 5 21 20) (40 1 130) simpleGrading (1 1 1)
hex (1 2 18 17 5 6 22 21) (660 1 130) simpleGrading (1 1 1)
hex (2 3 19 18 6 7 23 22) (100 1 130) simpleGrading (1 1 1)
hex (4 5 21 20 8 9 25 24) (40 1 20) simpleGrading (1 1 1)
hex (6 7 23 22 10 11 27 26) (100 1 20) simpleGrading (1 1 1)
hex (8 9 25 24 12 13 29 28) (40 1 50) simpleGrading (1 1 1)
hex (9 10 26 25 13 14 30 29) (660 1 50) simpleGrading (1 1 1)
hex (10 11 27 26 14 15 31 30) (100 1 50) simpleGrading (1 1 1)
);
edges
(
);
patches
(
wall tankWall
(
(0 16 17 1)
(1 17 18 2)
(2 18 19 3)
(0 4 20 16)
(4 8 24 20)
(8 12 28 24)
(12 13 29 28)
(13 14 30 29)
(14 15 31 30)
)
patch inout
(
(15 11 27 31)
(11 7 23 27)
(7 3 19 23)
)
wall heatedPlate
(
(5 6 22 21)
)
(
(9 5 21 25)
(9 25 26 10)
(10 26 22 6)
)
empty backAndFront
(
(0 1 5 4)
(4 5 9 8)
(8 9 13 12)
(1 2 6 5)
(9 10 14 13)
(2 3 7 6)
(6 7 11 10)
(10 11 15 14)
(16 17 21 20)
(20 21 25 24)
(24 25 29 28)
(17 18 22 21)
(25 26 30 29)
(18 19 23 22)
(22 23 27 26)
(26 27 31 30)
)
);
mergePatchPairs
(
);
// ************************************************** *********************** //

Can someone help me please?

Best Regards

 sandy August 6, 2009 08:13

Hi guys, when I import my gambit .neu file into OpenFOAM, I check the mesh is OK. However, after I change the frontandback into empty (2D mesh) and check the mesh again, I get error message as follow:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : checkMesh
Date : Aug 07 2009
Time : 01:55:47
Host : localhost.localdomain
PID : 5190
Case : /root/OpenFOAM/root-1.5/run/tutorials/LesInterPhaseChangeFoam/Hydrofoil/Sixdegree
nProcs : 1

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

Create polyMesh for time = constant

Time = constant

Mesh stats
points: 91414
internal points: 0
faces: 181229
internal faces: 89815
cells: 45174
boundary patches: 6
point zones: 0
face zones: 0
cell zones: 0

Number of cells of each type:
hexahedra: 45174
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
inlet 103 208 ok (non-closed singly connected)
outlet 158 318 ok (non-closed singly connected)
up 237 476 ok (non-closed singly connected)
down 236 474 ok (non-closed singly connected)
frontandback 90348 91414 ok (non-closed singly connected)
foil 332 664 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-10 -10 0) (30 10 0.007)
Mesh (non-empty) directions (1 1 0)
Mesh (non-empty, non-wedge) dimensions 2
***Number of edges not aligned with or perpendicular to non-empty directions: 38113
<<Writing 76226 points on non-aligned edges to set nonAlignedEdges
Boundary openness (-8.9509e-24 9.15928e-22 -1.31298e-19) OK.
Max cell openness = 2.56232e-16 OK.
Max aspect ratio = 287.879 OK.
Minumum face area = 2.19292e-05. Maximum face area = 0.452831. Face area magnitudes OK.
Min volume = 2.41268e-07. Max volume = 0.00316982. Total volume = 5.29651. Cell volumes OK.
Mesh non-orthogonality Max: 39.8412 average: 5.87407
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.763965 OK.

Failed 1 mesh checks.

End
==============================

What's wrong with it? Could somebody help me out? Thanks a lot.

 sandy August 10, 2009 04:29

Maybe I should try to get the mesh by the great Tool snappyHexMesh?

 hansel August 14, 2009 01:49

Comment deleted

 tgj December 8, 2009 13:15

hi,

as a beginner in OpenFOAM, i'm trying to run a 2D "virtual wind tunnel" with a square shaped obstacle using simplefoam. This is my BlockMeshDict:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.05;

vertices
(
(0 0 0)
(20 0 0)
(20 5 0)
(0 5 0)
(0 0 0.1)
(20 0 0.1) //Z5
(20 5 0.1)
(0 5 0.1)
(40 5 0)
(40 10 0)
(20 10 0) //Z10
(40 5 0.1)
(40 10 0.1)
(20 10 0.1)
(20 -5 0)
(40 -5 0) //Z15
(40 0 0)
(20 -5 0.1)
(40 -5 0.1)
(40 0 0.1)
(27 1 0) //Z20
(32 1 0)
(32 4 0)
(27 4 0)
(27 1 0.1)
(32 1 0.1) //Z25
(32 4 0.1)
(27 4 0.1)
(27 0 0)
(32 0 0)
(32 0 0.1) //Z30
(27 0 0.1)
(27 5 0)
(32 5 0)
(32 5 0.1)
(27 5 0.1) //Z35
(20 1 0)
(20 4 0)
(20 4 0.1)
(20 1 0.1)
(40 1 0) //Z40
(40 4 0)
(40 4 0.1)
(40 1 0.1)
);

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

hex (1 28 20 36 5 31 24 39) (7 1 1) simpleGrading (1 1 1)
hex (29 16 40 21 30 19 43 25) (8 1 1) simpleGrading (1 1 1)
hex (36 20 23 37 39 24 27 38) (7 3 1) simpleGrading (1 1 1)
hex (21 40 41 22 25 43 42 26) (8 3 1) simpleGrading (1 1 1)
hex (37 23 32 2 38 27 35 6) (7 1 1) simpleGrading (1 1 1)
hex (22 41 8 33 26 42 11 34) (8 1 1) simpleGrading (1 1 1)

hex (28 29 21 20 31 30 25 24) (5 1 1) simpleGrading (1 1 1)
hex (23 22 33 32 27 26 34 35) (5 1 1) simpleGrading (1 1 1)
);

edges
(
);

patches
(
patch inlet
(
(0 3 7 4)
)

patch outlet
(
(16 40 43 19)
(40 41 42 43)
(41 8 11 42)
)

wall walls
(
(0 1 5 4)
(3 7 6 2)
(2 10 13 6)
(10 9 12 13)
(8 9 12 11)
(15 16 19 18)
(14 15 18 17)
(14 1 5 17)

(20 21 25 24)
(23 22 26 27)
(20 24 27 23)
(21 22 26 25)
)

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

(1 28 20 36)
(5 31 24 39)
(29 16 40 21)
(30 19 43 25)
(28 29 21 20)
(31 30 25 24)
(23 22 33 32)
(27 26 34 35)
(36 20 23 37)
(39 24 27 38)
(21 40 41 22)
(25 43 42 26)
(37 23 32 2)
(38 27 35 6)
(22 41 8 33)
(26 42 11 34)
)
);

mergePatchPairs
(
);

// ************************************************** *********************** //

blockmesh works but displays the warning:
Default patch type set to empty
--> FOAM Warning :
From function polyMesh::polyMesh(... construct from shapes...)
in file C:\tmp\OpenFOAM-1.5\src\OpenFOAM\meshes\polyMesh\polyMeshFromShape Mesh.C at line 576
Found 12 undefined faces in mesh; adding to default patch.

when i try to run simplefoam, i get:

Programme terminated with errors: exit code 1, status 0.
Error messages:

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 C:\tmp\OpenFOAM-1.5\src\finiteVolume\fields\fvPatchFields\constrai nt\empty\/emptyFvPatchField.C at line 148.

FOAM exiting

i really don't know where those undefined patches are. Any help would be appreciated ;)

 hansel December 8, 2009 16:21

When I make my meshes, I always changed the undefined type from empty to patch. For some reason a default empty patch causes me problems too.

All times are GMT -4. The time now is 18:36.