CFD Online URL
[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   August 22, 2006, 10:46
Default Hi, I tried to remove a wa
  #1
oric
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   August 23, 2006, 04:57
Default empty patches are not included
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
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)
mattijs is offline   Reply With Quote

Old   August 23, 2006, 09:17
Default ok, so I used patch in
  #3
oric
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   May 15, 2009, 21:21
Default This mesh contains patches of type empty but is not 1D or 2D
  #4
Member
 
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 7
mahaputra is on a distinguished road
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
mahaputra is offline   Reply With Quote

Old   May 16, 2009, 06:42
Default
  #5
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,553
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
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:olyMesh(... 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
ngj is online now   Reply With Quote

Old   May 16, 2009, 07:09
Default
  #6
Member
 
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 7
mahaputra is on a distinguished road
Quote:
Originally Posted by ngj View Post
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:olyMesh(... 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
mahaputra is offline   Reply With Quote

Old   May 16, 2009, 07:56
Default
  #7
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,553
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
The point (300 100 0) is among others defined in the vertices-list more than once.
ngj is online now   Reply With Quote

Old   May 16, 2009, 09:22
Default
  #8
Member
 
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 7
mahaputra is on a distinguished road
Quote:
Originally Posted by ngj View Post
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:rintStack(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:perator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/home/user/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/blockMesh"
#3 Foam:olyMesh::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:olyMesh:olyMesh(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 ?
mahaputra is offline   Reply With Quote

Old   May 16, 2009, 10:45
Default
  #9
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,553
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
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
ngj is online now   Reply With Quote

Old   May 16, 2009, 10:52
Default
  #10
Member
 
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 7
mahaputra is on a distinguished road
oh my God!

i didnt see it. Thanks Niels.

now my simulation is running
mahaputra is offline   Reply With Quote

Old   July 10, 2009, 15:52
Default
  #11
New Member
 
sesha
Join Date: Mar 2009
Posts: 23
Rep Power: 7
hamsadhwani8 is on a distinguished road
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


Reading environmentalProperties
Reading field pd

--> 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:utlet" from line 34 to line 35
expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.
Reading field gamma

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

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
(
);

// ************************************************** *********************** //
hamsadhwani8 is offline   Reply With Quote

Old   July 10, 2009, 16:54
Default
  #12
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,553
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
Quote:
Originally Posted by hamsadhwani8 View Post
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
ngj is online now   Reply With Quote

Old   July 10, 2009, 17:11
Default
  #13
New Member
 
sesha
Join Date: Mar 2009
Posts: 23
Rep Power: 7
hamsadhwani8 is on a distinguished road
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
hamsadhwani8 is offline   Reply With Quote

Old   July 13, 2009, 04:39
Default
  #14
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,553
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
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
ngj is online now   Reply With Quote

Old   August 4, 2009, 16:16
Default
  #15
New Member
 
anthony
Join Date: Jul 2009
Posts: 1
Rep Power: 0
bobby is on a distinguished road
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)
)
wall adiaPlate
(
(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
bobby is offline   Reply With Quote

Old   August 6, 2009, 09:13
Default
  #16
Senior Member
 
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 8
sandy is on a distinguished road
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 is offline   Reply With Quote

Old   August 10, 2009, 05:29
Default
  #17
Senior Member
 
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 8
sandy is on a distinguished road
Maybe I should try to get the mesh by the great Tool snappyHexMesh?
sandy is offline   Reply With Quote

Old   August 14, 2009, 02:49
Default
  #18
Senior Member
 
Steve Hansel
Join Date: Jun 2009
Location: Colorado, USA
Posts: 112
Rep Power: 7
hansel is on a distinguished road
Comment deleted
hansel is offline   Reply With Quote

Old   December 8, 2009, 13:15
Default
  #19
tgj
New Member
 
Join Date: Dec 2009
Posts: 3
Rep Power: 7
tgj is on a distinguished road
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:olyMesh(... 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

Last edited by tgj; December 8, 2009 at 13:18. Reason: correcting errors
tgj is offline   Reply With Quote

Old   December 8, 2009, 16:21
Default
  #20
Senior Member
 
Steve Hansel
Join Date: Jun 2009
Location: Colorado, USA
Posts: 112
Rep Power: 7
hansel is on a distinguished road
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.
hansel 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 22, 2008 00:17
Moving mesh forces on patches and turbulence solver jackdaniels83 OpenFOAM Running, Solving & CFD 3 May 31, 2007 11:29
First steps w moving mesh FOAM FATAL ERROR solver table is empty tehache OpenFOAM Running, Solving & CFD 2 May 14, 2007 05:59
Mesh Type rakib FLUENT 0 September 17, 2000 08:28


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