[derath]

Hi to all
Which means this error of blockMesh?
> FOAM FATAL ERROR : Inconsistent number of faces between block pair 2 and 4

From function blockMesh::blockMesh(IOdictionary& meshDescription)
in file createMergeList.C at line 202.

FOAM exiting
Someone can help me?
Thanks in advantage
Giuseppe

[hjasak]

It means you've got 2 blocks you are trying to connect to each other in blockMesh but they haven't got the matching number of cells in this direction or that the scaling is different.

Hrv

[Turbulence]

Hi all,
I tried to manipulate the blockMeshDict, but I am not able to get rid of this problem.
"inconsistent number of faces between block pairs 0 and 1"
Can anyone help?

blockMeshDict:

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(

(-1 39.8 -0.5)
(81 39.8 -0.5)
(-1 40.2 -0.5)
(81 40.2 -0.5)
(-1 39.8 1)
(-1 39.8 52)
(81 39.8 52)
(81 39.8 1)
(-1 40.2 1)
(-1 40.2 52)
(81 40.2 52)
(81 40.2 1)
(-1 81.2 1)
(-1 81.2 52)
(81 81.2 52)
(81 81.2 1)
(-1 -1.2 1)
(-1 -1.2 52)
(81 -1.2 52)
(81 -1.2 1)
);

blocks
(
hex (0 4 7 1 2 8 11 3) (410 2 5) simpleGrading (1 1 1)

hex (4 5 6 7 8 9 10 11) (410 2 170) simpleGrading (1 1 1)

hex (8 9 10 11 12 13 14 15) (410 205 170) simpleGrading (1 1 1)

hex (16 17 18 19 4 5 6 7) (410 205 170) simpleGrading (1 1 1)

);

boundary
(
bPlane
{
type patch;
faces
(
(0 4 7 1)
);
}
tPlane
{
type patch;
faces
(
(2 3 11 8)
);
}
fPlane
{
type patch;
faces
(
(0 2 8 4)
);
}

backPlane
{
type patch;
faces
(
(1 7 11 3)
);
}

lPlane
{
type patch;
faces
(
(0 1 3 2)
);
}


FPlane
{
type patch;
faces
(
(4 8 9 5)
(8 12 13 9)
(16 4 5 17)
);
}

BackPlane
{
type patch;
faces
(
(7 6 10 11)
(10 14 15 11)
(19 18 6 7)
);
}


LuPlane
{
type patch;
faces
(
(8 11 15 12)
);
}

LbPlane
{
type patch;
faces
(
(16 19 7 4)
);
}

RPlane
{
type patch;
faces
(
(5 6 10 9)
(9 10 14 13)
(17 18 6 5)
);
}

TuPlane
{
type patch;
faces
(
(12 15 14 13)
);
}


blPlane

{

type patch;
faces

(
(16 17 18 19)
);

}

);

................

Thank You

[Rider]

Could you post a drawing ? (about the geometry that you want to create with blockMesh)

[Turbulence]

PFA the image.Will this do?

[Rider]

Ok, this is the geometry that I had deduced with the points

The problem is in the syntax of blocks. The correct syntax is :

hex (0 1 3 2 4 7 11 8) 

hex (4 7 11 8 5 6 10 9) 

hex (16 19 7 4 17 18 6 5) 

hex (8 11 15 12 9 10 14 13)

[Turbulence]

Hi Rider,
Thank you very much
Could you explain me how to number,so that I wont make this mistake again..

Thank You
Turbulence.

[Rider]

Hi Turbulence,

You will find the explanation of the rule to use (with illustration) on the following link:

http://www.openfoam.org/docs/user/blockMesh.php



Rider.

[Turbulence]

Thank you very much Rider

[Rider]

Your welcome

[Samsam2]

I have same problem and dont know what is wrong with my mesh. I get error of "Inconsistent number of faces between block pair 0 and 1". Here is copy of my blockmesh dict:
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}

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

scale 1;

vertices
(
(-296 -296.6 -5000)
(-296 -296.6 2192)
(-296 -296.6 2792)
(-296 -296.6 2992)
(-296 296.6 2992)
(-296 296.6 2792)
(-296 396.6 2792)
(-296 396.6 2192)
(-296 296.6 2192)
(-296 296.6 -5000)
(296 -296.6 -5000)
(296 -296.6 2192)
(296 -296.6 2792)
(296 -296.6 2992)
(296 296.6 2992)
(296 296.6 2792)
(296 396.6 2792)
(296 396.6 2192)
(296 296.6 2192)
(296 296.6 -5000)

);
blocks
(
hex (0 9 8 1 10 19 18 11) (16 16 194) simpleGrading (1 1 1)
hex (1 8 5 2 11 18 15 12) (16 16 22) simpleGrading (1 1 1)
hex (2 5 4 3 12 15 14 13) (16 16 5) simpleGrading (1 1 1)
hex (8 7 6 5 18 17 16 15) (16 2 22) simpleGrading (1 1 1)
);

edges
(
);

boundary
(
frontAndBack
{
type wall;
faces
(
(10 11 18 19)
(11 12 15 18)
(12 13 14 15)
(18 15 16 17)
(9 8 1 0)
(8 5 2 1)
(5 4 3 2)
(7 6 5 8)
);
}
walls
{
type wall;
faces
(
(0 1 11 10)
(1 2 12 11)
(2 3 13 12)
(15 14 4 5)
(16 15 5 6)
(18 17 7 8)
(19 18 8 9)
);
}
outlet
{
type patch;
faces
(
(0 10 19 9)
);
}
inletone
{
type patch;
faces
(
(3 13 14 4)
);
}
inlettwo
{
type patch;
faces
(
(17 16 6 7)
);
}
);

Could you please help me how to solve this problem?
Thanks alot!

[gpouliasis]

I am reviving this thread, since i found a problem that is not listed here. It could help somebody.

This errror can appear also if the number of specified cell in the same direction is different. In example:
(50 10 1)
(50 20 1)

It is logical, but still i made it wrong the first time

[pradeep_m]

Creating block offsets
Creating merge list

--> FOAM FATAL ERROR:
Inconsistent number of faces between block pair 0 and 1

From function void Foam::blockMesh::calcMergeInfo()
in file blockMesh/blockMeshMerge.C at line 222.

FOAM exiting


blockMesh file

convertToMeters 1;

vertices
(
(0 0 -0.01) //0
(0.1 0 -0.01) //1
(0.234 0.02127 -0.01) //2
(0.279 0.308 -0.01) //3
(0.659 0.308 -0.01) //4
(0.8545 0 -0.01) //5
(0 0.321 -0.01) //6
(0.1 0.321 -0.01) //7
(0.234 0.321 -0.01) //8
(0.279 0.321 -0.01) //9
(0.659 0.321 -0.01) //10
(0.8545 0.321 -0.01) //11
(0 0 0.01) //12
(0.1 0 0.01) //13
(0.234 0.02127 0.01) //14
(0.279 0.308 0.01) //15
(0.659 0.308 0.01) //16
(0.8545 0 0.01) //17
(0 0.321 0.01) //18
(0.1 0.321 0.01) //19
(0.234 0.321 0.01) //20
(0.279 0.321 0.01) //21
(0.659 0.321 0.01) //22
(0.8545 0.321 0.01) //23


);

blocks
(
hex (0 1 7 6 12 13 19 18) (110 110 1) simpleGrading (1 1 1)
hex (1 2 8 7 13 14 20 19) (110 456 1) simpleGrading (1 1 1)
hex (2 3 9 8 14 15 21 20) (110 300 1) simpleGrading (1 1 1)
hex (3 4 10 9 15 16 22 21) (110 1454 1) simpleGrading (1 1 1)
hex (4 5 11 10 16 17 23 22) (110 718 1) simpleGrading (1 1 1)
);

edges
(
);

boundary
(
inlet
{
type patch;
faces
(
(0 12 18 6)
);
}
outlet
{
type patch;
faces
(
(5 11 23 17)
);
}
bottom
{
type symmetryPlane;
faces
(
(0 1 13 12)
);
}
top
{
type patch;
faces
(
(6 18 19 7)
(7 19 20 8)
(8 20 21 9)
(9 21 22 10)
(10 22 23 11)
);
}
obstacle
{
type wall;
faces
(
(1 2 14 13)
(2 3 15 14)
(3 4 16 15)
(4 5 17 16)
);
}
);

mergePatchPairs
(
);


can anyone please address my problem?

[pradeep_m]

geometry attached here

[Drew.M]

I know this is old but, the link is no longer working. Is there an updated link @rider???

Thanks!

[AtoHM]

https://www.openfoam.com/documentati...ckmesh-utility