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

FATAL ERROR: face 6 in patch 2 does not have neighbour cell face: 4(8 9 21 20)

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

Like Tree1Likes
  • 1 Post By AlanR

Reply
 
LinkBack Thread Tools Display Modes
Old   January 18, 2010, 14:59
Default FATAL ERROR: face 6 in patch 2 does not have neighbour cell face: 4(8 9 21 20)
  #1
Member
 
Robin Gilbert
Join Date: Jan 2010
Posts: 66
Rep Power: 6
robingilbert is on a distinguished road
Hello I was trying to make an I-shaped room and i got the following error:
FATAL ERROR: face 6 in patch 2 does not have neighbour cell face: 4(8 9 21 20)

This is how my blockMeshDict looks like:
convertToMeters 1;

vertices
(
(0 0 0)
(3 0 0)
(3 1 0)
(2 1 0)
(2 2 0)
(3 2 0)
(3 3 0)
(0 3 0)
(0 2 0)
(1 2 0)
(1 1 0)
(0 1 0)
(0 0 1)
(3 0 1)
(3 1 1)
(2 1 1)
(2 2 1)
(3 2 1)
(3 3 1)
(0 3 1)
(0 2 1)
(1 2 1)
(1 1 1)
(0 1 1)
);

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

edges
(
);

patches
(
wall floor
(
(13 1 0 12)
)
wall ceiling
(
(18 6 7 19)
)
wall fixedWalls
(
(6 5 17 18)
(4 3 15 16)
(2 1 13 14)
(7 8 20 19)
(9 10 22 21)
(11 0 12 23)
(8 9 21 20)
(4 5 17 16)
(11 10 22 23)
(3 2 14 15)
)
);

mergePatchPairs
(
(9 4 16 21 8 5 17 20)
(10 3 15 22 11 2 14 23)
);

Please help me....I am new to OpenFOAM as well as C++
robingilbert is offline   Reply With Quote

Old   January 18, 2010, 17:41
Default
  #2
Member
 
Alan Russell
Join Date: Aug 2009
Location: Boise, Idaho USA
Posts: 61
Rep Power: 7
AlanR is on a distinguished road
Robin,

Without going through all of your vertices, blocks, etc., myself, you probably have things in the wrong order. It's very easy to get the order of vertices mixed up in a patch, which will give you fatal errors. First, I would start with one block at a time. I like to number the vertices so that the hex block numbers are consecutive - it's easier to keep track of that way. So you will have 24 vertices and your first block will be hex (0 1 2 3 4 5 6 7) (30 10 10) simpleGrading (1 1 1). Next, try just running blockMesh on one block at a time - blockMesh is very fast, so this will save you debugging time. Once you get all three blocks individually correct, you have problems with mergePatchPairs. Each patch that you want to merge must be individually named. You need something like wall fixedWall1 (6 5 17 18) wall fixedWall2 (4 3 115 16). Then, your mergePatchPairs will look like mergePatchPairs ( (fixedWall2 fixedWall1) (fixedWall3 fixedWall4) etc). Be careful with the order of mergePatchPairs - there is a note in the User Guide about which goes first.
So, break things down, order vertices so the blockMeshDict is easy to debug, and build up your geometry one step at a time. I'm still relatively new at this myself - spending a little time on learning blockMesh is worth the effort. It works quite well once you get used to it. Below is a simple geometry model multiple blocks and merged patch pairs as an example.
Good luck,
Alan

/*--------------------------------*- 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) //a
(2 0 0)
(2 1 0)
(0 1 0)
(0 0 1)
(2 0 1)
(2 1 1)
(0 1 1)
(0 1 0) //b
(2 1 0)
(2 2 0)
(0 2 0)
(0 1 1)
(2 1 1)
(2 2 1)
(0 2 1)
(2 1 0) //c
(3 1 0)
(3 2 0)
(2 2 0)
(2 1 1)
(3 1 1)
(3 2 1)
(2 2 1)
(3 1 0) //d
(5 1 0)
(5 2 0)
(3 2 0)
(3 1 1)
(5 1 1)
(5 2 1)
(3 2 1)
(3 0 0) //e
(5 0 0)
(5 1 0)
(3 1 0)
(3 0 1)
(5 0 1)
(5 1 1)
(3 1 1)

);

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

edges
(
);

patches
(
patch inlet
(
(0 4 7 3)
(8 12 15 11)

)
patch outlet
(
(25 26 30 29)
(33 34 38 37)

)
wall upper
(
(11 15 14 10)
(19 23 22 18)
(27 31 30 26)
)
wall lower
(
(0 1 5 4)
(1 2 6 5)
(16 17 21 20)
(32 33 37 36)
(32 36 39 35)

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

patch i1
(
(3 7 6 2)
)

patch i2
(
(8 9 13 12)
)

patch i3
(
(9 10 14 13)
)

patch i4
(
(16 20 23 19)
)

patch i5
(
(17 18 22 21)
)

patch i6
(
(24 28 31 27)
)

patch i7
(
(24 25 29 28)
)

patch i8
(
(35 39 38 34)
)

);

mergePatchPairs
(
(i2 i1)
(i3 i4)
(i6 i5)
(i7 i8)
);

// ************************************************** *********************** //
Eliz likes this.
AlanR is offline   Reply With Quote

Old   January 18, 2010, 20:10
Default
  #3
Member
 
Robin Gilbert
Join Date: Jan 2010
Posts: 66
Rep Power: 6
robingilbert is on a distinguished road
Hi Alan,

Thanks... I got it running. the error was with the meshpatchpairs.... I dint know that i had to name it!!! thank you.
robingilbert is offline   Reply With Quote

Reply

Tags
fatal error

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
Import netgen mesh to OpenFOAM hsieh Open Source Meshers: Gmsh, Netgen, CGNS, ... 32 September 13, 2011 05:50
BlockMeshmergePatchPairs hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 07:36
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15
Warning 097- AB CD-adapco 6 November 15, 2004 04:41


All times are GMT -4. The time now is 11:23.