CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Native Meshers: blockMesh (
-   -   Errors during blockMesh meshing (

Madeleine P. Vincent September 8, 2011 10:10

Errors during blockMesh meshing
1 Attachment(s)
Hi all,

I have a blockMeshDict file that I can't seem to get to mesh correctly. I have verified all the vertices, blocks, patches, etc.

Can someone help me track down the error in my ways?

The file is attached.

Thanks for your help,

MartinB September 8, 2011 11:04

Hi Madeleine,

the problem with mergePatchPairs is, that after merging the first two patches, no other patch to be merged should be adjacent to the already merged ones.

One solution is to define three blocks instead of one big block which must be merged. So all in all you should add six additional blocks. This would be my preferred solution.

A minor saving can be achieved by only adding two blocks in x-direction and two mergePatchPairs entries for the upper and the lower part of your geometry.

The rest of your definitions is fine...


Madeleine P. Vincent September 9, 2011 09:27


thank you very much for your reply.

I am trying to make sure that I understand exactly what you are saying.

In the file that I uploaded, the problem is due to the fact the master_pole_right and master_pole_near patches (which are to be merged) touch at one point.

[The same problem exists for the master_pole_right and master_pole_far].

If there is a patch to be merged, it cannot touch any other merged patches, regardless of whether the two patches are parallel and touch at or point, or if they are perpendicular (or any other angle).

And your suggestion is to cut the 3 large blocks into 4 small blocks each, with each small block directly interfacing (1 to 1) with the blocks adjacent to it. In this way, there is no merging of patches needed.

Is that correct?

It seems like a fairly big drawback of the merge patches functionality. This limits the use of merging, and leads to a lot of extra blocks. I am sure there is a good reason...

Again, thanks for your help.


MartinB September 9, 2011 12:43

1 Attachment(s)
Hi Maddy,

yes, it is correct, a possible topology is shown in the attachment.


Madeleine P. Vincent September 14, 2011 04:56


OK - I understand. Thanks again for your help.


fakekarma November 9, 2011 12:30

1 Attachment(s)
Hallo Martin,
I've experienced the same problem with my case, anyway I can't find a solution to avoid the usage of "mergePatchPairs" with my blockMeshDict that I've attached here.

Whene you say "the problem with mergePatchPairs is, that after merging the first two patches, no other patch to be merged should be adjacent to the already merged ones" do you mean that there is no solution at all with "mergePatchPairs"?

Hope that you can help me,

Best regards,


MartinB November 9, 2011 14:22

1 Attachment(s)
Hi Elia,

there is no mergePatchPairs necessary for your mesh. You must use the vertices "multiple" times, i.e. they belong to more than just one block.

The attached blockMeshDict contains the necessary changes and some comments... I left the redundant vertices in place, but you can drop them in your next blockMeshDict.

Oh, you must define the frontAndBack plane as "patch" with boundary condition slip if you want to have a 3D mesh. You can use the "empty" patch only if you define a pure 2D mesh, i.e. one cell in Y direction.


fakekarma November 9, 2011 14:30

1 Attachment(s)
Dear Martin,

I've just thought the same thing during the last hour and I switch to a faceMathing approach as you have described, so at least I'm sure now that every possible try has been made. I've attached my modified blockMeshDict here.

Thanks again for your soon and precise answer,

Best regards,


58alvareznew November 17, 2011 11:44

Help with an error
1 Attachment(s)
Hi Martin,

I am currently a new user to openfoam. I am trying edit a blockMesh file the graded cavity example given with the package. Originally it was a 2x2 and I was trying to create a 3x3. When I run blockMesh from the terminal window I get this error:

FOAM Warning :
From function bool Foam::blockMesh::blockLabelsOK(...)
in file blockMesh/blockMeshCheck.C at line 179
out-of-range point label 16 (max = 15) in block 0

Your help would be much appreciated. Attached is the blockMesh file if this may help.

Thanks, Robert Newsom

MartinB November 17, 2011 12:07

Hi Robert,

if you want to introduce more blocks, you must add appropriate vertices, too. In your blockMeshDict you have only 16 vertices defined in the "vertices" section, but you are using vertex numbers up to 31 in your block definitions.

You see the problem?


58alvareznew November 17, 2011 14:30

Thank You Martin. I guess I forget to add athe appropriate corresponding z values.

58alvareznew November 17, 2011 23:27

Project Help
2 Attachment(s)
Hi Martin,

I am a student and college and I was asked to make CFD models for my senior design project. I have never done any modeling before this is my first time. I am trying to make a model and examine how the air flow through a diffuser changes. I have looked at the manuel on the openfoam website and it is not helping that much. I was wondering if you could give me any advice on how to approach it. I have the openfoam installed and I can run the first example program.

I found an additional example on the internet that looks very similar to what I am trying to do. It is also an example given from openfoam. The case is named cylinder. It is in the tutorials>basic>potentialFoam>cylinder.
I was able to get the blockMesh created but I get an error that says that file can not be found? I believe the it is because of the controlDict file. I have attached it. Also I attached a figure of that I am trying to model.

Martin I really appreciate your help.
Thank you very much, Robert Newsom

afo November 18, 2011 05:51

blockMeshDict topology
2 Attachment(s)
Hi Martin,

I'm trying to compile a blockMeshDict file, in order to generate the geometry for a hopper. when I run blockMesh, the console returns this error

Creating block mesh from
No non-linear edges defined
Creating topology blocks
Creating topology patches

Check topology
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam201/platforms/linuxGccDPOpt/lib/"
#1 Foam::sigSegv::sigHandler(int) in "/opt/openfoam201/platforms/linuxGccDPOpt/lib/"
#2 Uninterpreted:
#3 Foam::blockMesh::checkBlockMesh(Foam::polyMesh const&) const in "/opt/openfoam201/platforms/linuxGccDPOpt/lib/"
#4 Foam::blockMesh::createTopology(Foam::IOdictionary const&, Foam::word const&) in "/opt/openfoam201/platforms/linuxGccDPOpt/lib/"
#5 Foam::blockMesh::blockMesh(Foam::IOdictionary const&, Foam::word const&) in "/opt/openfoam201/platforms/linuxGccDPOpt/lib/"
in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/blockMesh"
#7 __libc_start_main in "/lib/tls/i686/cmov/"
in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/blockMesh"
Segmentation fault

there must be something wrong with the topology, but I can't figure out what it is. I'm including the blockMeshDict file and the hopper plantform , I'd really appreciate your help.
Thank you in advance, Paolo

MartinB November 18, 2011 06:22

1 Attachment(s)
Hi Robert,

your sketch in the Word document is not really readable in my Libre Office Writer... making a PDF or an .png might be a better way to communicate sketches.

The tutorial you mention is using the codeStream functionality for demonstration purposes. It runs fine within a pure Linux environment, but it may cause trouble in Windows.

If you just want to use the mesh itself you can use the blockMeshDict from the previous OpenFOAM-1.7 version, I attached the file. You have to unpack the archive and replace the blockMeshDict file in the /constant/polyMesh directory. In the system/controlDict you can remove the "functions { ... }" part.

Some information about a diffuser can be found in the openfoamwiki:


MartinB November 18, 2011 06:53

4 Attachment(s)
Hi Paolo, (and Robert, this might be interesting for you, too...)

the numeration of the hexblocks is bad, as well as the definition of the frontAndBack patches.

To "debug" these kind of problems you can do this:

- Increase z-Coordinate from 6.2 to 996.2 or similar to get a better overview in the following steps.

- Create empty dummy entries for edges, boundary etc, just to have a complete blockMeshDict.

- Start "paraFoam -blocks", you can visualize the problems in Paraview with "Surface with Edges" or "Wireframe" option.

- Comment all blocks from the blockMeshDict and add them one by one again. Control the definition of the blocks in Paraview.

- After all blocks are fine add the patches one by one.

- After this is done, too, decrease the z-Coordinate again.

Some of the intermediate steps are shown in the attached files.

The corrected version of the blockMeshDict is attached, too.


afo November 18, 2011 07:02

Many Thanks
Hi Martin,
I really thank you for your help, that was very kind of you! I'll let you know if everything worked fine. :)

afo November 18, 2011 07:47

yes it works
Thanks Martin everything works fine! You made my day! :D

afo November 24, 2011 10:52

default faces
1 Attachment(s)
Hi martin

sorry if I disturb you again, the mesh you corrected last week worked well. I made a little change in order to insert a smaller inlet, when i run it, blockMesh builds it, and paraview doesn't show anything wrong, I'am able to run simulations too, but console returns with a minor error and creates default faces in boundary:

reating block mesh topology
--> FOAM Warning :
From function polyMesh::polyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 881
Found 1 undefined faces in mesh; adding to default patch.

Check topology

Basic statistics
Number of internal faces : 6
Number of boundary faces : 30
Number of defined boundary faces : 30
Number of undefined boundary faces : 0
Checking patch -> block consistency

Creating block offsets
Creating merge list .

Creating polyMesh from blockMesh
Creating patches
Creating cells
Creating points with scale 0.001

There are no merge patch pairs edges

Writing polyMesh
Mesh Information
boundingBox: (-4.073 0 0) (-0.134 7.093 0.0062)
nPoints: 3572
nCells: 1700
nFaces: 6885
nInternalFaces: 3295
patch 0 (start: 3295 size: 140) name: walls
patch 1 (start: 3435 size: 3400) name: frontAndBack
patch 2 (start: 6835 size: 20) name: inlet
patch 3 (start: 6855 size: 10) name: inletCentral
patch 4 (start: 6865 size: 20) name: outlet
patch 5 (start: 6885 size: 0) name: defaultFaces


how can i fix this? I include constant and 0 folders, if they might help you.

Thank you again Paolo

MartinB November 24, 2011 11:24

Hi Paolo,

it's just a warning so generally you can try to ignore it.

The exact reason is the face (14 29 29 14), which is a face collapsed to a line, and which results from the wedge shaped block #6.

You can add these lines to your blockMeshDict and make the warning disappear:
type empty;
(14 29 29 14)

But you must define BC's for the "dummy" patch again. Another idea is to add the face to your "walls" patch: the warning should disappear and it is treated like a wall...


afo November 25, 2011 03:23

thanks again Martin

All times are GMT -4. The time now is 04:23.