CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Meshing & Mesh Conversion

[blockMesh] Internal Walls

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

Like Tree1Likes
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 21, 2010, 03:56
Default Internal Walls
  #1
Senior Member
 
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 12
balkrishna is on a distinguished road
I wish to generate a mesh for the geometry below. It is an air lift reactor :



My blockMeshDict is as follows :
Code:
/*--------------------------------*- C++ -*----------------------------------* \
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.01;

vertices
(
    (0 0 0)
    (9.7 0 0)
    (9.7 12 0)
    (0 12 0)
    (10.3 0 0)
    (10.3 12 0)
    (21.7 0 0)
    (21.7 12 0)
    (22.3 0 0)
    (22.3 12 0)
    (32 0 0)
    (32 12 0)
    (0 0 14)
    (9.7 0 14)
    (9.7 12 14)
    (0 12 14)
    (10.3 0 14)
    (10.3 12 14)
    (21.7 0 14)
    (21.7 12 14)
    (22.3 0 14)
    (22.3 12 14)
    (32 0 14)
    (32 12 14)
    (0 0 130)
    (9.7 0 130)
    (9.7 12 130)
    (0 12 130)
    (10.3 0 130)
    (10.3 12 130)
    (21.7 0 130)
    (21.7 12 130)
    (22.3 0 130)
    (22.3 12 130)
    (32 0 130)
    (32 12 130)
    (0 0 140)
    (9.7 0 140)
    (9.7 12 140)
    (0 12 140)
    (10.3 0 140)
    (10.3 12 140)
    (21.7 0 140)
    (21.7 12 140)
    (22.3 0 140)
    (22.3 12 140)
    (32 0 140)
    (32 12 140)
);

blocks
(
 hex (0 1 2 3 12 13 14 15) (10 10 10) simpleGrading (1 1 1)
 hex (1 4 5 2 13 16 17 14) (4 10 10) simpleGrading (1 1 1)
 hex (4 6 7 5 16 18 19 17) (10 10 10) simpleGrading (1 1 1)
 hex (6 8 9 7 18 20 21 19) (4 10 10) simpleGrading (1 1 1)
 hex (8 10 11 9 20 22 23 21) (10 10 10) simpleGrading (1 1 1)
 hex (12 13 14 15 24 25 26 27) (10 10 100) simpleGrading (1 1 1)
 hex (13 16 17 14 25 28 29 26) (4 10 100) simpleGrading (1 1 1)
 hex (16 18 19 17 28 30 31 29) (10 10 100) simpleGrading (1 1 1)
 hex (18 20 21 19 30 32 33 31) (4 10 100) simpleGrading (1 1 1)
 hex (20 22 23 21 32 34 35 33) (10 10 100) simpleGrading (1 1 1)
 hex (24 25 26 27 36 37 38 39) (10 10 10) simpleGrading (1 1 1)
 hex (25 28 29 26 37 40 41 38) (4 10 10) simpleGrading (1 1 1)
 hex (28 30 31 29 40 42 43 41) (10 10 10) simpleGrading (1 1 1)
 hex (30 32 33 31 42 44 45 43) (4 10 10) simpleGrading (1 1 1)
 hex (32 34 35 33 44 46 47 45) (10 10 10) simpleGrading (1 1 1)
  );

edges
(
);

patches
(
 patch sparger (
	      (4 6 7 5)
	      ) 

 patch outlet (
     (36 37 38 39)
     (37 40 41 38 )
     (40 42 43 41)
     (42 44 45 43)
     (44 46 47 45)
       	       )


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

mergePatchPairs 
(
);

// ************************************************************************* //
This gives the following error on running blockMesh :
Code:
--> FOAM FATAL ERROR: 
Trying to specify a boundary face 4(13 16 17 14) on the face on cell 1 which is either an internal face or already belongs to some other patch.  This is face 16 of patch 2 named walls.

    From function polyMesh::polyMesh
(
    const IOobject&,
    const Xfer<pointField>&,
    const cellShapeList& cellsAsShapes,
    const faceListList& boundaryFaces,
    const wordList& boundaryPatchTypes,
    const wordList& boundaryPatchNames,
    const word& defaultBoundaryPatchType
)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 483.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/home/ifmg/OpenFOAM/OpenFOAM-1.7.0/lib/linuxGccDPOpt/libOpenFOAM.so"
#1  Foam::error::abort() in "/home/ifmg/OpenFOAM/OpenFOAM-1.7.0/lib/linuxGccDPOpt/libOpenFOAM.so"
#2  Foam::polyMesh::polyMesh(Foam::IOobject const&, Foam::Xfer<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/ifmg/OpenFOAM/OpenFOAM-1.7.0/lib/linuxGccDPOpt/libOpenFOAM.so"
#3  
 in "/home/ifmg/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linuxGccDPOpt/blockMesh"
#4  
 in "/home/ifmg/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linuxGccDPOpt/blockMesh"
#5  
 in "/home/ifmg/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linuxGccDPOpt/blockMesh"
#6  __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#7  
 in "/home/ifmg/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linuxGccDPOpt/blockMesh"
Aborted
How do i specify wall boundary condition for the internal walls . I checked the forums for the same but no topic could help me out . Do suggest me on how to overcome this error .

Last edited by balkrishna; October 21, 2010 at 04:54.
balkrishna is offline   Reply With Quote

Old   July 21, 2011, 19:14
Default
  #2
Senior Member
 
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 12
kumar is on a distinguished road
HI balakrishna,
Did you manage to mesh your internal boundaries. I have a similar problem with same error and want to use blockMesh to solve thisproblem.

Give me suggestions to solve this problem.


regards
K.SUresh kumar
kumar is offline   Reply With Quote

Old   July 21, 2011, 19:54
Default
  #3
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,956
Blog Entries: 43
Rep Power: 121
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Greetings to both of you!

Check this tutorial: multiphase/interDyMFoam/ras/damBreakWithObstacle

See Allrun and createObstacle.setSet.

For more about setSet: http://openfoamwiki.net/index.php/SetSet

Best regards,
Bruno
mizzou likes this.
__________________
wyldckat is offline   Reply With Quote

Old   July 22, 2011, 01:22
Default
  #4
Senior Member
 
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 12
balkrishna is on a distinguished road
Yes ..... this was a long time ago .... i managed to do the meshing and run the case too .... The key was in not meshing the baffles .... i.e. i commented the lines in red ....
Code:
blocks
(
 hex (0 1 2 3 12 13 14 15) (10 10 10) simpleGrading (1 1 1)
 hex (1 4 5 2 13 16 17 14) (4 10 10) simpleGrading (1 1 1)
 hex (4 6 7 5 16 18 19 17) (10 10 10) simpleGrading (1 1 1)
 hex (6 8 9 7 18 20 21 19) (4 10 10) simpleGrading (1 1 1)
 hex (8 10 11 9 20 22 23 21) (10 10 10) simpleGrading (1 1 1)
 hex (12 13 14 15 24 25 26 27) (10 10 100) simpleGrading (1 1 1)
// hex (13 16 17 14 25 28 29 26) (4 10 100) simpleGrading (1 1 1)
 hex (16 18 19 17 28 30 31 29) (10 10 100) simpleGrading (1 1 1)
// hex (18 20 21 19 30 32 33 31) (4 10 100) simpleGrading (1 1 1)
 hex (20 22 23 21 32 34 35 33) (10 10 100) simpleGrading (1 1 1)
 hex (24 25 26 27 36 37 38 39) (10 10 10) simpleGrading (1 1 1)
 hex (25 28 29 26 37 40 41 38) (4 10 10) simpleGrading (1 1 1)
 hex (28 30 31 29 40 42 43 41) (10 10 10) simpleGrading (1 1 1)
 hex (30 32 33 31 42 44 45 43) (4 10 10) simpleGrading (1 1 1)
 hex (32 34 35 33 44 46 47 45) (10 10 10) simpleGrading (1 1 1)
  );
balkrishna is offline   Reply With Quote

Old   July 22, 2011, 02:54
Default
  #5
Senior Member
 
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 12
kumar is on a distinguished road
HI Bruno,
Thanks for pointing the right direction. This is what I want. I already started looking in to the tutorial.

I think it will help me solve the problem.


regards
K.SUresh kumar
kumar is offline   Reply With Quote

Old   February 20, 2017, 12:21
Default Internal Patches
  #6
New Member
 
Join Date: Feb 2017
Posts: 5
Rep Power: 5
CHiller is on a distinguished road
Hi, I want to create an internal patch using blockMesh. But while generating the mesh I get an error. Can someone tell me how to create internal patches, boundaries or baffles with blockMesh?

sketch of the case:


blockMeshDict:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
        ( 0  0  0) //  0
	(10  0  0) //  1
	(10  1  0) //  2
	( 0  1  0) //  3
	(10  2  0) //  4
	( 0  2  0) //  5
	(10  3  0) //  6
	( 0  3  0) //  7
	
	( 0  0  0.1) //  8
	(10  0  0.1) //  9
	(10  1  0.1) // 10
	( 0  1  0.1) // 11
	(10  2  0.1) // 12
	( 0  2  0.1) // 13
	(10  3  0.1) // 14
	( 0  3  0.1) // 15
);

blocks
(

        hex ( 0  1  2  3  8  9 10 11) (20 2 1) simpleGrading (1 1 1)
	hex ( 3  2  4  5 11 10 12 13) (20 2 1) simpleGrading (1 1 1)
	hex ( 5  4  6  7 13 12 14 15) (20 2 1) simpleGrading (1 1 1)
);

edges
(
);

patches
(
	patch inernalPatch
	(
		( 5  4 12 13)
		( 3 11 10  2)
	)
);

boundary
(
);

mergePatchPairs
(
);

// ************************************************************************* //
The output after running blockMesh:
Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
/*   Windows 32 and 64 bit porting by blueCAPE: http://www.bluecape.com.pt   *\
|  Based on Windows porting (2.0.x v4) by Symscape: http://www.symscape.com   |
\*---------------------------------------------------------------------------*/
Build  : 4.x-ed69f631ce88
Exec   : C:/PROGRA~1/BLUECF~1/OpenFOAM-4.x/platforms/mingw_w64GccDPInt32Opt/bin/blockMesh.exe
Date   : Feb 20 2017
Time   : 17:10:20
Host   : "FENNEK"
PID    : 1300
Case   : C:/PROGRA~1/BLUECF~1/ofuser-of4/run/incompressible/porousSimpleFoam/pultrusion_0215
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Creating block mesh from
    "C:/PROGRA~1/BLUECF~1/ofuser-of4/run/incompressible/porousSimpleFoam/pultrusion_0215/system/blockMeshDict"
Creating curved edges
Creating topology blocks
Creating topology patches

Reading patches section

Creating block mesh topology

Reading physicalType from existing boundary file

Default patch type set to empty


--> FOAM FATAL ERROR:
Trying to specify a boundary face 4(5 4 12 13) on the face on cell 1 which is either an internal face or already belongs to some other patch.  This is face 0 of patch 0 named inernalPatch.

    From function void Foam::polyMesh::setTopology(const cellShapeList&, const faceListList&, const wordList&, Foam::labelList&, Foam::labelList&, Foam::label&, Foam::label&, Foam::cellList&)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 324.

FOAM aborting

We're sorry, but the application crashed and safe stack tracing isn't available in this current implementation of blueCFD-Core patches for OpenFOAM.

This application has requested the Runtime to terminate it in an unusual way.
Please contact the application's support team for more information.
CHiller is offline   Reply With Quote

Old   April 21, 2017, 07:00
Default
  #7
Senior Member
 
KaLium's Avatar
 
Kal-El
Join Date: Apr 2017
Location: Finland
Posts: 150
Rep Power: 4
KaLium is on a distinguished road
Why are you using blockMesh for a complex geometry?

I would recommend snappyHexMesh.
KaLium is offline   Reply With Quote

Old   April 21, 2017, 10:16
Default
  #8
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,887
Rep Power: 34
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Hi all,

@CHiller

Your blocks were merged, you as blockMesh said, you are trying to create patch inside the mesh (and it worries blockMesh). You have several choices:

1. Use 4 additional points (though with identical coordinates) to avoid automatic block merging.
2. Use createBaffles utility to create "patch" inside a mesh.

@KaLium

Complex geometry?
alexeym is offline   Reply With Quote

Old   September 11, 2019, 18:04
Default Thanks
  #9
New Member
 
Join Date: Apr 2017
Posts: 9
Rep Power: 4
haydii is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Greetings to both of you!

Check this tutorial: multiphase/interDyMFoam/ras/damBreakWithObstacle

See Allrun and createObstacle.setSet.

For more about setSet: http://openfoamwiki.net/index.php/SetSet

Best regards,
Bruno

Many thanks Dear Bruno for straight help, It definitely works !

Regards,
Haydi
haydii is offline   Reply With Quote

Reply

Tags
blockmesh, error, loop, reactor

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Internal Flow in an Arch yjia2 OpenFOAM Pre-Processing 2 June 16, 2018 11:54
Possible to create cyliner baffle (internal) using topoSet or stl Mesh? keepfit OpenFOAM 4 February 19, 2017 15:40
[Gmsh] Generating multiple internal walls using gmshToFoam rendagar OpenFOAM Meshing & Mesh Conversion 2 October 20, 2014 04:56
[ICEM] Dealing with thin internal walls in geomety FreeFall79 ANSYS Meshing & Geometry 4 November 13, 2013 12:16
Heat Flux at Internal walls or Fluid Solid Interface Mahi CFX 3 October 1, 2012 03:18


All times are GMT -4. The time now is 12:41.