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

BlockMesh face merging

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 10, 2005, 03:21
Default Is there a blockMesh file in t
  #1
Member
 
Duderino
Join Date: Mar 2009
Posts: 40
Rep Power: 8
duderino is on a distinguished road
Is there a blockMesh file in the tutorials where face merging is used? I want to look at the syntax.

Thank you!
duderino is offline   Reply With Quote

Old   March 10, 2005, 04:38
Default I think there's merging in the
  #2
New Member
 
Chris Greenshields
Join Date: Mar 2009
Posts: 28
Rep Power: 8
chris is on a distinguished road
I think there's merging in the example case:
$FOAM_TUTORIALS/simpleFoam/pitzDaily3Blocks

The documentation about face merging is at:
http://www.opencfd.co.uk/openfoam/do...32-1680006.3.2
chris is offline   Reply With Quote

Old   March 10, 2005, 09:40
Default In my case, `simpleFoam . pitz
  #3
nakamura
Guest
 
Posts: n/a
In my case, `simpleFoam . pitzDaily3Blocks` shows "--> FOAM FATAL IO ERROR : keyword interface is undefined ....".
So I changed the type of interface from patch to wall
and added some lines like
interface
{
type fixedValue;
value uniform (0 0 0);
}
to 0/{R,U,epsilon,k,nuTilda,p}.
After these changes I can excute it.
I think that after merging the patch "interface" has no sence but simpleFoam may not think so,,,
  Reply With Quote

Old   March 12, 2005, 09:49
Default I want to attach (merge) a cub
  #4
Member
 
Duderino
Join Date: Mar 2009
Posts: 40
Rep Power: 8
duderino is on a distinguished road
I want to attach (merge) a cuboid to the curved surface of a cylinder with blockMesh. The blockMesh tool generates a grid which looks good. But at the merged cell layers it somehow produces pyramid-cells, which are unwanted.

What can I do to merge the cuboid to the cylinder without the pyramid-cells?

May somebody with blockMesh experience can look at it?! I attache the blockMeshDict file
blockMeshDict
duderino is offline   Reply With Quote

Old   March 14, 2005, 04:39
Default Hi Duderino, I run checkMes
  #5
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Hi Duderino,

I run checkMesh on your geometry and get

hexahedra: 2516
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 9
Number of regions: 1 (OK).


So it seems to have correctly merged the cells and introduced 9 general polyhedra (i.e. anything not of the above) on the interface. You might see them as pyramids since vtk/paraview cannot handle polyhedra and we decompose them before passing them to vtk)

You can pick these up using the cellSet utility (in mesh/manipulation). See the cellSetDict dictionary on how to use it ('shapeToCell')

Mattijs
mattijs is offline   Reply With Quote

Old   March 15, 2005, 05:49
Default Hi Mattijs, Thank you for y
  #6
Member
 
Duderino
Join Date: Mar 2009
Posts: 40
Rep Power: 8
duderino is on a distinguished road
Hi Mattijs,

Thank you for your help.

If I merge two patches (surfaces) at the exakt same location of the exakt same size, I will get two "internal" patches(with nFaces 0).
Allthough this "internal" patch has zero(?) Faces, I am still asked for a boundary condition.

Does it matter which boudary I choose?

Thank you!
duderino is offline   Reply With Quote

Old   March 15, 2005, 06:02
Default a) leave them there and give t
  #7
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
a) leave them there and give them a 'simple' boundary condition (e.g. fixedValue)

b) remove them. You can edit the polyMesh/boundary file and remove the patches with zero faces (and adapt the number of patches at the top of the file).

(Note that removing patches is only allowed for zero-sized patches)
mattijs is offline   Reply With Quote

Old   March 15, 2005, 07:25
Default Hi Mattijs, I've applied yo
  #8
nakamura
Guest
 
Posts: n/a
Hi Mattijs,

I've applied your suggestion b) to simpleFoam/pitzDaily3Blocks and it goes fine.

Thanks.
  Reply With Quote

Old   March 31, 2006, 19:42
Default I am trying to merge two patch
  #9
jimhuang
Guest
 
Posts: n/a
I am trying to merge two patches with a shared edge. Could any one tell me how to declare both patches as the masters. Thanks!

Jim
  Reply With Quote

Old   June 23, 2008, 22:25
Default hi everyone. i was trying to c
  #10
New Member
 
nikhil babu madduri
Join Date: Mar 2009
Posts: 17
Rep Power: 8
nikhilmadduri is on a distinguished road
hi everyone. i was trying to create a mesh around a solid cylinder. can anyone suggest me which will be the best way? as im new to openfoam, i started with quarter part of the whole mesh to be generated containg the quarter of the cylinder. i did it in blockmesh...while executing it, i was finding the following errors. can anyone suggest me what might be the bug in here?

/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4.1 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : blockMesh /home/nikhil/OpenFOAM/nikhil-1.4.1/run/tutorials/icoFoam cavi
tyGrade
Date : Jun 24 2008
Time : 09:42:12
Host : localhost
PID : 22816
Root : /home/nikhil/OpenFOAM/nikhil-1.4.1/run/tutorials/icoFoam
Case : cavityGrade
Nprocs : 1
Create time


Reading block mesh description dictionary

Creating block mesh

Creating blockCorners

Creating curved edges

Creating blocks

Creating patches

Creating block mesh topology

Default patch type set to empty

Check block mesh topology

Basic statistics
Number of internal faces : 0
Number of boundary faces : 12
Number of defined boundary faces : 12
Number of undefined boundary faces : 0

Checking patch -> block consistency

Creating block offsets

Creating merge list .

Creating points

Creating cells

Creating patches

Creating mesh from block mesh

Default patch type set to empty

Creating merge patch pairs

Adding point and face zones
Creating attachPolyTopoChanger
#0 Foam::error::printStack(Foam:stream&) in "/home/nikhil/OpenFOAM/OpenFOAM-1
.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/nikhil/OpenFOAM/OpenFOAM-1.4.1/li
b/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xffffe420]
#3 Foam::triangle<foam::vector<double>, Foam::Vector<double> const&>::ray(Foam:
:Vector<double> const&, Foam::Vector<double> const&, Foam::intersection::algorit
hm, Foam::intersection::direction) const in "/home/nikhil/OpenFOAM/OpenFOAM-1.4.
1/lib/linuxGccDPOpt/libmeshTools.so"
#4 Foam::face::ray(Foam::Vector<double> const&, Foam::Vector<double> const&, Fo
am::Field<foam::vector<double> > const&, Foam::intersection::algorithm, Foam::in
tersection::direction) const in "/home/nikhil/OpenFOAM/OpenFOAM-1.4.1/lib/linuxG
ccDPOpt/libOpenFOAM.so"
#5 Foam::List<foam::objecthit> Foam::PrimitivePatch<foam::face,> > const&>::projectPoints<foam::primitivepatch<foam> > const&> >(Foam::Primitive Patch<foam::face,> > const&> const&, Foam::Field<foam::vector<double> > const&, Foam::intersection::algorithm, Foam: :intersection::direction) const in "/home/nikhil/OpenFOAM/OpenFOAM-1.4.1/lib/lin uxGccDPOpt/libdynamicMesh.so"
#6 Foam::slidingInterface::projectPoints() const in "/home/nikhil/OpenFOAM/Open FOAM-1.4.1/lib/linuxGccDPOpt/libdynamicMesh.so"
#7 Foam::slidingInterface::changeTopology() const in "/home/nikhil/OpenFOAM/Ope nFOAM-1.4.1/lib/linuxGccDPOpt/libdynamicMesh.so"
#8 Foam::polyTopoChanger::changeTopology() const in "/home/nikhil/OpenFOAM/Open FOAM-1.4.1/lib/linuxGccDPOpt/libdynamicMesh.so"
#9 Foam::polyTopoChanger::changeMesh(bool, bool) in "/home/nikhil/OpenFOAM/Open FOAM-1.4.1/lib/linuxGccDPOpt/libdynamicMesh.so"
#10 Foam::attachPolyTopoChanger::attach(bool) in "/home/nikhil/OpenFOAM/OpenFOA M-1.4.1/lib/linuxGccDPOpt/libdynamicMesh.so"
#11 main in "/home/nikhil/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOp t/blockMesh"
#12 __libc_start_main in "/lib/i686/libc.so.6"
#13 Foam::regIOobject::readIfModified() in "/home/nikhil/OpenFOAM/OpenFOAM-1.4. 1/applications/bin/linuxGccDPOpt/blockMesh"


regards,
nikhil.
nikhilmadduri is offline   Reply With Quote

Old   February 23, 2010, 09:59
Default
  #11
New Member
 
sesha
Join Date: Mar 2009
Posts: 23
Rep Power: 8
hamsadhwani8 is on a distinguished road
Quote:
Originally Posted by duderino View Post
I want to attach (merge) a cuboid to the curved surface of a cylinder with blockMesh. The blockMesh tool generates a grid which looks good. But at the merged cell layers it somehow produces pyramid-cells, which are unwanted.

What can I do to merge the cuboid to the cylinder without the pyramid-cells?

May somebody with blockMesh experience can look at it?! I attache the blockMeshDict file
blockMeshDict
I have used this blockMesh to run a meshMerger. However, it fails giving me the following. The blockMesh file is attached. FYI I am using OpenFoam-1.5. Can someone help?
>blockMesh
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : blockMesh
Date : Feb 23 2010
Time : 08:48:53
Host : seshasai-srinivasans-macbook-pro.local
PID : 2538
Case : /Volumes/OpenFOAM/stsriniv-1.5/run/tutorials/interFoam/poreDrop/mergeTest
nProcs : 1

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


Reading block mesh description dictionary

Creating block mesh

Creating blockCorners

Creating curved edges

Creating blocks

Creating patches

Creating block mesh topology

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 5 undefined faces in mesh; adding to default patch.

Check block mesh topology

Basic statistics
Number of internal faces : 8
Number of boundary faces : 20
Number of defined boundary faces : 20
Number of undefined boundary faces : 0

Checking patch -> block consistency

Creating block offsets

Creating merge list .

Creating points

Creating cells

Creating patches

Creating mesh from block mesh

Default patch type set to empty


mergePatchPairs not currently supported.

From function blockMesh
in file genBlockMesh.C at line 198.

FOAM exiting
Attached Files
File Type: txt blockMeshDict.txt (2.9 KB, 200 views)
hamsadhwani8 is offline   Reply With Quote

Old   March 18, 2010, 07:24
Default
  #12
New Member
 
Marco
Join Date: Mar 2010
Posts: 9
Rep Power: 7
om3ro is on a distinguished road
I could run your code, maybe it's just a different version of OF, 1.6 instead of 1.5 (where mergePatchPairs is not currently supported.)

Marco
om3ro is offline   Reply With Quote

Old   June 23, 2010, 05:56
Default
  #13
New Member
 
Ramnik Singh
Join Date: Jun 2009
Location: Stuttgart, Germany
Posts: 17
Rep Power: 8
Ramnik is on a distinguished road
Quote:
Originally Posted by mattijs View Post
Hi Duderino,

I run checkMesh on your geometry and get

hexahedra: 2516
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 9
Number of regions: 1 (OK).


So it seems to have correctly merged the cells and introduced 9 general polyhedra (i.e. anything not of the above) on the interface. You might see them as pyramids since vtk/paraview cannot handle polyhedra and we decompose them before passing them to vtk)

You can pick these up using the cellSet utility (in mesh/manipulation). See the cellSetDict dictionary on how to use it ('shapeToCell')

Mattijs

Hey Mattijs,

I am having a similar problem while merging faces. I could not undertand this part of ur message.

"You can pick these up using the cellSet utility (in mesh/manipulation). See the cellSetDict dictionary on how to use it ('shapeToCell')"

can u pl help
Thanks
Ramnik
Ramnik 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
merging the meshes Virag CFX 2 March 5, 2007 07:41
vortices merging bin FLUENT 0 March 7, 2005 00:48
merging .ndt files azmir CD-adapco 6 November 7, 2003 22:59
Merging and Uniting Theju FLUENT 0 February 28, 2002 07:10


All times are GMT -4. The time now is 03:06.