CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...

Unstructured hex mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 13, 2006, 08:23
Default Hi everybody, Here at my un
  #1
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 9
lr103476 is on a distinguished road
Hi everybody,

Here at my university people are also working with Hexpress (by Numeca int.), which also generates unstructured hexa(poly)hedral meshes. Mesh density is regulated by the creation of refinement block. So at those block-interfaces cells are doubled or halved in size.

When I convert such a mesh to Fluent everything is OK, I can fully use the mesh in Fluent for computations and stuff.

Two problems occur:

1) I cannot convert this Fluent mesh to OpenFOAM, a segmentation fault after 'Creating shapes for 3-D cells'.

2) Via starCD format I am able to convert this mesh to OpenFOAM, but strange things occur at the interfaces of the refinement block -> At the 'hanging nodes' tetrahedral cells are generated, which is strange.

The unstructured (hexpress) mesh and close up looks like this:
http://www.aero.lr.tudelft.nl/~frank.../test_full.png
http://www.aero.lr.tudelft.nl/~frank/images/test.png

The conversion (via starToFoam) looks like:
http://www.aero.lr.tudelft.nl/~frank/images/test_OF.png


Any ideas?

Frank
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   November 14, 2006, 04:13
Default What you have here is a mesh w
  #2
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
What you have here is a mesh with "hanging nodes", in Fluent terminology.
There is a discution on the forum hanging nodes regarding the import of such meshes from fluent.
The suggested solution is what you have done (route through star), because, at least for the moment, fluentMeshToFoam has to be completed in order to be able to import this type of mesh.

Dragos
dmoroian is offline   Reply With Quote

Old   November 14, 2006, 04:29
Default Allright. But in my view,
  #3
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 9
lr103476 is on a distinguished road
Allright.

But in my view, star-CD is capable of handling the interfaces between the refinement blocks. So why are there still pyramid shaped cells at those interfaces?

Frank
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   November 14, 2006, 05:14
Default I am no expert, so I might be
  #4
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
I am no expert, so I might be wrong, but here is what I understood until now from OpenFOAM: one of the rules regarding the mesh in OpenFOAM, is that one face may belong to maximum 2 cells (one cell on each side of the face, or one cell and nothing on the other side if it's a boundary face).
In your case, the mesh breaks the rule, because at the interface, there are faces belonging to at least 3 cells. If you look at the interface between the coarse and fine mesh, one face on the coarse side is matching 2 faces on the fine mesh (in 2D). What it is needed is to split the face from the coarse side of the mesh in 2, so it will match the fine side faces. Here comes starToFoam (I think) which replaces the big face with two smaller ones. Why it does it in that staggering way, I have no idea.

Dragos
dmoroian is offline   Reply With Quote

Old   November 14, 2006, 05:15
Default Just a few questions: * Are
  #5
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Just a few questions:

* Are the couples created correctly for your Star-CD mesh?

* If you have access to pro-STAR, try using one of the v4 series. In the new version, couples can be used as before, but they are removed via a cptranslate command before the ccm file is saved. There will then be no hanging nodes, but instead the cell faces will be split to create polys, which are just the right thing for OpenFOAM
olesen is offline   Reply With Quote

Old   November 14, 2006, 05:43
Default What do you mean by couples? H
  #6
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 9
lr103476 is on a distinguished road
What do you mean by couples? How do I check if there are created correctly?

No, we dont have Star-CD or pro-Star here.

Frank
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   November 14, 2006, 05:56
Default Couples represent either an in
  #7
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Couples represent either an integral match or an arbitrary match between cells. They used to be in a '.cpl' file, but perhaps your export tool writes them somewhere else (or not at all).

If the format is well documented or easy to decode, you might think about writing your own import routine (not as hard as it may sound).

The brute force solution would be to write out each level of refinement as an individual mesh, convert each to an OpenFOAM mesh and use something like mergeMeshes to join them together.
olesen is offline   Reply With Quote

Old   November 14, 2006, 06:24
Default @ But in my view, star-CD is c
  #8
Senior Member
 
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8
jens_klostermann is on a distinguished road
@ But in my view, star-CD is capable of handling the interfaces between the refinement blocks. So why are there still pyramid shaped cells at those interfaces?

The pyramid shaped cells has to do with paraview (or maybe the pvReader). This problem was mentioned in one of the discussions earlier.

Jens
jens_klostermann is offline   Reply With Quote

Old   November 14, 2006, 06:43
Default Just do a checkMesh and check
  #9
Senior Member
 
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8
jens_klostermann is on a distinguished road
Just do a checkMesh and check what celltypes are present!

Jens
jens_klostermann is offline   Reply With Quote

Old   November 14, 2006, 06:58
Default checkMesh delivers the followi
  #10
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 9
lr103476 is on a distinguished road
checkMesh delivers the following results:

Number of cells by type:
hexahedra: 2106
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 246
Number of regions: 1 (OK).

So in fact there are some polyhedrals present and thus its a conversion issue.

btw, when I switch off the internal mesh in paraview, the mesh looks good. The polyhedrals are created by conversion only in the 3th dimension.

Frank
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   November 14, 2006, 07:16
Default So this left cell are your pol
  #11
Senior Member
 
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8
jens_klostermann is on a distinguished road
So this left cell are your polyhedra (in 3D a decaeder in 2D pentas or so):

+--+--+
|00|00|
|00+--+
|00|00|
+--+--+

(Sorry for the bad draft!)

and everything is fine, is'n it

Jens
jens_klostermann is offline   Reply With Quote

Old   November 14, 2006, 07:21
Default mmm, yes, I guess you're right
  #12
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 9
lr103476 is on a distinguished road
mmm, yes, I guess you're right. Sometimes, in paraFoam thing looks different then they really are. Is foamToTecplot already supporting polyhedrals?

Frank
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   November 24, 2006, 06:56
Default Allright, I solved this proble
  #13
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 9
lr103476 is on a distinguished road
Allright, I solved this problem partially by using zipUpMesh to remove the hanging nodes. Very easy!.

Now a second problem arises, when I want to move the mesh. Using checkMesh I got the following warning:

==========================================
--> FOAM Warning :
From function bool primitiveMesh::warnCommonPoints(const label, const Map<label>&, bool&) const
in file meshes/primitiveMesh/primitiveMeshCheck.C at line 1607
Face 11 vertex labels 5(36095 36108 41 50 40) and face 12 vertex labels 6(40 50 41 385 37 36) share 3 vertices.
This mesh should only be used with faceDecomp finiteElement decomposition.
Further face-face warnings will be suppressed.
Face-face connectivity OK.
==========================================

The result is that I can't get this mesh moving using one of my solvers based on icoDyMFoam.

==========================================
==> How do I use faceDecomp finiteElement decomposition ???
==========================================

Regards, Frank
__________________
Frank Bos
lr103476 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
unstructured mesh phoenics user Phoenics 26 March 22, 2012 13:17
Structurted mesh and unstructured mesh Wiroon Main CFD Forum 4 July 1, 2005 04:41
Structurted mesh and unstructured mesh Wiroon FLUENT 2 June 28, 2005 09:40
unstructured mesh mehd icho Main CFD Forum 0 February 27, 2003 08:44
Unstructured mesh Mir CD-adapco 2 May 15, 2002 15:44


All times are GMT -4. The time now is 07:27.