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

Problem during creation of a new mesh generator

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 13, 2005, 15:44
Default Hello OpenFoam friends, i a
  #1
New Member
 
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 7
klaus is on a distinguished road
Hello OpenFoam friends,

i am up to include pre/post-processor modules for foam into my CalculiX-pre/post-processor (www.calculix.de). But i encounter problems in situations when two cell-faces match each other, who differ only in the point were the node sequence starts (face 1 starts at point x but face 2 starts at y, for example 0,1,2,3 and 2,1,0,3). Usually just one face who points to the element of higher index is kept. But in this situation (i have a scetch but how can i ship it?) the solver does not work.

I will try to solve the situation with "cyclic faces". One face for each element, but i do not know if it will work.

Has anybody an idea?

Best,
Klaus
klaus is offline   Reply With Quote

Old   July 14, 2005, 05:57
Default Sketch: I usually dump .obj fi
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
Sketch: I usually dump .obj files. Are very simple 3D geometry files.
v x y z
f 1 2 3

Download javaview (www.javaview.de?) or use objToVTK and use Paraview. You can attach the .obj files.

You cannot have two faces inbetween the same two cells. You will have to discard one of them.

Or like you do using cyclics is a solution but a very inefficient one.

Can you do simple geometries already? E.g. two hexes?
mattijs is offline   Reply With Quote

Old   July 14, 2005, 13:12
Default Hello Mattijs, thanks for t
  #3
New Member
 
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 7
klaus is on a distinguished road
Hello Mattijs,

thanks for the reply. Yes i can already create meshes if they are "topologically" simple. That means if the meshed blocks have the same amount of elements at opposide sides. Lets say 10 elements at the bottom and 10 at top. But very often it is usefull to have a mesh-transition from lets say 10 at the bottom to 6 at top. In this case some "top"-faces of elements will join "side"-faces of others. In this case openFoam gives no result.

I had a try with blockMesh were each element was a separate block but also in this case the mesh-transition failed.

By the way the tool which produces the mesh is proven for FEM applications and i use it every day. I just want to add the interface for foam. I can already read the results and create "simple" meshes. But without mesh transition it is hard to realize complicated situations. I know that most CFD-solvers require the "ordered" block-structure but i had the impression that openFoam can deal with arbitrary meshes.

Best,
Klaus

P.S.
i could send a scetch if you like.
klaus is offline   Reply With Quote

Old   July 14, 2005, 13:23
Default yes, please send sketch. -
  #4
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
yes, please send sketch.

- can you output a format for which there is converter? e.g. fluentMeshToFoam?

- Foam has no problems with unstructured meshes. And has no concept of 'blocks' so you will have to do the merging to convert a multi block mesh into an unstructured mesh.

- Please attach blockMeshDict that gave problems.
mattijs is offline   Reply With Quote

Old   July 14, 2005, 16:02
Default Hi Mattijs, how can i attac
  #5
New Member
 
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 7
klaus is on a distinguished road
Hi Mattijs,

how can i attach something in the "Message" window of our discussion board? And no, i have no other format available in my tool which foam understands. Concerning CFD i only support duns in the moment.

I wanted to write a propper polyMesh first but because of the problems i wrote a blockMesh file.

But actually i would like to generate a propper polyMesh file still. How can i deal with situations were two matching elements require a different starting-point for the internal face? (The very question)

I care about a smaller blockMeshDict a bit later and will ship it (something has to be done before)


Klaus
klaus is offline   Reply With Quote

Old   July 14, 2005, 16:08
Default How can i deal with situations
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,734
Rep Power: 20
hjasak will become famous soon enough
Quote:
How can i deal with situations were two matching elements require a different starting-point for the internal face? (The very question)
When Foam does the check on whether two faces are identical, it will search for the appropriate starting point, so the faces (1 2 3 4) and (3 4 1 2) will actually be identical.

However, if you're writing a mesh directly in the FOAM format, this issue does not arise: cells are defined in terms of faces so you never need to ask two faces for equality.

I have written a pretty detailed section on how to make and order elements in your own mesh generators to be used with FOAM - have a search through the manual.

Have fun,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   July 14, 2005, 16:18
Default To attach: \attach{...}
  #7
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
To attach:

\attach{...}

Have a look in Documentation->Formatting on the left.
mattijs is offline   Reply With Quote

Old   July 15, 2005, 18:36
Default Hello Mattijs and Hrvoje, n
  #8
New Member
 
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 7
klaus is on a distinguished road
Hello Mattijs and Hrvoje,

now it runs. The hint to:

- set the number of non-orthogonality correctors to 2 (in system/fvSolution)
- halve the time-step.

did the work. Now i can generate bodies with transient element density. Thanks a lot!

My program cgx will be available in about 2 months with the foam handling capabilities. I will write if it had happened.

So long,
Klaus

P.S:
You wrote:
"The faces have to be ordered such that on a given cell the faces to
neighbouring higher numbered cells are in increasing order if the
neighbouring cells are in increasing order."

does the utility renumberMesh solve this also?
klaus is offline   Reply With Quote

Old   July 18, 2005, 05:25
Default Yes renumberMesh does this as
  #9
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
Yes renumberMesh does this as well.
mattijs 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
Various types of Mesh creation Wooster CFX 0 October 18, 2007 15:53
Mesh Creation Nikos CD-adapco 5 February 1, 2007 20:43
3D Mesh creation ialu CD-adapco 3 June 12, 2002 11:00
Rake Creation Problem Prateep Chatterjee FLUENT 1 February 2, 2001 03:14
3D mesh generator Gassan Abdoulaev Main CFD Forum 4 January 25, 2000 11:20


All times are GMT -4. The time now is 12:40.