CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] merging meshs from different types of blocks

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

Like Tree3Likes
  • 2 Post By diamondx
  • 1 Post By BrolY

Reply
 
LinkBack Thread Tools Display Modes
Old   November 8, 2012, 10:12
Default merging meshs from different types of blocks
  #1
Member
 
Join Date: Jul 2012
Posts: 31
Rep Power: 5
kpax is on a distinguished road
hi everybody,

i am currently trying to mesh a bifurcating vessel using ICEM 14.0.
I managed to create a pre-mesh which seemed reasonable, but pre-mesh quality check tells me that i have some problems with skewness (equiangle skewness has more than 0.3% elements with skewness < 0.05). so i converted one of the blocks to type 'free' (all other blocks are 'mapped'). This reduced the number of highly skewed elements, but when i created the real mesh and checked it, the interface areas between the different types of blocks contained uncovered faces.
When I tried to convert the .msh file to use in OF (using fluentMeshToFoam), i got a weird error that did not occur for all mapped blocks.

so i think the problem is that the different types of blocks need to be connected in some way? I read in another thread that you can simply merge the nodes with a certain tolerance, but that did not work for me.

any help is appreciated.

kpax
kpax is offline   Reply With Quote

Old   November 8, 2012, 12:14
Default
  #2
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
you could try this :

geometry -> create/modify curve -> concatenate/reapproximate curves

You will end with one curve, and it should work.
BrolY is offline   Reply With Quote

Old   November 8, 2012, 12:35
Default
  #3
Member
 
Join Date: Jul 2012
Posts: 31
Rep Power: 5
kpax is on a distinguished road
hmm, not sure what you mean? there is only one curve at the interface of the two blocks (which delineates different surfaces), so nothing to concatenate?!


edit: ok, maybe i should add some pictures. here you can see the blocking i chose (middle one is the free block), and the elements with uncovered faces.
Attached Images
File Type: jpg blocks.jpg (22.9 KB, 20 views)
File Type: jpg uncovFaces.jpg (23.5 KB, 19 views)
kpax is offline   Reply With Quote

Old   November 8, 2012, 13:55
Default
  #4
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
Quote:
Basically, Uncovered faces means that you have volume elements with an exposed side. It should be covered by a shell or another volume element. Missing internal edges means that you have a 2D elements with an exposed side. It should be covered by a line element or another 2D element.

When you get either error (Uncovered faces or missing internal edges), you should push the [Fix] button. This will prompt you to select or type in a new part name. It will create shell elements (or line elements) to cover the "uncovered" faces (or edges) and put the new elements in the part name you selected. You will then have a valid boundary to take to Fluent and use as a wall or internal wall or whatever.

Simon
did you try this, when pushing the fix, name the new part "interior_something" then when setting boundary condition, declare that part as "interior"
Give it a try, you can share your project with us,i'll take a look at it when i have time.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   November 8, 2012, 14:00
Default
  #5
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
Quote:
you could try this :

geometry -> create/modify curve -> concatenate/reapproximate curves

You will end with one curve, and it should work.
Broly, it's either you're drunk or you're in the wrong thread :

How can I extrude a 2D Hexa Mesh along a center curve?
Far and BrolY like this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   November 8, 2012, 14:37
Default
  #6
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
Lol you are right Diamondx !
let's say I'm working too much
Far likes this.
BrolY is offline   Reply With Quote

Old   November 9, 2012, 07:23
Default
  #7
Member
 
Join Date: Jul 2012
Posts: 31
Rep Power: 5
kpax is on a distinguished road
Quote:
Originally Posted by diamondx View Post
did you try this, when pushing the fix, name the new part "interior_something" then when setting boundary condition, declare that part as "interior"
Give it a try, you can share your project with us,i'll take a look at it when i have time.

hey ali,

this seems to be working, the only problem is that after this "fix" i get a multiple edges error. these multiple edges are located around the interfaces as you can see in the attached picture.

i think this is going in the right direction, because OpenFoam seemed to accept the interface internal BC... however, when trying to convert the mesh, i got
"Unused points found in the mesh, number unused by faces: 10444 number unused by cells: 10444"
I guess this is due to the multiple edges?



ps. i also tried putting all the surfaces in the same part, as suggested by simon here: Hex-tet merge
-> did not affect the multiple edge problem described above



edit: i just realized that it's only the middle block that makes problems. e.g., when i choose only the lower block (in the pictures) to be 'free', and the rest as 'mapped', then i dont get any uncovered faces at all. weird.
Attached Images
File Type: jpg multipleEdges.jpg (13.1 KB, 5 views)

Last edited by kpax; November 9, 2012 at 08:09.
kpax is offline   Reply With Quote

Old   November 9, 2012, 08:56
Default
  #8
Member
 
Join Date: Jul 2012
Posts: 31
Rep Power: 5
kpax is on a distinguished road
ok, i think i'm getting closer to the solution...

apparently, the critical step is when i convert the middle block from mapped to free. for some reason, this makes the block turn transparent on one side (see attached pictures). it's this step that leads to uncovered faces.

anyone seen this before?



edit: found a solution. separating the middle block into three parts and converting only the left and right one to type free works.. dont understand why exactly, though.
anyway, thx for your help.
Attached Images
File Type: jpg mappedBlock.jpg (22.0 KB, 6 views)
File Type: jpg freeBlock.jpg (23.2 KB, 8 views)

Last edited by kpax; November 9, 2012 at 09:42.
kpax is offline   Reply With Quote

Old   November 9, 2012, 12:00
Default
  #9
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
What you are experienceing is something I've ever wondered to myself.
For me, it's normal that ICEM sees uncovered faces considering the fact there are more cells on one side of the mesh than the other (the free block can have different number of nodes than the "structured" block).

This trouble is even more obivous when you use the option "refinnement".

That should be something the solver should handle instead of ICEM.
Do you agree with that ?
BrolY is offline   Reply With Quote

Old   November 9, 2012, 12:00
Default
  #10
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
You did great while I was sleeping I'm glad you fixed your problem
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   November 10, 2012, 00:03
Default
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
i am currently trying to mesh a bifurcating vessel using ICEM 14.0.
I managed to create a pre-mesh which seemed reasonable, but pre-mesh quality check tells me that i have some problems with skewness (equiangle skewness has more than 0.3% elements with skewness < 0.05). so i converted one of the blocks to type 'free' (all other blocks are 'mapped'). This reduced the number of highly skewed elements, but when i created the real mesh and checked it, the interface areas between the different types of blocks contained uncovered faces.
Do you access to Simon's tip and tricks where he showed the method to handle the full hexa meshing in similar cases

Quote:
When I tried to convert the .msh file to use in OF (using fluentMeshToFoam), i got a weird error that did not occur for all mapped blocks.
Where this converter is available?


Quote:
so i think the problem is that the different types of blocks need to be connected in some way? I read in another thread that you can simply merge the nodes with a certain tolerance, but that did not work for me.
Cant this problem be tackled with top-down approach more efficiently?
Far is offline   Reply With Quote

Old   November 13, 2012, 10:31
Default
  #12
Member
 
Join Date: Jul 2012
Posts: 31
Rep Power: 5
kpax is on a distinguished road
Quote:
Originally Posted by Far View Post
Do you access to Simon's tip and tricks where he showed the method to handle the full hexa meshing in similar cases
no, do you have a link?


Quote:
Originally Posted by Far View Post
Where this converter is available?
It comes with OF, just type "fluentMeshToFoam mesh.msh" for a file named mesh.msh. usually works quite nicely.

Quote:
Originally Posted by Far View Post
Cant this problem be tackled with top-down approach more efficiently?
could you explain that in a bit more detail?


thx!
kpax 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
dsmcInitialise - dsmcFoam archymedes OpenFOAM Pre-Processing 93 February 11, 2014 02:22
converting Fluent mesh to openfoam standard mesh deepesh OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 17 October 25, 2013 03:59
fluent3DMeshToFoam bego OpenFOAM 27 May 29, 2013 13:08
Difficulty Merging Blocks lsingh OpenFOAM Native Meshers: blockMesh 0 January 26, 2012 10:57
Merging the blocks in ICEM saisanthoshm88 ANSYS Meshing & Geometry 1 December 27, 2010 11:14


All times are GMT -4. The time now is 08:53.