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

[snappyHexMesh] MultiRegions: Snappy creates extra domains between Regions

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

Like Tree1Likes
  • 1 Post By Cartuns11

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 29, 2015, 10:40
Default MultiRegions: Snappy creates extra domains between Regions
  #1
New Member
 
Cartuns11's Avatar
 
Join Date: May 2015
Location: Barcelona
Posts: 24
Rep Power: 7
Cartuns11 is on a distinguished road
Hello,

I have been working on a multiRegion model using snappyHexMesh. I created complex surfaces in stl format, these were closed and had good contacts, but after the snappyHexMesh process, between regions and even on faces-region to outside volume, there were extra domains with 1 or 3 cells......

I have seen some posts in the forum, which talk about this, but I haven't found the solution or the problem cause. May be, for complex geometries, the snappy has problems to approach on surface, I don't know......

Does anyone know some solution?

Thanks. Greetings.
Cartuns11 is offline   Reply With Quote

Old   January 14, 2018, 14:31
Default
  #2
Member
 
Çağatay Emre Ayhan
Join Date: Sep 2017
Location: Istanbul, Turkey
Posts: 31
Rep Power: 5
Cagatayemre is on a distinguished road
Hello, Did you find a solution ?
Cagatayemre is offline   Reply With Quote

Old   January 17, 2018, 09:12
Default
  #3
New Member
 
Cartuns11's Avatar
 
Join Date: May 2015
Location: Barcelona
Posts: 24
Rep Power: 7
Cartuns11 is on a distinguished road
Hi,

(using OF+1606)
Yes! I solved this problem last month! ( coincidence)

The solution is how you name the control volume (==blockMesh volume) and the commands of "splitMeshRegion" application.


First step is to name the blockMesh. I threw blockMesh and snappyHexMesh without a name for the control volume/blockMesh and as consequence, splitMeshRegion named controlVolume as "domain0".....for default. So, blockMesh has to have a name and following codes show where you have to write name in the blockMeshDict ( in this case the name is "air":



Old:

Code:
vertices
(
    (2.7 -0.8 0.57)
    (2.95 -0.8 0.57)
    (2.95 -0.5 0.57)
    (2.7 -0.5 0.57)
    (2.7 -0.8 0.85)
    (2.95 -0.8 0.85)
    (2.95 -0.5 0.85)
    (2.7 -0.5 0.85)
);

blocks
(
    hex (0 1 2 3 4 5 6 7) (60 60 60) simpleGrading (1 1 1)
)

Solution:
Code:
vertices
(
    (2.7 -0.8 0.57)
    (2.95 -0.8 0.57)
    (2.95 -0.5 0.57)
    (2.7 -0.5 0.57)
    (2.7 -0.8 0.85)
    (2.95 -0.8 0.85)
    (2.95 -0.5 0.85)
    (2.7 -0.5 0.85)
);

blocks
(
    hex (0 1 2 3 4 5 6 7) air (60 60 60) simpleGrading (1 1 1)
)

And the last step consists in which commands are introduced in the splitMeshRegion line:


Old:
Code:
 splitMeshRegions -cellZones
This command splits all regions = all cellZones, incluiding domain0, domain1, ......domain2345

Solution:
Code:
 splitMeshRegions -cellZonesOnly
This command only splits the cellZones which are named by the user.


Using these steps, I haven seen the extra domains anymore.
I hope this explanation is useful for you.
phantomsws likes this.
Cartuns11 is offline   Reply With Quote

Old   January 22, 2018, 09:39
Default
  #4
Member
 
Çağatay Emre Ayhan
Join Date: Sep 2017
Location: Istanbul, Turkey
Posts: 31
Rep Power: 5
Cagatayemre is on a distinguished road
Thank you my friend. I also have found a solution to this problem. I have changed the location in mesh coordianates.

There were more than one locations in mesh and. I think that was the problem.


Solution was to put just one location inside the small geometry
Quote:
Originally Posted by Cartuns11 View Post
Hi,

(using OF+1606)
Yes! I solved this problem last month! ( coincidence)

The solution is how you name the control volume (==blockMesh volume) and the commands of "splitMeshRegion" application.


First step is to name the blockMesh. I threw blockMesh and snappyHexMesh without a name for the control volume/blockMesh and as consequence, splitMeshRegion named controlVolume as "domain0".....for default. So, blockMesh has to have a name and following codes show where you have to write name in the blockMeshDict ( in this case the name is "air":



Old:

Code:
vertices
(
    (2.7 -0.8 0.57)
    (2.95 -0.8 0.57)
    (2.95 -0.5 0.57)
    (2.7 -0.5 0.57)
    (2.7 -0.8 0.85)
    (2.95 -0.8 0.85)
    (2.95 -0.5 0.85)
    (2.7 -0.5 0.85)
);

blocks
(
    hex (0 1 2 3 4 5 6 7) (60 60 60) simpleGrading (1 1 1)
)

Solution:
Code:
vertices
(
    (2.7 -0.8 0.57)
    (2.95 -0.8 0.57)
    (2.95 -0.5 0.57)
    (2.7 -0.5 0.57)
    (2.7 -0.8 0.85)
    (2.95 -0.8 0.85)
    (2.95 -0.5 0.85)
    (2.7 -0.5 0.85)
);

blocks
(
    hex (0 1 2 3 4 5 6 7) air (60 60 60) simpleGrading (1 1 1)
)

And the last step consists in which commands are introduced in the splitMeshRegion line:


Old:
Code:
 splitMeshRegions -cellZones
This command splits all regions = all cellZones, incluiding domain0, domain1, ......domain2345

Solution:
Code:
 splitMeshRegions -cellZonesOnly
This command only splits the cellZones which are named by the user.


Using these steps, I haven seen the extra domains anymore.
I hope this explanation is useful for you.
Cagatayemre is offline   Reply With Quote

Reply

Tags
openfoam, snappyhexmesh

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
[mesh manipulation] why splitMeshRegions creates extra domains? skuznet OpenFOAM Meshing & Mesh Conversion 9 December 22, 2020 05:14
[Gmsh] gmshToFoam - Hybrid mesh conversion creates 2 regions bhanu2204 OpenFOAM Meshing & Mesh Conversion 5 February 18, 2018 08:04
[snappyHexMesh] Multi region meshing with SHM creates extra regions Dav3dum OpenFOAM Meshing & Mesh Conversion 0 August 8, 2016 09:54
MultiRegions: How are neighbouring domains coupled? Ivooo OpenFOAM Programming & Development 2 May 24, 2016 09:58
[snappyHexMesh] snappyHexMesh: extra domains domain1 domain2 ... appear skuznet OpenFOAM Meshing & Mesh Conversion 3 November 29, 2015 07:43


All times are GMT -4. The time now is 14:11.