CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Open Source Meshers: Gmsh, Netgen, CGNS, ...

2d mesh by salome

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

Like Tree3Likes
  • 1 Post By gschaider
  • 1 Post By startingWithCFD
  • 1 Post By startingWithCFD

Reply
 
LinkBack Thread Tools Display Modes
Old   May 16, 2009, 10:33
Default 2d mesh by salome
  #1
Member
 
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 8
mahaputra is on a distinguished road
Dear All


does anybody know, how to make a 2d mesh in Salome and can be recognized by OpenFOAM ?


many thanks
mahaputra is offline   Reply With Quote

Old   May 19, 2009, 18:17
Default
  #2
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by mahaputra View Post
does anybody know, how to make a 2d mesh in Salome and can be recognized by OpenFOAM ?
I assume that the converter (ideasUnvToFoam) fails. Probably (haven't checked) it doesn't support 2D-Meshes. The easiest thing (unless you want to rewrite the convert) is to extrude in Salome the mesh to a 3D-mesh that is 1 layer thick and export that. Just the thing the convert would do to get a Foamish 2D-mesh

Bernhard
nimasam likes this.
gschaider is offline   Reply With Quote

Old   May 20, 2009, 00:37
Default
  #3
Member
 
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 8
mahaputra is on a distinguished road
Quote:
Originally Posted by gschaider View Post
I assume that the converter (ideasUnvToFoam) fails. Probably (haven't checked) it doesn't support 2D-Meshes. The easiest thing (unless you want to rewrite the convert) is to extrude in Salome the mesh to a 3D-mesh that is 1 layer thick and export that. Just the thing the convert would do to get a Foamish 2D-mesh

Bernhard
Thanks Bernhard


so, could you please suggest me, some option to make a 2D mesh (exclude using blockMeshDict or any commercial software) ?

by the way, out of the topic, i have a problem related to dieselFoam, please spend a while your time to see my case in : Ammonium gas in the air

i really need some suggestion and help


Thousand Thanks


Nugroho Adi S
mahaputra is offline   Reply With Quote

Old   December 12, 2013, 15:45
Default
  #4
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
Quote:
Originally Posted by gschaider View Post
The easiest thing (unless you want to rewrite the convert) is to extrude in Salome the mesh to a 3D-mesh that is 1 layer thick and export that.
Dear Bernard

i follow this suggestion, now it can be converted with ideasUnvToFoam, but it returns patches as default faces and it can not recognize patches, do you have any idea how i can keep patches name in conversion from salome
__________________
Training Course on OpenFOAM at (http://www.isme.ir/)
My Weblog (http://openfoam.blogfa.com/)
nimasam is offline   Reply With Quote

Old   December 12, 2013, 18:25
Default
  #5
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by nimasam View Post
Dear Bernard

i follow this suggestion, now it can be converted with ideasUnvToFoam, but it returns patches as default faces and it can not recognize patches, do you have any idea how i can keep patches name in conversion from salome
Have you named the patches in Salome?
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   December 13, 2013, 03:10
Default
  #6
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
well, my steps in salome:
1- create 2D sketch
2-create face
3-explod face to edges
4-creates groups
5- mesh face (2D mesh)
6- extrude it
it fails to recognize my groups

then i changed my approach,
1- create 2D sketch
2-create face
3- extrude face to create volume
4- explode volume
6- create groups
7- create mesh
3D project with 2D-1D netgen element
but OpenFOAM can not recognize the elements

any idea how i can create one cell thickness for 2D simulation in OpenFOAM with Salome and with known patches ?
__________________
Training Course on OpenFOAM at (http://www.isme.ir/)
My Weblog (http://openfoam.blogfa.com/)
nimasam is offline   Reply With Quote

Old   December 13, 2013, 06:06
Default
  #7
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by nimasam View Post
well, my steps in salome:
1- create 2D sketch
2-create face
3-explod face to edges
4-creates groups
5- mesh face (2D mesh)
6- extrude it
it fails to recognize my groups

then i changed my approach,
1- create 2D sketch
2-create face
3- extrude face to create volume
4- explode volume
6- create groups
7- create mesh
3D project with 2D-1D netgen element
but OpenFOAM can not recognize the elements

any idea how i can create one cell thickness for 2D simulation in OpenFOAM with Salome and with known patches ?
If I remember it correctly you've got to create mesh groups or so (not sure of the nomenclature, don't want to start Salome and it is done in one of the basic tutorials on Salome anyway) from the geometry groups.
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   December 13, 2013, 12:11
Default
  #8
Member
 
Join Date: Nov 2012
Posts: 58
Rep Power: 4
startingWithCFD is on a distinguished road
Geometry module
1) create 2D sketch
2) create face
3) extrude face to create volume
4) use propagate on the extrusion (operations -> blocks -> propagate) to create groups ("compounds") of edges that have the same discretization
5) create face groups

Mesh module
6) create mesh for the extrusion
7) create a sub-mesh for the extrusion at the compound containing edges you want to discretize with only one interval. Algorithm: wire discretization. New hypothesis: nb. of segments = 1
8) compute the mesh
hsmao likes this.
startingWithCFD is offline   Reply With Quote

Old   December 13, 2013, 12:13
Default
  #9
Member
 
Join Date: Nov 2012
Posts: 58
Rep Power: 4
startingWithCFD is on a distinguished road
Sorry, forgot these last steps:
9) Right click on mesh, create group, face, group on geometry. Geometrical object: direct geometry selection and choose the groups on the geometry.
10) Right click on the mesh and export to UNV

That's all folks!
hsmao likes this.
startingWithCFD is offline   Reply With Quote

Old   June 11, 2014, 14:38
Default
  #10
New Member
 
Hann Mao
Join Date: Jul 2013
Posts: 2
Rep Power: 0
hsmao is on a distinguished road
Quote:
Originally Posted by startingWithCFD View Post
Geometry module
1) create 2D sketch
2) create face
3) extrude face to create volume
4) use propagate on the extrusion (operations -> blocks -> propagate) to create groups ("compounds") of edges that have the same discretization
5) create face groups

Mesh module
6) create mesh for the extrusion
7) create a sub-mesh for the extrusion at the compound containing edges you want to discretize with only one interval. Algorithm: wire discretization. New hypothesis: nb. of segments = 1
8) compute the mesh

Thanks! This worked perfectly.
hsmao 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
Dynamic Mesh Problem. Tom Clark FLUENT 9 July 7, 2010 07:56
virtual geometry richard FLUENT 4 January 7, 2009 06:16
2d irregular grid Remy Main CFD Forum 1 December 22, 2008 05:49
How to do Geometry from 3D mesh in ICEM San24 Main CFD Forum 4 August 8, 2005 02:49
General questions on grid-based computing Adrin Gharakhani Main CFD Forum 21 June 5, 2000 13:47


All times are GMT -4. The time now is 22:39.