|
[Sponsors] |
May 16, 2009, 10:33 |
2d mesh by salome
|
#1 |
Member
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 17 |
Dear All
does anybody know, how to make a 2d mesh in Salome and can be recognized by OpenFOAM ? many thanks |
|
May 19, 2009, 18:17 |
|
#2 | |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Quote:
Bernhard |
||
May 20, 2009, 00:37 |
|
#3 | |
Member
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 17 |
Quote:
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 : http://www.cfd-online.com/Forums/ope...tml#post216606 i really need some suggestion and help Thousand Thanks Nugroho Adi S |
||
December 12, 2013, 14:45 |
|
#4 | |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 24 |
Quote:
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
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
||
December 12, 2013, 17:25 |
|
#5 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
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 |
|
December 13, 2013, 02:10 |
|
#6 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 24 |
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 ?
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
December 13, 2013, 05:06 |
|
#7 | |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Quote:
__________________
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 |
||
December 13, 2013, 11:11 |
|
#8 |
Member
Join Date: Nov 2012
Posts: 58
Rep Power: 13 |
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 |
|
December 13, 2013, 11:13 |
|
#9 |
Member
Join Date: Nov 2012
Posts: 58
Rep Power: 13 |
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! |
|
June 11, 2014, 14:38 |
|
#10 | |
New Member
Hann Mao
Join Date: Jul 2013
Posts: 2
Rep Power: 0 |
Quote:
Thanks! This worked perfectly. |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
decomposePar problem: Cell 0contains face labels out of range | vaina74 | OpenFOAM Pre-Processing | 37 | July 20, 2020 05:38 |
Salome cgns format mesh to SU2 | JPBLourenco | SU2 | 19 | November 18, 2019 02:11 |
[Other] conformed FSI mesh for unstructured fluid region | ashish.svm | OpenFOAM Meshing & Mesh Conversion | 10 | August 2, 2019 08:40 |
[snappyHexMesh] Creating multiple multiple cell zones with snappyHexMesh - a newbie in deep water! | divergence | OpenFOAM Meshing & Mesh Conversion | 0 | January 23, 2019 04:17 |
Converting Salome hybrid mesh to OpenFOAM | Arnoldinho | OpenFOAM | 4 | March 28, 2012 10:24 |