CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Mesh Generation & Pre-Processing Software > ANSA

2D-Mesh with blocking? possible?

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

Like Tree1Likes
  • 1 Post By The_Kaiser

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 24, 2016, 05:15
Default 2D-Mesh with blocking? possible?
  #1
New Member
 
Join Date: Mar 2016
Posts: 29
Rep Power: 8
The_Kaiser is on a distinguished road
Hey,

I tried to do a blocking of my 2D Geometry with HEXA_BLOCK. Unfortunately, I get only 3D hexa blocks (I know, I know, a hexa is 3D. But I hoped to get sth 2D). I want to do it in 2D, to easily vary the thickness and number of elements in the third dimesnion with the TRANSLATE option. (want to use it in OpenFOAM, unstationary simulation). Is it possible to do somehow a blocking of a 2D geometry? Maybe splitting the sourface in "blocks" in my CAD-program, then mesh it with ANSA? Could this work?

Thanks in advance

Last edited by The_Kaiser; October 24, 2016 at 07:23. Reason: idea for solving
The_Kaiser is offline   Reply With Quote

Old   October 24, 2016, 08:28
Default
  #2
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 286
Rep Power: 19
vangelis is on a distinguished road
Hi there,

Indeed ANSA hexablock is meant for 3D meshing.

You could of course create these Boxes and only mesh one of their facets only, but I think this is not an efficient approach.

I would therefore recommend that you work on the level of geometry in xy plane, and with CUT operations, cut parallelogram patches that you can mesh with MAP QUAD mesh. The functions that you should use for meshing are then:

Perimeters>Length, Number and Spacing
Have also in mind the function Perimeters Align, which can be used to "copy" a distribution from one perimeter to another.

After meshing all macros with map quad mesh, you can, as you write, use Volumes>Extrude>translate in z coordinate and create one cell thickness for OpenFOAM 2D.

Remember to use Elements>Vol2Shell>Skin to create shell mesh in the free exposed facets of the created hexa mesh, so that you can assign BCs on them

Hope this helps

Vangelis
vangelis is offline   Reply With Quote

Old   October 25, 2016, 10:17
Default
  #3
New Member
 
Join Date: Mar 2016
Posts: 29
Rep Power: 8
The_Kaiser is on a distinguished road
Hey,

Thanks for the advise, it works fine so far!

A problem comes after using Elements>Vol2Shell>Skin. I get the shell, but the problem is, every mesh element gave me 1 face. So when I have over a milion faces, it's kinda impossible to assign the boundary conditions... Help again please?
The_Kaiser is offline   Reply With Quote

Old   October 25, 2016, 10:50
Default
  #4
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 286
Rep Power: 19
vangelis is on a distinguished road
I forgot to mention that for quick selection you should activate the Feature Angle selection tool at the bottom centre of ANSA GUI next to ENT and PID selection. In this way with one click you can pick a whole area within the user specified feature angle (by default 40deg)
Vangelis
vangelis is offline   Reply With Quote

Old   October 28, 2016, 06:46
Default
  #5
New Member
 
Join Date: Mar 2016
Posts: 29
Rep Power: 8
The_Kaiser is on a distinguished road
Works so good. You are like a magician Thanks
vangelis likes this.
The_Kaiser is offline   Reply With Quote

Reply

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
[snappyHexMesh] SHM problem : KVLCC2 with appendage mesh sc.park OpenFOAM Meshing & Mesh Conversion 1 March 13, 2016 14:28
[mesh manipulation] Importing Multiple Meshes thomasnwalshiii OpenFOAM Meshing & Mesh Conversion 18 December 19, 2015 19:57
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 07:42
[ICEM] Problem making structured mesh on a surface froztbear ANSYS Meshing & Geometry 4 November 10, 2011 09:52
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55


All times are GMT -4. The time now is 06:53.