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

[ANSYS Meshing] Ansys Workbench 14.0 creating 2D axi-symmetric mesh

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

Like Tree1Likes
  • 1 Post By evcelica

Reply
 
LinkBack Thread Tools Display Modes
Old   February 19, 2013, 07:03
Default Ansys Workbench 14.0 creating 2D axi-symmetric mesh
  #1
New Member
 
Barry VRee
Join Date: Feb 2011
Posts: 2
Rep Power: 0
barryvree is on a distinguished road
Hi all,

Currently I am working on a problem involving rapid depressurization of CO2 in a pipe. This is clearly an axi-symmetric problem.
I would like to simmulate this problem using CFX. I know about the fact that CFX cannot handle truly 2d bodies and therefore I created a wedge of the pipe for meshing purposes.

However, in the ansys workbench 14.0 mesher, it is not possible to use the "extruded 2d mesh" functionality as a "mesh strategy".

How can I now create a mesh of this wedge of the pipe that has one element thickness?

Thanks in advance!
barryvree is offline   Reply With Quote

Old   February 19, 2013, 07:34
Default
  #2
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
I cannot recommend this technique.
If you really want only 1 cell along the wedge, the segment would have to be very thin (lets say <5°). This results in a cell with the same small angle at the center of your wedge.
For a decent mesh quality, an angle of at least 20° (better 30°) is required.

Either you choose a wedge with this angle and have lots of unnecessary cells or you use Fluent, which can handle real axisymmetric domains.
flotus1 is offline   Reply With Quote

Old   February 19, 2013, 07:53
Default
  #3
New Member
 
Barry VRee
Join Date: Feb 2011
Posts: 2
Rep Power: 0
barryvree is on a distinguished road
Thanks for your reply,

The reason I'm would like to use CFX is the fact that it contains CO2 in both gas and liquid form which is needed for my simulation of rapid depressurization when liquid CO2 will vaporize.
barryvree is offline   Reply With Quote

Old   March 9, 2013, 05:00
Default
  #4
New Member
 
Join Date: Mar 2013
Posts: 5
Rep Power: 4
flame_vivi is on a distinguished road
Hi,

I m doing combustion in a coaxial cylinder geometry and I m using CFX. I created a slice of 3°, but I have the same problem of you, in workbench 14. I'm struggling to create a single element through the thickness, "manually". Have you managed to find a solution for you prob?
thanks
flame_vivi is offline   Reply With Quote

Old   March 9, 2013, 05:22
Default
  #5
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Reading the posts in this thread again, you will see that a slice of 3° is not a good idea.
flotus1 is offline   Reply With Quote

Old   March 9, 2013, 05:55
Default
  #6
New Member
 
Join Date: Mar 2013
Posts: 5
Rep Power: 4
flame_vivi is on a distinguished road
Yes I guess so. I gota get started with a 2D simulation, or at least a quasi-2D, though, especially because the grid domain is quite big. So I was wondering how to handle 2D axial symmetric geometries in CFX.

thank you anyway
flame_vivi is offline   Reply With Quote

Old   March 9, 2013, 11:01
Default
  #7
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
The only thing you could do is to remove a part of the domain near the axis of rotation and put a symmetry boundary condition at the newly created face.
This prevents the problem with the sharp angle at the center.
Nevertheless, it also alters the shape of the fluid domain.

CFX is simply not the tool of choice for planar and axisymmetric problems.
flotus1 is offline   Reply With Quote

Old   March 11, 2013, 16:26
Default
  #8
New Member
 
Join Date: Mar 2013
Posts: 5
Rep Power: 4
flame_vivi is on a distinguished road
I agree. Thank you for the reply anyway.
flame_vivi is offline   Reply With Quote

Old   March 13, 2013, 16:44
Question
  #9
New Member
 
René
Join Date: Mar 2013
Location: Switzerland
Posts: 5
Rep Power: 4
rene78 is on a distinguished road
But imagine one still wants to create a mesh of 1 element thickness? I have the same problem as the original poster (me using V13). The function "extruded 2d mesh" doesn't seem to be available anymore.

Is there anybody, who could give me a hint on creating such a mesh?
rene78 is offline   Reply With Quote

Old   March 16, 2013, 02:58
Default
  #10
New Member
 
Join Date: Mar 2013
Posts: 5
Rep Power: 4
flame_vivi is on a distinguished road
hi rene,

I know small angles are not the best choice for a good quality mesh, but if you want to give it a try, go for a structured mesh. If you have the same number of nodes along the edges of your angle, you can be sure that there will be only one element through the thickness. CFX is not a 2D solver so the solution will be calculated on x,y,z anyway, but the fact that there is only one element on the third dimension, let you see the problem as 2 dimensional. I hope I ve been clear.
flame_vivi is offline   Reply With Quote

Old   April 26, 2013, 07:09
Default 2D analysis in CFX and Fluent
  #11
New Member
 
Namsu
Join Date: Jun 2011
Location: Neubiberg 85579, Munich, Germany
Posts: 4
Rep Power: 6
Usman15 is on a distinguished road
I am modeling turbulent non-premixed combustion in a Can Combustor with and without swirl induced recirculation zones. I am using use CFX and Fluent and comparing the results. For Flueut I have made a 2D grid while for CFX a thin wedge of 1 degree. I have following confusions:
· While making a thin wedge grid on ICEMCFD I gave rotational periodicity along the axis of rotation (Mesh→Global mesh parameters→Define periodicity→Rotational periodic). So that CFX take it as an axisymmetric problem. Then in CFX I am using symmetry BC for flow without swirl and periodic BC for flow with swirl. Is it the right approach? Or should I make the grid without rotational periodicity and then give the same BC in CFX?
· How can we apply periodic BC in CFX? Is it in domain interface?
· If in the third dimension instead of one cell I take two or more layers of cells, what effect will it have on the results?
Many Thanks in advance.
Usman15 is offline   Reply With Quote

Old   May 1, 2013, 23:43
Default
  #12
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 486
Rep Power: 9
evcelica is on a distinguished road
like Michelle Obama said, you can remove the central region of your mesh and use symmetry. If a small enough volume is removed it will not effect your solution.
flotus1 likes this.
evcelica is offline   Reply With Quote

Old   October 14, 2013, 02:40
Smile CFX can handle axisymmetric problems
  #13
New Member
 
Petr Jurcicek
Join Date: Feb 2010
Posts: 21
Rep Power: 7
Peter023 is on a distinguished road
Hi everyone,

according to my experience there is a way how to handle the axisymmetric simulation in CFX.

The geometry can be rotated as little as 1deg around its axis. In the ANSYS meshing tool, the necessary mesh smoothing is applied first and the meshing method is set to "sweep" (Mesh->Insert->Method) with manually specifying the two periodic boundaries (left, right). The number of divisions for the sweep method is 1. Its a good practice to name these two boundaries, e.g. symmetry_a, symmetry_b. Another named selection should be "axis" which is the geometry's axis :-)

In CFX then, the symmetry boundaries will be symmetry_a and symmetry_b. The rest of the setting is as usual. The quantities, e.g. mass flow will be 1/sweep angle of the real mass flow.

Note: Fluent loads pure 2D geometry but according to my knowledge, the geometry is "sweeped" or extruded in Fluent (1 deg) instead. Generally, the method used in fluent and CFX is analogical but Fluent makes it easier.

Hope this helps. Contact me in the case of any doubts, please. The above described method has only one disadvantage: the sweep meshing is awfully slow!!

Cheers,
Peter
Peter023 is offline   Reply With Quote

Reply

Tags
2-d, axisymmetric, co2, depressurization, mesh control

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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
[ANSYS Meshing] Multi-size mesh generation in ANSYS 12.1 Workbench nsakib520 ANSYS Meshing & Geometry 0 April 6, 2012 15:19
ansys imports icem-cfd ansys mesh adam2008 ANSYS Meshing & Geometry 0 March 5, 2011 09:40
2D mesh by ANSYS Workbench 8.1 Dome CFX 4 June 6, 2005 06:20
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 09:38


All times are GMT -4. The time now is 00:24.