[barryvree]

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!

[flotus1]

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.

[barryvree]

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.

[flame_vivi]

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

[flotus1]

Reading the posts in this thread again, you will see that a slice of 3° is not a good idea.

[flame_vivi]

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

[flotus1]

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.

[flame_vivi]

I agree. Thank you for the reply anyway.

[rene78]

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?

[flame_vivi]

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.

[Usman15]

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.

[evcelica]

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.

[Peter023]

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