CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   2D mesh in ANSYS 10.0 Workbench (http://www.cfd-online.com/Forums/cfx/22560-2d-mesh-ansys-10-0-workbench.html)

Frank Peters May 16, 2006 11:53

2D mesh in ANSYS 10.0 Workbench
 
I am using ANSYS workbench 10.0.

According to the help-file it should be possible to perform a 2D model:

Cite: "You can configure Workbench for a 2-D simulation by first creating or opening a surface model in DesignModeler, or in any supported CAD system that has provisions for surface bodies (Autodesk Mechanical Desktop and Autodesk Inventor do not support surface bodies). The model must be in the x-y plane. 2-D planar bodies are supported, 2-D wire bodies are not. Then, on the Project Page, choose 2-D in the Analysis Type drop-down menu located under Advanced Geometry Defaults, and attach the model into Simulation. You can specify a 2-D simulation only when you attach the model. After attaching, you cannot change from a 2-D simulation to a 3-D simulation or vice versa."

I have created a 2D surface model and followed the directions. Then when I create the mesh using CFX-Mesh I get: "CFX-Mesh can only operate on Solid Volumes! Please ensure that atleast one unsurepressed Solid is available."

I tried several things but can not create a 2D problem. Please, can someone help me?

Regards, Frank.

Glenn Horrocks May 16, 2006 18:42

Re: 2D mesh in ANSYS 10.0 Workbench
 
Hi,

To generate a 2D mesh you need to draw the geometry in the xy plane and then extrude it in the z direction (or rotate it about the x axis if axisymmetric). Set the number of elements to extrude to 1. You can then mesh the 2D surface with a mesh which is 1 element thick.

Glenn Horrocks

Frank Peters May 17, 2006 04:41

Re: 2D mesh in ANSYS 10.0 Workbench
 
Dear Glenn,

Thanks for your response. I tried this before and tried it again just now, but failed.

I feel the difficulty comes from the fact that in Workbench the generation of the geometry and of the mesh are split.

If I extrude the xy-geomemtry in the z-direction, what happens, if I set Analysis Type 2-D in the Advanced Geometry Defaults and start "Generate CFX Mesh", is that I get the error: "No valid bodies found"

There is no problem if I use Analysis Type 3-D. Then CFX-Mesh starts okay. The problem with this is, however, that CFX-Mesh seems to use tetrahedrals only. Generating one layer of thetrahedrals (and imposing periodic boundary conditions in that direction seems hard to me).

Regards, Frank.

Glenn Horrocks May 17, 2006 18:21

Re: 2D mesh in ANSYS 10.0 Workbench
 
Hi,

Do not select 2D under advanced geometry defaults. As I said, you need to generate a 3D body by extruding or rotating a short distance. In CFX-Mesh set the meshing option to 2D extruded and set the top and bottom surfaces to the extruded pair. Done it many times, it works fine and generates a hex/prism mesh (extruded quads are hexes and tris give prisms).

Glenn Horrocks

Frank Peters May 18, 2006 04:36

Re: 2D mesh in ANSYS 10.0 Workbench
 
Dear Glenn,

Thanks a lot. I did it!

I am new at CFX and this was not immediatley obvious for me fom the help.

Regards, Frank.


All times are GMT -4. The time now is 23:56.