How I could import Ansys mesh into CFX?
 

Dears,

I wanna import ansys mesh into CFX (I have ansys 12). I can import the mesh, but I can't define the boundary condition, because CFX consider whole geometry as a block. Could u plz help me?

m.shahverdi@gmail.com

Does it gives you access to primitive 2d & 3D regions? What happens when you click on "..." symbol next to location under Basics settings. If there are primitive regions listed there you can group them together to define BCs.

Good luck,
Sandeep

Dear Rana,

When I import the mesh into CFX, I have only a rigid bosy and for BCD definition, there is only 2D premetive, so I can't define BCD on each face.

Thank you

That's all you need. BCs are specified on 2D faces. identify the 2D region where you want to apply bc and group them by holding Ctrl key.

Sandeep

P.S. Rana is my last name :)

OK, but the problem is that I should separate the surface at first. because each of them should be set separately as BC (e.g. wall, inlet, ...).
If you let me have your email, I can submit the mesh file to you. I would highly appreciated if you could take a look and help me.

m.shahverdi@gmail.com

Named Selections
 

You need to break up the model into Named selections before you output it from ANSYS Meshing. If it is a 3D model, then you name the faces (inlet, outlet, etc.) If it is a 2D model, you name the perimeter edges. Similarly you can select and put the volumes or (or 2D surfaces) into a named selection such as "FLUID".

To to it, use the selection tool to select the entities and then right click to create a "named Selection". Give it a name and generate it. Then move on to the next one.

Once this is done, recompute the mesh and output it again. Each named selection will appear as separate and nicely selectable boco region in CFD.

I think there is a manual way to select clumps of shell or line elements in CFX Pre and put them into separate boundaries, but I never do it that way.

If you mean "ANSYS Classic" as your mesh generator, then do the same thing with "nodal components"...

The CFX-Pre User's Guide has a note about having to use named components of 2D MESH200 elements to create defined regions when importing an ANSYS CDB mesh into CFX (// CFX-Pre User's Guide // 9. Importing and Transforming Meshes // 9.1. Importing Meshes // 9.1.3. Supported Mesh File Types).

This is slightly misleading. For my purposes, I needed to delete all 2D meshes and instead create named nodal components on my boundary surfaces. A good tutorial can be found in "ANSYS CFX: Importing Meshes into CFX," J. Luis Rosales, The Focus, Issue 52, PADT Inc., October 6, 2006. (http://www.padtinc.com/epubs/focus/2...heFocus_52.pdf)

Hope this might save someone some time down the road as it did me.

Hello!
I have a similar problem: I want to import a geometry from classic to workbench respectively Fluent and generate the mesh there. I created named selections (in Classic called components) and exported it as an igs/Iges file. All I get is the area, but not the lines, contruction points and not the components if I open it in the design modeler... I got this error message Attachment 24269
I tried it with ALLSEL as told in the error message but still, no lines and no components... What do I have to do do receive all my lines, cpoints etc. I created in Classic?
Thanks for your help!