CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   2d mesh in ansys 12.0 (

sairam March 3, 2010 13:48

2d mesh in ansys 12.0
hello everyone i have a problem in moving the part from geometry to mesh can anyone help me in this. i have a 2d part and i'm unable to see it in mesh section, its telling that unable to attach geometry file, as i said u its not a soild its just a 2d part, and its showing a message as "No valid bodies found" in meshing. Any help would be nice thank you in advance

wadebogs March 3, 2010 17:11

This error generally comes up when reading 2D or 3D geom into 3D or 2D respectively. (not sure why they don't have better error messages :D)

You need to make sure the geometry options in workbench are set to 2D. You can do this via workbench options or by clicking on the geometry part of the Workbench schematic.

Make sure you have surface bodies as well in Design Modeler - if you have sketches you can use concept -> surfaces from sketches to create the surface body.

Oh, and as always with Fluent you have to have the geometry on the xy plane (z=0).

If this doesn't work start again from scratch and ensure 2D options are used from the start.

Good luck! ;)

CorranChetano March 10, 2010 22:41

2D mesh does not work
I am trying to set up a 2D axis symmetric test case with three domains (fluid domain and 2 different wall domains).
I was used to the old combination of Gambit and Fluent and now have to get used to the new ANSYS 12.0 workbench. The transition, though, turns out to be harder than I initially thought.

In order to set up the 2D mesh I tried what is mentioned above, but that did not work. I was told once that you actually have to create a 3D object (the anticipated 2D cross section with depth 1) and then go on and mesh. But that is not working either as I am not able to specify my three separate domains, the DesignModeler always merges my objects together as one body (and the add new body button is not usaable either). Can somebody please enlighten me as to what I am doing wrong, or if this is just not the way to do it.

I know that this all sounds rather basic, but the beginner tutorials provided by ANSYS do not really help. If sb knows a better source to get started, that would help, too. Thank you a lot in advance!


RossFS March 13, 2010 22:30

I've recently been trying to do something similar to you, CorranChetano, and the only way I've been getting it to work is to generate the different areas in some CAD software. One part for fluid and two parts for solids (one solid above and below the fluid). The parts are made quite thin (as thin as your smallest element so that the meshing software only goes 1 element deep into your 2D model)

I then assembled the parts together in the CAD software and saved it as an IGES file. I import this in via geometry and suppress the solid sections when in there. Something else I did at one point to get it going was to add some "Connections" (when doing the meshing) between the solid and fluid (where they touch).

I end up just having the fluid section meshed (due to the suppression of the solid sections) and setting up the walls via boundary conditions in the setup section.

CorranChetano March 16, 2010 06:17

Thank you very much for this hint, but is there no "native" (meaning implemented in DesignModeler) way to introduce several computational domains (liquid and solid)?

PSYMN April 21, 2010 17:57

Mixed Dimension...
Liquid and solid is not the problem... (You can have multiple bodies and define any of them as Solid or Liquid. If they are separate parts, they will be meshed separatey, but if you put them into a multibody part, they will be meshed with conformal mesh).

The problem is more with mixed dimesion models... 2D and 3D parts together. There are special settings to handle this configuration at 12.1. And now at 13.0, you can handle mixed dimension parts...


Jallen13a October 6, 2010 14:30


Originally Posted by CorranChetano (Post 250209)
Thank you very much for this hint, but is there no "native" (meaning implemented in DesignModeler) way to introduce several computational domains (liquid and solid)?

Corran, I am rather new to Fluent but think I may be able to help. While it may be easier to use other CAD software you can use DesignModeler for simple geometries. Once you already have your liquid or solid defined in DesignModeler and want to add the other one, you will have to do a second extrusion. To keep this extrusion from being combined to the already defined body you want to change "Operation" to "Add Frozen." This should keep the new body separate from what you already have. When you select each body on your model view, you can select whether you want each body to be a solid or fluid.

This should leave you with multiple bodies, where each one is defined as a solid or fluid. If you want a conformal mesh you'll want to highlight all the bodies, right click and "form new part" so that you'll have a multi-body part, rather than multiple parts (which would lead to non-conformal meshes)

PSYMN October 6, 2010 17:33

Named Selections
Right Jeremy,

And on top of that, you may want to put each body in a named selection so they appear as named regions in Fluent (FLUID, POROUS, FLUID2, SOLID, etc.)

Wait August 3, 2011 22:47

thank you!
"you have sketches you can use concept -> surfaces from sketches to create the surface body."

Thank you very much! you solve my question.:)

All times are GMT -4. The time now is 03:06.