CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   2D channel mesh (

danillocafaldo July 29, 2010 22:33

2D channel mesh

I need to simulate a very simple 2D geometry in CFX (a retangular channel) using the Workbench-mesh to generate the mesh.

I used the mesh control with the option "ALL QUAD" to have retangles and in the sizing options I can control the element size, so I control the number of elements.

The problem is that I don't know how to force one direction to have just one element.

Could anyone help me?


PSYMN July 30, 2010 08:57

Do you mean you want to make it 1 element thick (two and a half dimensions) because CFX doesn't actually handle 2D?

For a while now, CFX has been taking in a 2D model in Fluent Format and converting it automatically. I have not done that with an ANSYS Meshing mesh thru the workbench schematic yet though. Ask about that in the solver forum.

If that is not your question, a pic would help.

danillocafaldo July 30, 2010 10:50

Thank you PSYMN for your answer.

Yes, it's that what I want.

I want to simulate the vortices in a mixing layer 2D with a tangent hiperbolic initial condition.
So, I need a mesh like that
The mesh that I did (just to learn how to generate a mesh like that) in the Workbench meshing:
But I can't control very well this mesh, when I refine it appears another element in the 3rd direction.

I don't know if I'm doing the correct way.

I will take a look in what you said.

Thank you


charlotte July 30, 2010 11:15

When you are in the Mesh program, right-click on the mesh icon and choose "insert/Method". Choose the geometry, in the "method" case, choose "Sweep" instead of "Automatic".
Then you use the following options:
Free Face Mesh Type: All Quad
Type: Number of Divisions
Sweep Num Divs: 1

If you have an error or it doesn't sweep in the desired direction, choose manually the source and target face:
Src/Trg Selection: Manual Source and Target.

There are some very good meshing tutorials on ANSYS customer portal... I'd recommend to do them: it takes a couple of hours and it will speed up your learning curve.



PSYMN July 30, 2010 13:51

If you have access to ICEM CFD, that would be the easiest way to generate this mesh, I could outline those steps if you needed them.

If you are doing it in ANSYS Meshing with the sweep option that Charlotte suggested, you will need to make sure your model is 3D (extrude the geometry in DM or your cad system first). You will then need to control the distribution along the edges. You will probably also need to set the source face to "mapped"...

danillocafaldo July 30, 2010 18:28

Thank you charlotte and PSYMN.

Charlotte: I followed these steps and it worked perfectly. Ok, I will try some tutorials at the custumer portal.

PSYMN: I've read that ICEM could do this in a easier way, but for now I need to use the Workbench Meshing. Probaly I will have acces to it soon.

Thank you again


All times are GMT -4. The time now is 13:38.