Hi,I want to build a 2D model in CFX 10.0 on the x-y plane. I know I have to set only one element thick on the z direction and think it as a 2D model,but I dont know how. Shoud I do the thickness setting in ICEM or in CFX? and please tell me how, thank you!

Using ICEM, make your 2D mesh. Then go to the Edit Mesh tab and select the Extrude Mesh icon. Choose 1 for number of layers.

Once that's done export to CFX5 format.

Thank you very much for your reply, Andrew. I have tried, but I found that in the Edit Mesh tab there are many icons with the Extrude Mesh icon not included. I dont know what causes the problem, could you please give me some advice? thank you!

What version of ICEM are you using? I have ICEM CFD version 11.0. In this version, Extrude Mesh is the second item from the left under the Edit Mesh tab.

The ICEM version I'm using is 10.0, and I couldn't find the Extrude Mesh icon in the Edit Mesh tab. I really wonder what is the problem with my software. Thank you, Andrew.

Search the help file for Extrude Mesh. It may help you to locate this feature.

The help file is typically located in: [icem install path]\docu\icemcfd_help.chm

Replace [icem install path] with your installation directory (C:\Program Files\ANSYS Inc\v100\icemcfd or whatever it is)

The ICEM version I'm using is 10.0, and I couldn't find the Extrude Mesh icon in the Edit Mesh tab. I really wonder what is the problem with my software. Thank you, Andrew.

ICEM!

Make sure your version of ICEM can even create HEX elements. Depending on licensing, ICEM can be pretty crippled, which could explain your lack of the extrude mesh icon. You may be better off creating a mesh in ANSYS Workbench if you have it.

Thank you all very much. That's pretty funny and embarrased that I found the Extrude Mesh icon in the Mesh tab rather than in the Edit Mesh tab. After I succeeded in extruding the mesh for 1 element thick, I found it a little unconvenient to define new parts, as I need to define inlet,outlet,front,back,top and bottom for the very simple retangular 2D problem I have set. I just can't directly select the region I want to define as a part. I have to use the "creat part in region" function,and provide the Min and Max X,Y,Z coordinates that represents the region I want to define. I dont know if it is a normal way to define new parts that you may use in the later CFX boundary setting.If you have any more cute way for this problem,please tell me. Thank you.

When you extrude the mesh there are options for "Side Part", "Top Part", and "Volume Part". These can help you assign mesh elements to families. I've never done a 2D simulation, so I'm not sure the best way to assign family names. Did you assign your curves to families before creating the 2D mesh? I would think that it'd be smart enough to assign shell elements to the curves' families.

Hi Jaloa,

ICEM CFD is overkill for this kind of thing. Have you looked at doing it in the Workbench Meshing application?

-CycLone

Thank you,Andrew. I've paid attention to the options for "Side Part", "Top Part", and "Volume Part", and I have tried to name them separately as "side","top" and "duct". Just like what I mentioned before, to make it really simple,my geometry is a rectangle in x-y plane(the picutre link is http://www.sigmirror.com/files/1827_ckxfm/before%20Extruding.bmp), and after Extruding the mesh, the mesh became a flat hexahedron, with the size 50*10*1(x*y*z),while the geometry is still a rectangle in x-y plane with the size 50*10(x*y). The "side" part(In the new GUI,family is called as part instead) turned out to be including four regions，left "side", right "side",up "side" and down "side", as I indicated in the picture(the picture link is http://www.sigmirror.com/files/1828_qgnvx/after%20Extruding.bmp). I wanted to set the left one "inlet",the right one as "outlet", the up one as "top", and the down one as "bottom". Still, I want to set the "top" part(indicated in the picture) as "front". Once done, I could set boundary conditions easily in CFX for each parts. I'm sorry that I don't quite understand about the assign work you suggested. I just think maybe you can tell from the picture what I should do for better. Thanks again.

Hi,Robin. I've also tried to solve the problem in ANSYS Workbench. But do you mean I have to first draw a 3D geomtry with the Model Designer,or just draw a 2D geometry in it, and then export them into "CFX Mesh" for mesh extruding and region defining? By the way,the Workbench I'm using is a 10.0 version, which includes five models,"Geometry","Advanced Meshing","CFX-Mesh","Empty Project" and "Advanced CFD".

Before you create the mesh, do this:

1. Create 4 curves at the edges of your plane. 2. Assign each curve to a different part family. Call them TOP, BOTTOM, INLET, and OUTLET. 3. Create a surface based on the curves. Call it FRONT. 4. Create a surface mesh based on the geometry, leaving the part name "inherited". The surface mesh will be assigned to the part FRONT. 5. Click on the extrude button. In the "side part name" box, leave "inherited". In the "top part name" put BACK. In the volume part name you can put a name for the fluid domain.

Each of the side parts will take the name of the edge it was extruded from, so you will have TOP, BOTTOM, INLET, and OUTLET surfaces.

I hope that helps.

I think I have an idea of what you might be doing wrong since I had a similar problem in the beginning. Here are the steps you should follow if you're doing an hexa mesh:

1- Create a 2D geometry (for the example, let's say you create a rectangle)

2- Name the 4 curves and the created plane by putting the into 5 distinct parts: Inlet, Outlet, Top, Bottom and Symmetry_Plane_1

3- Create your 2D blocking.

4- *** Be sure to associate the block's edges and faces to the corresponding geometry ***

5- Extrude your mesh leaving the sides' names as "inherited" and name the top "Symmetry_Plane_2"

This should work. Step 4 is essential to have the rignt names at the right places when working with blocks.

If you are extruding an unstructured (i.e. triangular) mesh, be sure to name the edges before creating the surface mesh.

Hope this helps,

Felix

Thank you very much,Andrew, I have solved my problem according to your suggestions.

Thanks a lot,Felix,you and Andrew really helped me,I appreciate it very much.