creating groups of faces for openfoam boundary conditions

You can achieve what you want if you create an extrusion mesh.

Try do the following:
1) Create a volume by extrusion of your 2D domain (face => volume) in the Geometry module, define group of faces for boundary conditions: inlet, outlet, wall, symm. You will also need a group of all edges in the "extrusion" direction (=side edges = the edges on which you want only 1 element) and a group of faces corresponding to your initial face (=the source face) and a second group of faces corresponding to its "translated image" after extrusion (the "destination" face).
2) In Mesh module: create a mesh with:
- 1D algo=Wire discretization, 1D hypothesis: average length (=global mesh size)
- 2D algo=quadrangle
- 3D algo=extrusion
validate but do not compute mesh yet : it will fail.
3) Create a submesh on the "side edges":
- 1D algo = Wire discretization, hypothesis: number of element = 1
4) if you want, create submeshes to define refinements on the edges of your "source face"
5) Create a submesh on your "source" face:
- 2D algo = triangle or Netgen 2D
6) Create a submesh on your "destination" face
-2D algo = projection 2D, hypothesis: select the "Source" of the projection = your "source face", leave the rest empty.

Now you should be able to compute the mesh without error. Extrusion meshing is a bit tedious, but it should always work when :
1) the "source" and "destination" 2D face mesh are identical
2) the "side" faces are meshed with a structured grid of quadrangles (= side faces must have exactly 4 edges!)

You can find also a tutorial on the wiki: www.caelinux.org/wiki/index.php/Doc:CAET...nd_Extrusion_meshing