I'm trying to run icoFoam on a
 

I'm trying to run icoFoam on a 2-D (1-cell thickness) mesh that was converted from a FLUENT case file. I ran checkMesh on the mesh and everything looked fine. The icoFoam keeps skipping the U (momentum equation) solving the pressure equation only. Has anyone had the same problem?

Sounds like the tolerance you
 

Sounds like the tolerance you specified for U is already met by the solution you start from.
Tighten the tolerance on U, and icoFoam will start solving for the momentum equations.

Thanks for your time. Even if
 

Thanks for your time. Even if it's the case, it should print out the residual info etc. I reduced the tolerance. Still, icoFoam doesn't solve the momentum equations.

I bet your front and back empt
 

I bet your front and back empty planes are bent. Run checkMesh from the dev version on it - you should get something like:

Checking geometry...
Boundary openness (8.47033e-18 -8.47033e-18 -4.51751e-17) OK.
This is a 2-D mesh
Domain bounding box: (0 0 0) (0.1 0.1 0.01)

(mine is a 2-D mesh).

Alternatively, replace the boundary condition on front and back from empty to symmetryPlane and see what happens. If it starts solving, your domain is bent (look at it sideways).

Please let me know,

Hrv

Hrv, Thanks for your time o
 

Hrv,

Thanks for your time on this. Changing empty type to symmetryPlane, OF indeed solves U.

Whn I did checkmesh, the only difference from yours is that it says

...
This is a 3-D mesh.

My colleague got this mesh by extruding 2-D mesh in Gridgen.

I see no sign of trouble at all. I seem to recall that OF once complained about "no solving direction ... (-1 -1 -1)" For this case, checkMesh doesn't say anything that indicates potential for troubles. iIt "silently" skips the momentum equations without any error message or warning at all.

The problem turned out to be t
 

The problem turned out to be the extrusion process done in Gridgen. The extrusion somehow created a conical section of the cylinder surface and one of the boundary thereforem got curved! When the 1-cell thick mesh is generated correctly, the problem went away. And the solver starts solving the momentum equations. Some osrt of warning message would be useful.