CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Boundary conditions problem in ICEM and Fluent (

Far December 6, 2011 03:43

Boundary conditions problem in ICEM and Fluent
4 Attachment(s)
Dear all

I am trying to solve the problem of heat transfer from turbine rotor to cooling flow coming from compressor. So inlet is the cooling air and outlet is the air to turbine section. please refer to second Fig.

I have defined the boundary conditions as shown in Fig. 2 and defined them in ICEM BC panel as shown in Fig. 3.

My problem is that we I open this mesh file into fluent I only get the axis, rotor (wall), stator (wall) and stator shroud (wall) boundary conditions in Fluent. I tried many times but I am unable to get the inlet, outlet and rotor shroud boundary conditions in Fluent.

Any suggestion ?

PSYMN December 9, 2011 12:34

No line elements in those parts...
Here is my guess...

The Bocos that you setup in ICEM CFD are based on the part names... They don't necessarily require you to have mesh in those parts, but only an entity such as a curve or point. This is so that you can set up the Boundary Conditions even before your mesh is generated. However, the boundary conditions do need to be applied to the mesh during output. If there is no mesh in a particular part, there is nothing to carry the boco out to Fluent.

I am guessing that if you turn off your geometry in ICEM CFD and just try to display your mesh in those parts (inlet and outlet) you won't have any. Optionally, you could try mesh info and see if any elements show in those parts...

If you want mesh in those parts, you will need to ensure that the related edges (I am assuming this is a 2D Hexa blocking) are associated to those curves. Also, if you have an edge that is spanning across parts, you will need to split that edge (or split the block) so that you can associate each edge segment to the correct curve.

Once you have line elements generated in the INLET and OUTLET parts, the output interface will be able to assign the boundary conditions and you will find them in FLUENT.

Best regards,


Far December 9, 2011 12:48

1 Attachment(s)
Dear Simon thank-you for your help. I have also attached the ICEM files for your reference, meanwhile I am trying your suggestions

PSYMN December 12, 2011 16:23

Right, so these files confirmed my theory...

Better than edge splits, i suggest you could just split the whole block, end to end, twice and then associate the middle segment with the inlet/outlet.... The advantage of this method (over edge splits) is that it gives you actual verticies that you can more easily (and precisely) associate to the specific points at the ends of the "openings"...

I should also note, that as your model currently stands, you only have very few elements across the inlet/outlet... make sure to put in at least 9, but probably more. Also the jump between the mesh size on the outlet edge and the mesh size of the adjacent element projected to the wall should be closer if you want to avoid convergence problems, use match edges...

Far December 16, 2011 12:30

Yeah Simon you are 100% correct. Thank-you for your help

I tried all your suggestions and they did the magic. I have got very good convergence and results with V2F, SST , Reynolds stress model and low Reynolds number K-Epsilon models for my heat transfer calculations.

Again I thank-you for your time and help

Crank-Shaft March 11, 2014 01:32

Hey Simon and Sijal,

It was interesting reading your comments above since I have a few issues myself with missing BCs in an exported mesh from ICEM.

It is simply a cube which is 200x100x100 (LxHxW) which is simply there to trial various methods of mesh export out to fluent solver. If the 'inlet' and 'outlet' BCs are actually assigned to the respective surfaces and there is clearly mesh on those surfaces (when turning them on and off), doesn't that mean that the BC, surface and the part is properly associated with the mesh?

Crank-Shaft September 10, 2014 19:48

5 Attachment(s)
Hello everyone,

I know this is reviving a very old thread, but I believe my concerns and questions are similar to save us starting yet another thread.

I've tried to block and mesh a very simple geometry - A uniform backward facing step - for validation of a turbulence modelling approach that I've been developing.

The first block (130 m long, adjacent to inlet) needs to have an BCSubsonicInlet at the front, then BCSymmetricPlanar at the sides. Both of these seem to be operating fine and is correctly identified in the CGNS output and my solver (

However, the top and bottom surfaces needs to have a BCSymmetricPlanar applied prior to the start of the BCViscousWall. In order to replicate the original configuration (backstep_bcs.jpg and backstep_mesh.jpg) I decided not to split the block further at this point and this also helps preserve node distribution. Unfortunately, this also means that the actual surface is only being associated with the mesh and BCViscousWall. The image attached (NotTakingSymmetry.png) is my wall proximity function and this reveals that the entire surface is detected as a BCWallViscous.

The BCSymmetricPlanar and the extended surface isn't being associated with any output mesh (ICEMCurrent.jpg and ICEMCurrent2.jpg). Is there a way to apply this BC without having an additional split in the block?

Thanks in advance for any suggestions you may have.

All times are GMT -4. The time now is 19:40.