CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Icem cfd aerofoil meshing (

cfd seeker February 2, 2012 13:04

Icem cfd aerofoil meshing
Hi all, I am facing problem in generating Unstructured Mesh of the aerofoil. After setting the parameters in "Part Mesh Setup" when i compute mesh on the surface, mesh goes through the aerofoil also. Kindly guide me through the proper steps for generating unstructured mesh on the aerofoil with prism layers and also having a density box.
Thanks in advance

cfd seeker February 3, 2012 11:12

any body who know about this, kindly reply here as I am really stuck up in this problem.

PSYMN February 4, 2012 16:10

Does mesh go "thru" the airfoil as if there is no boundary, or does the mesh go up to the airfoil and then there is also mesh inside the airfoil?

If the mesh is going thru the airfoil, then perhaps the curve is not part of the loop... Build topology to cut the surface with the curves.

If you just mean it is meshing inside the airfoil (as well as outside), then you have a decision... Do you want to model the solid (say for Conjugate heat transfer)? If not, then just delete the surface inside the airfoil. If yes, then just make sure that the surface inside is in a separate part so that you can apply solid properties to it...

cfd seeker February 6, 2012 09:55

Thanks for replying Simon. Actually there is a mesh inside the aerofoil and I have to analyze the aerofoil to find the aerodynamic coefficients, so in this case mesh inside the aerofoil is not required. I am new to ICEM and I am totally unaware of geometry(topology). In the present case I have two curves representing the upper and lower sides of aerofoil and large circle representing the Farfield around the aerofoil. I tried to build a surface using the curves of Farfield and Aerofoil but the created surface is also passing inside the aerofoil, so mesh is also formed inside aerofoil. Kindly guide me how to create a surface which forms outside the aerofoil and how to give Size function, create prism layers in 2D?
I know about the quad-meshing tutorials but I am interested in the Unstructured(tri mesh) mesh for my case. Thanks in advance and waiting for your reply.

PSYMN February 6, 2012 11:20

Just create a surface from the circle... It will pass thru the airfoil. You can put the surface in a new Part, perhaps named "FLUID".

Then Geometry (tab) => Geometry Repair => Build Diagnostic Topology. This will trim the surface with the airfoil curves and probably turn them red. You can then delete the surface within the airfoil.

For the unstructured patch conforming tri mesh you will need to set sizes on the curves. (under the mesh tab). When you set the sizes on the airfoil, you can set a number of layers, initial height and growth ratio...

Then surface mesh with patch conforming and you should be done (with boundary layers).

If you want a fancier boundary layer using the actual prism executable, you will need to turn on the advanced option for blayer2d. Search CFD online for that and I am sure you will find lots of posts...

If I were meshing this airfoil in a circle, I would use ICEM CFD Hexa. You can find a video about how to do that here...

diamondx February 7, 2012 15:34

I'm new to ICEM too, but i hope that you might find it useful.
The guy creates a mesh around aerofoil...

Far February 7, 2012 15:37

The name of that guy is PSYMN :rolleyes:

diamondx February 7, 2012 15:41

the guy's name "Simon Pereira"

cfd seeker February 8, 2012 04:51

your guidance help me a lot,thanks a lot. I have manged to have a surface outside aerofoil and also able to mesh it,I have also applied the prism layers but prism near the trailing edge is not respecting the geometry of aerofoil rather it is passing inside it, I have also increased the no. of nodes on the aerofoil curves but all in vein, so kindly tell me how to tackle this problem? Secondly I am interested in applying a density region on the upper surafce of aerofoil to capture the separation at higher angle of attacks but the mesh is not taking that density region into consideration( mesh forms as without the density box), what's the problem here? what mistake I am making in applying density box. I have build the density box using the four created points other than the aerofoil.

PSYMN February 8, 2012 21:39

The density box only works with the octree or delaunay tetra meshers...

MultiZone does not respect it (yet).

Not sure about your other issue... Maybe a picture...

All times are GMT -4. The time now is 05:23.