CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Free mesh control (

Rhyno466 September 20, 2011 21:17

Free mesh control
2 Attachment(s)
I am working with an airfoil with a structured mesh area around the airfoil and and unstructured (free) mesh throughout the rest of the domain. I have used ICEM to do fully structured airfoil meshes in the past with great success, but the current research (for my MS thesis) requires many meshes to be created for a quasi- steady state analysis and I am required (advised) to use the current hybrid mesh setup.

I am struggling to resolve the wake area with enough resolution, and cannot figure out a good way to increase the mesh density where I need to. It seems that the expansion ratio of the cells is too high and thus the cells increase in size too rapidly for my liking.

I am looking for help and ideas to be able to increase the density of the wake area. I have already tried increasing the edge spacing with minimal luck. I have also have zero success using the refinement function but is more then likely user error. Thanks!

BrolY September 21, 2011 03:57

Did you try mesh density boxes ?

Rhyno466 September 21, 2011 11:34

Thanks, this seems to be what I am looking for except that I am using blocking in order to get my structured boundary layer area. I dont think this mesh density function works with what I am doing currently. I dont even know how to mesh an airfoil without using a blocking scheme.

BrolY September 21, 2011 11:49

Density boxes work only with tetra mesh.

For the blocking, you can't use that function, but you have the edge parameters to help you. The bad thing is that it will propagate the refinement to the parallel edges. Another solution : create two topologies and make a non conformal merge (I think ICEM can handle only conformal merge, so you will need to do that with your solver software).

To create unstructured mesh is very easy with ICEM. Make a build topology of your domain. Check if your geometry is ok. Specified your maximal length in the mesh part parameters. Create a patch independent mesh (octree) of your domain. Delete the volume mesh. Smooth the surface mesh. Create a Delaunay (for example) volume mesh (based on the existing mesh). Smooth. Create your prism layers and that's good.
There are a lot of topics dealing with this method on this forum if you want ;)

PSYMN September 21, 2011 14:52

The paving algorithm needs an edge to control the mesh size locally.

You can give it one by splitting the unstructured block from the trailing edge to the middle of the outlet. Then setup a biased edge distribution...

This edge distribution won't propagate across an unstructured block, it will just control the mesh size on that edge of the loop and allow you to transition your mesh much better.

Rhyno466 September 23, 2011 15:55

OK, thanks! If edges control mesh size locally, what controls the global mesh sizing. As in how does it determine the maximum size that the cells grow to, and how fast they do grow to this maximum size?

PSYMN September 25, 2011 18:42

For that mesher (Patch Dependent Surface Meshing), you can set sizes on all the curves at once (global size), or set by part name or by individual curves...

You can also set sizes on Surfaces, there is an option to use these "surface" sizes and have the mesh transition towards coarser or finer mesh on the surface...

All times are GMT -4. The time now is 04:07.