CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Meshing one body part only (

serezhkin June 25, 2010 17:21

Meshing one body part only
Hi all,

I am new to this forum, and although I have some CFD experience, I just started using ANSYS.

I have an assembly imported into ICEM, which is a enclousre containing some parts. The air inside the enclosure was identified by ICEM and a body part was created.

When I do the meshing for the entire model, the air volume gets meshed, but it takes too much time, and I have to delete volume meshes for parts I don't need afterwards.

The question I have is as follows:

Is there a way for me to mesh the air volume only, without meshing the entire model?

Any help would be appreciated.

serezhkin June 28, 2010 14:23

Perhaps, as an alternative, someone could suggest a way to refine mesh in one volume mesh block only.

PSYMN June 29, 2010 11:37

Octree algorithm
Sometimes it helps to understand how the various algorithms work. The octree algorithm meshes the entire volume from min to max without respect to the geometry. The refinement algorithm is an OCTREE one that simply looks within each hexa and says "are there any entities within this box that are smaller than this current size. If yes, then refine (cut in half in 3 directions, 2^3=8, Octree). It refines inside and outside your area of interest based on your max size settings and any other geometry you have laying around. Then when all the refinement has stopped, it converts to tetra and transitions between mesh sizes. Then it fits to the geometry using the edge criterion to decide if edges need to be split before nodes can be moved to the surface (the message window will say it is running the "cutter"). Then shells are formed on the surfaces. Then the flood fill process happens. During flood fill, the algorithm finds a material point and marks it as in that part (such as FLUID), then it adds all the neighbor volume elements and continues until it is bounded by shells. (if a shell has the same fluid on both sides and is not marked as internal wall, it is removed, if the flood fill can go from the material point to another material point (such as the automatically created ORFN point outside the model), then you have leakage). After going thru each material point and flood filling, it throws away the remaining mesh and then it moves on to smoothing.

In your case, you have no material points, so it helps you by creating one in each volume. If you manually create a single material point in your fluid region, it will prevent the other regions from filling, but it won't prevent the refinement, that is the inherent downside in the octree method.

You could reduce your refinement by setting larger mesh sizes on the parts not adjacent to the fluid region you are interested in. Deleting geometry is also a good idea. If you mesh is good quality, you could try the patch dependent surface mesher followed by one of the bottom up tetra methods (such as Delaunay or Advancing Front). These have the advantage of being more targeted and only generating the mesh that you want, but the mesh setup is harder.

If your geometry is relatively simple (topologically speaking), it may be best to generate a quick Hexa mesh on it. For instance, an exhaust assembly may create quite a large box in XYZ space, and so would be very inefficient for octree tetra (unless you meshed it in smaller segments and merged them). However, it is relatively simple topologically and could be very easily hexa meshed.

Post an image and I can make a custom suggestion.

serezhkin June 29, 2010 15:36

Thank you for the detailed explanation!
This helps a lot.
I will try to remove material points from all bodies except the air volume. This way only the mesh which connects to material points will be left during the flood, if I understood correctly how the process works.

All times are GMT -4. The time now is 10:48.