2D Rectangular Mesh in Ansys Meshing
 

Ansys 12 Meshing.
A geometry is a simple tube, in 2D - just a rectanular.
I want to make a rectangular (or square) mesh. But when I'm trying to do so, the mesh is not fine in some parts of the domain (cells are not totally square). See picture below:
http://img.leprosorium.com/758634
How can I solve this issue?
Thanks in advance

Mapped
 

Could be one of several issues.


If it is not mapped, the free meshing is not always rectangular (looks mapped, but actually paved), and user should add a mapped face mesh control.


If it is mapped (already has a mapped face mesh control or adding one doesn’t help), this could be related to virtual topologies or facetization of the model, in which case using the “project to underlying geometry” (new option in 12.1) would help.

Thanks a lot, Simon!

I need also a mesh refinement near the boundary. How can I perform this while using the Mapped Face Meshing?

When I make a Mapped Face Meshing all Inflations are not working, it is written: "Active: No, Invalid Method".

I've tried turn on/off all options I've seen but I haven't managed to make a boundary layer refinement with Mapped Face Meshing. Does anybody know how to make this?

Hello Belgio,

Did you figure it out how to fix this issue?
I have the same problem...

Thanks,
Hoom

Same issue
 

I also have the same issue. With a mapped face, I cannot have a Boundary layer mesh on the same face. I worked around it (for the time being), by having a paved mesh on the face (using quad elements only) and then sweeping my domain using this face as the source. I had to specify manual source, so that I could add an inflation later on on this face and using the boundary edge.

Hope this helps.

Also, if anyone can find out how to add BL mesh to a mapped face, plz comment. The other, and more basic, way would be to use mesh sizing on an edge in the wall normal direction to get the BL mesh manually. It worked for me on a simple 3D geometry, but I haven't tried it on more complex ones.

You cannot add the usual inflation option to create a boundary layer mesh on faces with a mapped meshing.

Instead, as pranab_jha already mentioned, you can specify the cell distribution on the edges of the face.
Simply add a sizing option to the edges that need bunching.
Then you can add a bunching law to mimic a boundary layer mesh.
Remember to set the behaviour of the edge sizing to "hard", otherwise your input is likely to be ignored by the mesher.
Since version 15.0 of Ansys workbench, you can finally change the orientation of edges that produce a "reversed" bunching behaviour.
With the older versions, you simply put these edges to a second sizing function and choose the opposite bunching direction.

Of course this approach is limited to rather simple geometries and does not provide the amount of control you usually want, so better choose a meshing tool like ICEM for complex geometries.

How can subdivide the first grid raw near the wall to account for near wall treatment using ansys meshing. I have done mapped faced meshing with proper sizing but i cant subdivide the grid next to wall

Hi Everybody,
In mesh, I already divided the model into sweep-able bodies. But now, I see imprinted faces in my model on ANSYS Mechanic. Those imprinted faces are not existed in DM. How can I remove those faces since they affect the quality on meshing?