CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Is Bulid Topology necessary (http://www.cfd-online.com/Forums/ansys-meshing/113771-bulid-topology-necessary.html)

sujay February 26, 2013 08:40

Is Bulid Topology necessary
 
Dear All,

I am creating geometry from the vertices. The circles which are inlet and outlet get segmented when build topology is done.

Is i necessary to carry build topology operation ?

Thanks

Sujay Patil

BrolY February 26, 2013 08:48

Do you want to go for blocking or tetra mesh ?

For tetra mesh, it's highly recommanded, and even compulsory when you used the option patch dependent.

By the way, I think you can play with the option of the bluid topology to avoid the curves to be splitted.

sujay February 27, 2013 01:52

Quote:

Originally Posted by BrolY (Post 410194)
Do you want to go for blocking or tetra mesh ?

For tetra mesh, it's highly recommanded, and even compulsory when you used the option patch dependent.

By the way, I think you can play with the option of the bluid topology to avoid the curves to be splitted.

Dear Boles.

Thanks.

Blocking is not used.

Meshing Details :

Shell Meshing: Patch dependent with Quad dominant Mesh
Volume Meshing : Tetra/mixed with Robust(Octree)

With use of build topology surface created from circle (which were created from three vertices and used as inlet and outlet) get segmented along circumference with addition of few more vertices on circumference after topology.

That's why i want to avoid build topology. Will it OK

Sujay Patil

PSYMN February 28, 2013 15:20

You should not be surface meshing and then running PI tetra, just skip the surface meshing and run PI tetra directly. It is a top down method that will generate the surface mesh for you.

Patch conforming methods require you to build topology and require you to set the sizes on the curves. These methods start from the curves and then generate the surface mesh and then you could fill with a delaunay or advancing front algorithm.

PSYMN February 28, 2013 15:26

Sorry, reading thru a private email on the side and I got a bit more info... here is the side email...

Quote:

I am not importing the drawing from any CAD package. I am creating vertices and then geometry from these vertices.

Secondly, I am not specifying the shell meshing, they are default eventhoigh i use only mesh. There is no problem in meshing except some single/multiple edges and delauncy violation.

Do you mean i have to use patch independent shell meshing and then default volume meshing ?

Please correct me.
If you are building the geometry inside ICEM CFD, then the topology needs to be built for bottom up methods (it can already be built if you imported from CAD).

Those defaults are in place to fill gaps if you don't provide enough info. For instance, if you asked it to compute a volume mesh using delaunay, it would first need a surface mesh, so it would check to see what settings you have there.

In your case, you just need to go to Mesh => Compute Mesh => Volume mesh. Set the mesh type to "Tetra/Mixed" and the Mesh Method to "Robust (Octree)" and hit the compute button at the bottom.

You may still get multiple edges, but those are expected if you have t connections in your model. Single edges may indicate a hole or they may simply be the edges of baffle surfaces. Delaunay violations are issues such as tight corners where delaunay may have trouble placing tetras, but they don't matter if you are using the Octree method.


All times are GMT -4. The time now is 01:14.