CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] Is Bulid Topology necessary

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By BrolY

Reply
 
LinkBack Thread Tools Display Modes
Old   February 26, 2013, 08:40
Default Is Bulid Topology necessary
  #1
Member
 
Sujay
Join Date: Apr 2010
Location: Karnataka, India
Posts: 40
Rep Power: 7
sujay is on a distinguished road
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
sujay is offline   Reply With Quote

Old   February 26, 2013, 08:48
Default
  #2
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
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.
PSYMN likes this.
BrolY is offline   Reply With Quote

Old   February 27, 2013, 01:52
Default
  #3
Member
 
Sujay
Join Date: Apr 2010
Location: Karnataka, India
Posts: 40
Rep Power: 7
sujay is on a distinguished road
Quote:
Originally Posted by BrolY View Post
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
sujay is offline   Reply With Quote

Old   February 28, 2013, 15:20
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   February 28, 2013, 15:26
Default
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
attachDetach Topology Modifier: Proper Turbulent Boundary Conditions mturcios777 OpenFOAM Running, Solving & CFD 4 September 13, 2012 04:56
Topology change and zone modification WiWo OpenFOAM 0 July 7, 2010 04:35
[ICEM] Building topology command script files Anorky ANSYS Meshing & Geometry 8 January 11, 2010 08:25
ICEM topology Igor-a CFX 0 July 24, 2008 07:05
Topology SAM FLUENT 2 October 13, 2004 00:01


All times are GMT -4. The time now is 02:36.