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

[ICEM] Number of Nodes

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 13, 2011, 12:16
Default Number of Nodes
  #1
New Member
 
Join Date: Nov 2010
Posts: 22
Rep Power: 6
gi12 is on a distinguished road
Hi all

A quick question. Is it possible to specify the number of nodes for tetra meshing?, and if yes how can you do that

Many thanks
GI12
gi12 is offline   Reply With Quote

Old   October 13, 2011, 14:32
Default
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You specify the size of the mesh in the volume and/or on entities... Then the mesher fills the volume with elements of the specified sizes. The number of elements in the volume or the number of nodes in the mesh are the result of that filling process and will vary with a number of parameters including the type of mesh, growth rate, etc...

For unstructured mesh in simple situations, it may be possible to predict roughly, but the more complicated the geometry or the greater variety of mesh parameters, the harder that would be...

If you are talking about hexa blocking (structured meshing), then it becomes simpler and you can calculate the number of nodes or elements you want in each block and then back calculate the required edge parameters...

Usually, we use experience or trial and error with setting mesh params and seeing how many elements result for a particular model. If you want to scale things up just a bit, you can adjust the Global Element Scale Factor...
__________________
-----------------------------------------
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   October 13, 2011, 15:15
Default
  #3
New Member
 
Join Date: Nov 2010
Posts: 22
Rep Power: 6
gi12 is on a distinguished road
Thank you very much for your reply
Any mesh morphing capability in ICEM? the FLUENT mesh morpher is not clear
Thank you
GI12
gi12 is offline   Reply With Quote

Old   October 13, 2011, 16:23
Default Mesh Morphing in Fluent
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
No, not in ICEM CFD... There is one in ANSYS Meshing, but that is beta...

But actually, the Fluent Mesh Morpher just got decent for 14.0 (promoted from beta to release for 14.0)... It is not fancy like RBF-Morph which also works well in Fluent), but it is included at no extra cost ;^) and has powerful integration advantages because it morphs the mesh inside the case file while the solver is running (no expensive I/O or restarting).

You can get presentations about it on our website... I presented one over a month ago at the Houston conference and again last week at the conference in Irvine California... Go to the ANSYS website and you can download those presentations.

Best regards,

Simon
__________________
-----------------------------------------
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   October 13, 2011, 16:24
Default Ansys 14.0...
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Just an FYI, ANSYS 14.0 release is planned for 4 to 6 weeks from now...
__________________
-----------------------------------------
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   November 12, 2011, 20:58
Default curve number of nodes
  #6
New Member
 
Join Date: Nov 2010
Posts: 22
Rep Power: 6
gi12 is on a distinguished road
Hi PSYMN
Can you define the number of nodes in a curve for tet meshing? I know that is possible for Hex meshing , but for tet meshing number of nodes identifies the maximum size not the exact number of nodes and I always do not get the same number of nodes I entered.

Many Thanks
gi12 is offline   Reply With Quote

Old   November 14, 2011, 12:19
Default
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
It depends on the tetra method...

If you use delaunay or Advancing Front, it starts from the sizes set on the curves to mesh the curves (so you get exact sizes). From there the surface mesh is marched across the surfaces, and then from the surface mesh it generates the volume mesh. So with those meshers, the answer is yes. You can right click on curves in the model tree to display the curve sizing, you can use the Mesh tab to adjust the curve node distributions, biasing, etc. on the curves.

However, if you are using patch independent tetra, it uses a top down method that starts with the volume mesh and ends up fitting to the surfaces and curves after the mesh is refined. This method looks as the general sizing on the curves and surfaces and uses it with the Octree algorithm (you can check the help for specific details on this algorithm) to decide if the mesh needs to be refined or not. This method does not give you a precise use of the curve node distribution, it just uses the base size to decide (yes or no) to a further level of refinement. In fact, with octree, each level of refinement just splits the elements in half from the previous level, so control is approximate and sizes are limited to powers of 2 over the min size.

Read more about the algorithm in the help and you will get a good appreciation of how it is using your meshing parameters. I find this awareness helps users set their parameters more simply and more quickly.
__________________
-----------------------------------------
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   November 16, 2011, 07:01
Default Nodes position
  #8
New Member
 
Join Date: Nov 2010
Posts: 22
Rep Power: 6
gi12 is on a distinguished road
Thanks PSYMN.. That was really helpful
One more question please, is it possible to export XYZ nodes position as a txt file for a selected part?
Many thanks in advance
GI12
gi12 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
Mesh Refinement Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Mesh Utilities 41 January 17, 2013 03:43
Interpolation (Number of mapped nodes) Sam CFX 3 January 6, 2008 20:51
Number of nodes on block. Felix CFX 0 October 24, 2007 22:26
number of nodes anna CFX 2 December 15, 2006 11:29
mesh size - number of nodes sam FLUENT 0 November 11, 2006 14:10


All times are GMT -4. The time now is 12:00.