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

[ICEM] Free mesh control

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

Like Tree1Likes
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   September 20, 2011, 21:17
Default Free mesh control
  #1
Member
 
Ryne
Join Date: Jan 2010
Posts: 32
Rep Power: 7
Rhyno466 is on a distinguished road
I am working with an airfoil with a structured mesh area around the airfoil and and unstructured (free) mesh throughout the rest of the domain. I have used ICEM to do fully structured airfoil meshes in the past with great success, but the current research (for my MS thesis) requires many meshes to be created for a quasi- steady state analysis and I am required (advised) to use the current hybrid mesh setup.

I am struggling to resolve the wake area with enough resolution, and cannot figure out a good way to increase the mesh density where I need to. It seems that the expansion ratio of the cells is too high and thus the cells increase in size too rapidly for my liking.

I am looking for help and ideas to be able to increase the density of the wake area. I have already tried increasing the edge spacing with minimal luck. I have also have zero success using the refinement function but is more then likely user error. Thanks!
Attached Images
File Type: png coarser exit.png (40.4 KB, 76 views)
File Type: png finer exit.png (40.8 KB, 67 views)
Rhyno466 is offline   Reply With Quote

Old   September 21, 2011, 03:57
Default
  #2
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
Did you try mesh density boxes ?
BrolY is offline   Reply With Quote

Old   September 21, 2011, 11:34
Default
  #3
Member
 
Ryne
Join Date: Jan 2010
Posts: 32
Rep Power: 7
Rhyno466 is on a distinguished road
Thanks, this seems to be what I am looking for except that I am using blocking in order to get my structured boundary layer area. I dont think this mesh density function works with what I am doing currently. I dont even know how to mesh an airfoil without using a blocking scheme.
Rhyno466 is offline   Reply With Quote

Old   September 21, 2011, 11:49
Default
  #4
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
Density boxes work only with tetra mesh.

For the blocking, you can't use that function, but you have the edge parameters to help you. The bad thing is that it will propagate the refinement to the parallel edges. Another solution : create two topologies and make a non conformal merge (I think ICEM can handle only conformal merge, so you will need to do that with your solver software).

To create unstructured mesh is very easy with ICEM. Make a build topology of your domain. Check if your geometry is ok. Specified your maximal length in the mesh part parameters. Create a patch independent mesh (octree) of your domain. Delete the volume mesh. Smooth the surface mesh. Create a Delaunay (for example) volume mesh (based on the existing mesh). Smooth. Create your prism layers and that's good.
There are a lot of topics dealing with this method on this forum if you want
BrolY is offline   Reply With Quote

Old   September 21, 2011, 14:52
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
The paving algorithm needs an edge to control the mesh size locally.

You can give it one by splitting the unstructured block from the trailing edge to the middle of the outlet. Then setup a biased edge distribution...

This edge distribution won't propagate across an unstructured block, it will just control the mesh size on that edge of the loop and allow you to transition your mesh much better.
__________________
-----------------------------------------
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   September 23, 2011, 15:55
Default
  #6
Member
 
Ryne
Join Date: Jan 2010
Posts: 32
Rep Power: 7
Rhyno466 is on a distinguished road
OK, thanks! If edges control mesh size locally, what controls the global mesh sizing. As in how does it determine the maximum size that the cells grow to, and how fast they do grow to this maximum size?
Rhyno466 is offline   Reply With Quote

Old   September 25, 2011, 18:42
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: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
For that mesher (Patch Dependent Surface Meshing), you can set sizes on all the curves at once (global size), or set by part name or by individual curves...

You can also set sizes on Surfaces, there is an option to use these "surface" sizes and have the mesh transition towards coarser or finer mesh on the surface...
Rhyno466 likes this.
__________________
-----------------------------------------
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
Control mesh size in Cartesian lotus_blue ANSYS Meshing & Geometry 5 December 1, 2010 14:13
mesh quality control and fix tachyon_me OpenFOAM Native Meshers: snappyHexMesh and Others 0 October 6, 2009 12:48
Gambit Unstructed (Tet) Mesh - size control newbie FLUENT 3 August 26, 2008 11:38
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 09:38
mesh control problem TUM CFX 4 July 27, 2001 16:17


All times are GMT -4. The time now is 04:09.