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

[ICEM] Tetra mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 23, 2011, 15:06
Default Tetra mesh
  #1
New Member
 
Papis
Join Date: Dec 2010
Posts: 25
Rep Power: 5
papis is on a distinguished road
Hi again,
I created a 3d unstructured tetra grid of a wing using tetra mesh. from the mesh quality I noticed that tetras are made(also) INSIDE of the wing.By defining the boundary conditions on the airfoil surface you have no actual problem solving the mesh,but it's this the way it supposed to be done?

When meshing 2d airfoils I use the segment surface function to "approximate" the actual fluid surface but in 3d there is no such a function.

I also don't understand fully the concept of material points when defining a body.From the tutorials i have read material points at defined as a point in the inner and a point in the outer boundaries.But is it really one point enough for the mesher to understand the boundaries(which may be multiple sufaces.)?

I would greatly appreciate If anyone could enlighten me in this issues.

Thanks a lot
papis is offline   Reply With Quote

Old   June 24, 2011, 08:15
Default
  #2
New Member
 
Papis
Join Date: Dec 2010
Posts: 25
Rep Power: 5
papis is on a distinguished road
Here is a problem I am facing. On the first picture u see my whole model and on the second picture is only the wing. As you can see the wing mesh is not good. It is not a matter of tolerance as I have changed it to be very low.

How can I tell ICEM to mesh only the volume between the wing and the Farfield and not ALL the volumes. A closer look and you will find out that it meshes the volume inside the wing.

papis is offline   Reply With Quote

Old   June 24, 2011, 11:51
Default Flood Fill Explained...
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
The "Material point" is a simple concept once you understand how the octree mesher is working... This is all pretty well explained in the help, so I will let you go look that up. But basically, the octree mesher generates the volume mesh first (everywhere) and then fits to surfaces, creates shells, etc. At the end, it looks for your material point. It assumes you are interested in the volume element that your material point is in and adds that volume element to the PART of your material point. Then it assumes you probably don't just want a single element in your fluid, so it adds the neighbor elements (flood fill), and then it adds the neighbors of those elements. The flood fill algorithms keeps adding volume elements to the FLUID part until it is completely surrounded by shells (surfaces). Then it stops and checks for a new material point.

If it can't find any other material points, then it assumes the rest of the volume elements are junk and deletes them.

If it can find a material point, it will repeat the flood fill process for that volume.

If the flood fill can get from one material point to another or to the outside of the domain, we define that as leakage.

If you have no material points in your model, the software tries to help you out and creates materials for each volume. Perhaps this is your issue?

The solution, before meshing, is to create a single material point the the volume you want to mesh. If you created one in the wing, delete it. If you didn't, then no worries.

The solution, after meshing, if you don't want to remesh, is to create the material points and then run Flood fill manually (Option under Edit Mesh => Repair), or you could just delete the volume parts you done want right from the model tree.

Also... your wing mesh is way too coarse, but I am guessing you know that and it was just to simplify the images...
__________________
-----------------------------------------
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
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
[ICEM] Hexa mesh, curve mesh setup, bunching law Anorky ANSYS Meshing & Geometry 3 December 18, 2009 10:27
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 09:38
VOF with tetra mesh doesn't converge Gregor FLUENT 1 March 1, 2005 13:09


All times are GMT -4. The time now is 17:16.