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

[ICEM] Mesh sizing - Rule of thumb !!!

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 15, 2013, 01:41
Default Mesh sizing - Rule of thumb !!!
  #1
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,963
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I am very much confused about the mesh size for the tetra module. I really dont understand how I can assign the mesh sizes in beginning. I know we can do it by measuring the overall geometry size on particular location and using trial and error but this method does not seem to be robust and efficient.

Now my question is (with reference to octree):

1. How to define sizes on global level. Like scale factor, max element size and curvature and proximity.

2. How to define the sizes in part mesh set-up for :
a) local geometry (e.g. wing, aircraft etc)
b) For the far-field parts
c) For Fluid (material point)
Far is online now   Reply With Quote

Old   February 16, 2013, 15:55
Default
  #2
Senior Member
 
Join Date: Dec 2009
Posts: 129
Rep Power: 10
mjgraf is on a distinguished road
For me it depends (the universal answer). hehe.

I typically set the global scale factor 0.001, so if you have parasolid, typically in meters, this will allow me to think in millimeters.

I also ensure that the tri tolerance is small, 1e-6 for final meshing. HEXA use the b-surface option.

One can also think in scale of features to resolve. When thinking in mm this is easy. Also being restricted to the Octree growth formula simplifies things too.

Another indicator I use is the Surface Dev Quality metric to ensure I am resolving the geometry properly.

these are all pretty easy for the RANS models. Going to DES, SAS, etc. the mesh needs further refinement than just resolving the geometry and areas I know have large gradients or recirculations.

Just some thoughts.

Calculate and refine as necessary for things you may have missed like wall spacing, etc.

Quote:
Originally Posted by Far View Post
I am very much confused about the mesh size for the tetra module. I really dont understand how I can assign the mesh sizes in beginning. I know we can do it by measuring the overall geometry size on particular location and using trial and error but this method does not seem to be robust and efficient.

Now my question is (with reference to octree):

1. How to define sizes on global level. Like scale factor, max element size and curvature and proximity.

2. How to define the sizes in part mesh set-up for :
a) local geometry (e.g. wing, aircraft etc)
b) For the far-field parts
c) For Fluid (material point)
mjgraf is offline   Reply With Quote

Old   February 18, 2013, 05:00
Default
  #3
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
Maybe I didn't understand what's your problem is, but go to : Mesh -> Part Mesh Setup and Mesh -> Global Mesh Setup ...
BrolY is offline   Reply With Quote

Old   February 21, 2013, 14:03
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,963
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
My problem is " I always end up with ICEM stuck up in making mesh more than 30-40 million and progress bar is at 20% or less" . In my estimate I should get around one million mesh size for full volume.

I am always confused in :

1. Specifying the curve mesh parameters : Should I specify size or no of nodes. Will it be used in octree?

2. Surface mesh size: There are many large and small parts. If I specify the size as per smallest part then I have very large mesh due to over refinement in large parts. If I consider the largest part, I get the under resolved smaller parts.

3. Both curve mesh and surface mesh parameters are used for octree?

4. What is the role of the max element size.

In short I want the rule of thumb in setting the sizes for octree for any model and with one click on compute I get the one decent volume mesh.
Far is online now   Reply With Quote

Old   February 21, 2013, 14:25
Default
  #5
Senior Member
 
Join Date: Dec 2009
Posts: 129
Rep Power: 10
mjgraf is on a distinguished road
You probably have a max deviation set that is very small? I have had cases where using this creates really odd mesh densities that I feel should not be there. I have also had issues when using a UG generated parasolid and a simple surface, at least appears simple (cylinder for example) would take forever to mesh. I deleted the surface and used the remaining edge curves to create surface using ICEM surfacing and poof, issue gone.

1. just starting to investigate defining on curve and multiple material points, but to fully answer your question, refer to the Global Mesh Setup Tables in the ICEM CFD Help.

2. split by parts (be aware where curves and points go) and use the Part Mesh Setup. Then utilize the tetra size ratio to control the surface mesh growth from the small to large size parts (then for the volume, Delaunay Spacing Scaling Factor)

3. refer to 1.

4. allows control of the max element size on a part/curve/surface/body. Read the Help about Global Element Scale Factor. Ensure that Global Element Seed Size is larger or the max element size will not be what you expect. I have found an issue with Volume tetra max size where it can not be smaller than the Global Element Seed Size, but works for hexa-core, really odd.

A one click good mesh only comes with using similar models day-to-day. for the strange one that comes in that I am not sure, after running Build Topology and creating my parts, I use the Surface mesher part by part to fine tune. So much faster than waiting for the octree to complete for a large mesh just to look at the surface mesh. You also catch where the mesher messes up with the max deviation setting. When this happens I turn off max deviation, reduce my max element and then use the Surface Dev quality to make sure my deviation is within machining tolerance.


Quote:
Originally Posted by Far View Post
My problem is " I always end up with ICEM stuck up in making mesh more than 30-40 million and progress bar is at 20% or less" . In my estimate I should get around one million mesh size for full volume.

I am always confused in :

1. Specifying the curve mesh parameters : Should I specify size or no of nodes. Will it be used in octree?

2. Surface mesh size: There are many large and small parts. If I specify the size as per smallest part then I have very large mesh due to over refinement in large parts. If I consider the largest part, I get the under resolved smaller parts.

3. Both curve mesh and surface mesh parameters are used for octree?

4. What is the role of the max element size.

In short I want the rule of thumb in setting the sizes for octree for any model and with one click on compute I get the one decent volume mesh.
mjgraf is offline   Reply With Quote

Old   February 22, 2013, 04:41
Default
  #6
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,963
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
What is the effect of putting zero size?

I also want to know about hexa merge? How do we use it in tetra mesh generation process for the wings? (Reference Page No 70 ICEMCFD_Tips&Tricks2010.PDF

Far is online now   Reply With Quote

Old   February 22, 2013, 04:59
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,963
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by mjgraf View Post
You also catch where the mesher messes up with the max deviation setting. When this happens I turn off max deviation, reduce my max element and then use the Surface Dev quality to make sure my deviation is within machining tolerance.
Can you describe in detail the purpose of max deviation with some images if possible !!!
Far is online now   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
[ICEM] Negative volume error in hybrid mesh siw ANSYS Meshing & Geometry 4 September 3, 2014 05:25
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
erroneous temps in conjugate model? sieginc. STAR-CCM+ 11 July 14, 2012 03:41
[ANSYS Meshing] Mesh sizing Kirjain ANSYS Meshing & Geometry 6 June 23, 2012 14:50
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55


All times are GMT -4. The time now is 01:53.