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

[ICEM] Icem cfd 13.0

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   August 20, 2012, 13:39
Default Tutorial Submarine
  #41
New Member
 
Marina
Join Date: Apr 2012
Posts: 5
Rep Power: 5
Mmm2010 is on a distinguished road
Hello. Check up my project tutorial Submarine. Thank you.
Attached Files
File Type: zip 2g-1.zip (24.7 KB, 4 views)
Mmm2010 is offline   Reply With Quote

Old   August 20, 2012, 13:49
Default
  #42
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
.tin file is missing in your project. can't load it.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   August 20, 2012, 14:15
Default Tutorial Submarine
  #43
New Member
 
Marina
Join Date: Apr 2012
Posts: 5
Rep Power: 5
Mmm2010 is on a distinguished road
Sorry, 2g-2.zip this .tin file. (ICEM CFD 12.0.1)
Attached Files
File Type: zip 2g-2.zip (73.1 KB, 3 views)
Mmm2010 is offline   Reply With Quote

Old   February 15, 2013, 07:50
Default
  #44
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
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 PSYMN View Post

You didn't send me the Tetin file (*.tin), so I didn't know where you set what sizes or prisms. I just set the global max to 2 and set a min size (sizing function) to 0.5. Then I hit compute mesh...
I am really confused about max size and min size. Why min size is size function and where I can set other attributes of size function and how does min size interact with max size?

Is there any effect of scale factor on min size?
Far is offline   Reply With Quote

Old   February 15, 2013, 10:48
Default
  #45
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
During the Octree process, there is an initial subdivision where the volume is divided up into blocks. The size of these initial blocks is the max size multiplied by the scale factor...

So if your max size is 8 and your scale factor is 2.5, the blocks will all be size 20.

Then Octree starts to look at further refinement based on the entities within each block... It basically checks each and says "is there any settings within this block that are smaller than the current size". Lets say you had something size 3 in the block... It would check size 3*2.5=7.5 < 20, therefore subdivide. The single size 20 block is split on each side and becomes 8 (hence "octree") size 10 blocks. Then each of these is compared with the 7.5. Yup, 7.5 is less than 10, so they are subdivided again. Now you have a bunch of size 5 blocks, notice we ended up smaller than 7.5. This is why we suggest you stick with powers of 2 times a base size. Anyway, It checks each size 5 block again and concludes that they are less than 7.5, so the octree portion can stop on those blocks. Each block is then subdivided into 12 tetras, transitions are taken care of, smoothing, etc.

If you have curvature and proximity based refinement, then it will also check those. For instance, lets say you had set 3 cells in gap and 12 cells per 360 degrees, those become the "goals" of the refinement. It would want to keep refining until it met these requirements also. In some models, you may have a tiny gap or small curve you were not expecting. Lets say you had mostly gaps of 10 (leading to size 2.5 mesh in the above example because size 5 would not satisfy the requirement). Now imagine that somewhere in the model, you had a tiny gap, maybe 0.5. The octree subdivision would need 4 more steps to get down to that, 2.5 => 1.25 => 0.625 => 0.3125 (still too big for 3 across) => 0.15625! Each time it refines, the mesh count goes up by 2^3! at least in the local area, things could quickly get out of hand.

We need a way to limit that refinement; Min Size.

If we set the min size to something like 1, it is multiplied by the scale factor and becomes 2.5. This would be fine enough to allow it to reach the goal of 3 cells in gap for most of the model, but would not let it get rediculous in the little area I am not actually interested in...


So do you get it? Thes are Octree settings. Max size is the largest size you will see. Min size is a limit on refinement. All of them are multiplied by the scale factor.

Personally, I almost always leave my scale factor as 1 and always use powers of 2 for my sizes (1, 2, 4, 8, 16, 32, 64, etc.) I only adjust my scale factor if I want to tweak my mesh. For instance, if I wanted it 10% coarser, I would set it to 1.1.
BrolY 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

Old   February 15, 2013, 10:50
Default
  #46
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
Oh yea, I nearly forgot...

You can also set a max size and min size on parts. Previously, I was talking about the global Max and Min.

If you set them on parts, they work similarly.

Max on a part or surface or curve will cause the octree process to subdivide until it is less than or equal to that max size locally.

Min size on a part or surface or curve will cause the octree to go BELOW the global min size and allow you to refine further than normal near that entity. This can be handy if there is some tiny feature you want to capture, but you don't want unnecessary refinement happening all over...
__________________
-----------------------------------------
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

Tags
icem cfd 13.0

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
Need help icem cfd kakhtar ANSYS Meshing & Geometry 24 March 24, 2014 14:04
[ICEM] Icem CFD on Linux mechanicaldesign ANSYS Meshing & Geometry 6 February 14, 2013 11:39
Transport mesh from ICEM CFD, to Fluent, to Sysnoise Wieland FLUENT 2 April 15, 2012 06:28
Importing Solidworks part into ICEM CFD MetalSupremacist FLUENT 0 October 8, 2010 17:46
Which is better to develop in-house CFD code or to buy a available CFD package. Tareq Al-shaalan Main CFD Forum 10 June 12, 1999 23:27


All times are GMT -4. The time now is 02:41.