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

[ANSYS Meshing] Mesh Quality

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

Like Tree3Likes
  • 1 Post By Far
  • 1 Post By Far
  • 1 Post By Far

Reply
 
LinkBack Thread Tools Display Modes
Old   September 18, 2012, 02:55
Default Mesh Quality
  #1
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
Hi,

What are the parameters used to test the mesh quality:
I know a few such as aspect ration, expansion ratio, orthogonality angle.
There is also this parameter CGI, kindly explain it.
Add any other parameters that are important when reporting a mesh.

Thank you
Regards
Hamed
hamed.majeed is offline   Reply With Quote

Old   September 18, 2012, 10:01
Default
  #2
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
topic about mesh quality is discussed multiple time in this forum try searching the forum i'm sure you will find a lot.
Don't know much about cgi parameters, hope someone else can explain it.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 18, 2012, 11:12
Default
  #3
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
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 hamed.majeed View Post
Hi,

What are the parameters used to test the mesh quality:
I know a few such as aspect ration, expansion ratio, orthogonality angle.
There is also this parameter CGI, kindly explain it.
Add any other parameters that are important when reporting a mesh.

Thank you
Regards
Hamed
mostly we are interested in min angle (>18 deg) , minimum quality (shoud be > 0.3) and expansion ratio. Mostly these parameters are viewed from solver point of view.

There is very nice explanation of these parameters by Simon on this forum, search is the key
hamed.majeed likes this.
Far is offline   Reply With Quote

Old   September 18, 2012, 14:18
Talking
  #4
New Member
 
AHMED
Join Date: Apr 2012
Posts: 5
Rep Power: 5
navedahmid is on a distinguished road
I think its GCI not CGI
navedahmid is offline   Reply With Quote

Old   September 19, 2012, 11:17
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 Help documentation should also include something for each metric, but I am not sure what metric you are asking about (GCI or CGI, I don't know of either). What tool are you looking in?
__________________
-----------------------------------------
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 21, 2012, 22:23
Default
  #6
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
Hi,
It is the grid convergence index GCI. It is a factor to estimate discretization error based on Richardson extrapolation principle
hamed.majeed is offline   Reply With Quote

Old   September 22, 2012, 02:09
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
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 hamed.majeed View Post
Hi
It is the grid convergence index GCI. It is a factor to estimate discretization error based on Richardson extrapolation principle
Well it is the index of quality of CFD which you are performing. In other words, it is you who will decide that how much mesh size is needed to the asymptomatic behaviour. Whether it is 1 million, 10 million or even 100 million. ICEM will give you whatever you ask for.
hamed.majeed likes this.
Far is offline   Reply With Quote

Old   September 22, 2012, 10:35
Default
  #8
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
Hi,
thnx for reply.

I have another question. We place the 1st node from the wall based on y+ value and the formula 1st node distance is
delta y = sqrt(74)*Re^(-13/14)*L*y+*L
The value of y+ in above formula depends on the turbulence model used.

My question is:
Once 1st node distance is specified using above formula, what are the parameters that govern the selection of expansion ratio applied to the mesh.
I mean what should the increasing gap of node be starting from the 1st node
hamed.majeed is offline   Reply With Quote

Old   September 22, 2012, 11:40
Default
  #9
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
Usually a ratio of 1.2 is used. But you could go higher or lower if you want the total height of your boundary layer to be less or greater.

The point is just to have enough mesh discretization to capture the boundary layer profile. That profile is changing faster near the wall and reduces as you move away. The ratio is just to reduce the number of nodes so you are not using the same resolution to capture less change.
__________________
-----------------------------------------
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 22, 2012, 16:25
Default
  #10
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
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 hamed.majeed View Post
Hi,
thnx for reply.

I have another question. We place the 1st node from the wall based on y+ value and the formula 1st node distance is
delta y = sqrt(74)*Re^(-13/14)*L*y+*L
The value of y+ in above formula depends on the turbulence model used.

My question is:
Once 1st node distance is specified using above formula, what are the parameters that govern the selection of expansion ratio applied to the mesh.
I mean what should the increasing gap of node be starting from the 1st node
Rule(s) of thumb:

1. Use expansion ratio 1.2 at max and for transition critical flows lower values to 1.15 or 1.1

2. For fully turbulent flows you can use the Y+ upto 10, in that case you will have the 10-15 nodes in the whole boundary layer. You can find the boundary layer total thickness from the turbulent flat plate boundary layer formulae

3. Boundary layer gets thinner as Reynolds number increases and vice-versa
PSYMN likes this.

Last edited by Far; September 22, 2012 at 16:38. Reason: Addition of Point # 3
Far is offline   Reply With Quote

Old   September 23, 2012, 02:35
Default
  #11
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
2. For fully turbulent flows you can use the Y+ upto 10, in that case you will have the 10-15 nodes in the whole boundary layer
Aaah I wish the whole world would have like that but the transitional flows always give me a headache and as a result extra care for wall y+ and no. of cells in boundary layer

Quote:
You can find the boundary layer total thickness from the turbulent flat plate boundary layer formulae
I want to add something here, after finding boundary layer thickness from turbulent flat plate boundary layer formula, reduce it by an order of magnitude to get good approximate for airfoils/wing problems
cfd seeker is offline   Reply With Quote

Old   September 23, 2012, 02:48
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
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 Far
For fully turbulent flows you can use the Y+ upto 10, in that case you will have the 10-15 nodes in the whole boundary layer.

Quote:
Originally Posted by cfd seeker View Post
Aaah I wish the whole world would have like that but the transitional flows always give me a headache and as a result extra care for wall y+ and no. of cells in boundary layer .

-----------

For transitional flows (laminar to turbulent), you need Y+ less than 1 with other constraints.
Far is offline   Reply With Quote

Old   September 23, 2012, 02:55
Default
  #13
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
For transitional flows (laminar to turbulent), you need Y+ less than 1 with other constraints.
Yes and the most important constraint is values of "Turbulence Parameters"
cfd seeker is offline   Reply With Quote

Old   September 23, 2012, 02:56
Default
  #14
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
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 cfd seeker View Post
Yes and the most important constraint is values of "Turbulence Parameters"
I meant the mesh constraints like enough no of nodes in normal and streamwise direction.
Far is offline   Reply With Quote

Old   September 23, 2012, 03:06
Default
  #15
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Originally Posted by Far View Post
I meant the mesh constraints like enough no of nodes in normal and streamwise direction.
Turbulence parameters also affects the performance of Turbulent Transitional Models
cfd seeker is offline   Reply With Quote

Reply

Tags
mesh, mesh quality

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
No layers in a small gap bobburnquist OpenFOAM Native Meshers: snappyHexMesh and Others 2 November 25, 2012 09:54
Polyhedral Mesh Quality in Star-CCM+ niazaliahmed STAR-CCM+ 3 March 8, 2012 14:51
[ICEM] Tetra mesh quality before and after prism layer Chander ANSYS Meshing & Geometry 0 December 25, 2011 23:04
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 07:32.