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

[ANSYS Meshing] Ansys meshing result very high skewness

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

Like Tree1Likes
  • 1 Post By Far

Reply
 
LinkBack Thread Tools Display Modes
Old   March 10, 2012, 21:28
Default Ansys meshing result very high skewness
  #1
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
My Geometry is a wind turbine blade in a huge Air enclosure (1000m depth x 300m height)
I built it in Solidworks then select the enclosures in DesignModeler and started AnsysMeshing,I had tried many mesh types and reduce sizing
BUT the skewness alawys is very high as below:

Element 11088617
skewness Min 2.136 E-10
skewness Max 0.99999498

Any suggestion (I think to try ICEM CFD but iam not professional)
Attached Images
File Type: jpg Untitled.jpg (56.3 KB, 156 views)
File Type: jpg 1.jpg (33.5 KB, 129 views)
File Type: jpg 2.jpg (78.7 KB, 235 views)
m5edr is offline   Reply With Quote

Old   March 11, 2012, 01:29
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,906
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
BUT the skewness alawys is very high as below:
try to spot the max skewness area


Quote:
Any suggestion (I think to try ICEM CFD but iam not professional)
ANSYS meshing is good tool for quick design iteration, However ICEM is the ultimate tool to create high quality meshing and provides high control. It has also advantage of re-usability of blocking (Hexa).
Daniel_Khazaei likes this.
Far is offline   Reply With Quote

Old   March 11, 2012, 06:10
Default
  #3
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Quote:
Originally Posted by Far View Post
try to spot the max skewness area


ANSYS meshing is good tool for quick design iteration, However ICEM is the ultimate tool to create high quality meshing and provides high control. It has also advantage of re-usability of blocking (Hexa).
Thanks Dear Far
1-could you tell me how to spot the max skewness area?

2- When I tried ICEM by import the geometry From DM , the domains (Enclosures) looks different that in AM
I didn't know why , iam still beginner in ICEM

thanks again
m5edr is offline   Reply With Quote

Old   March 11, 2012, 08:44
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
In ANSYS Meshing, left click on the mesh branch of the tree...

In the resulting details panel, expand the statistics branch... Under Mesh metric, choose "Skewness" from the pulldown.

A histogram will appear below the graphics window.

Left click on the bar of the histogram and its elements will appear.

If the bar you want to see is too small to click easily, click on the "controls" button and adjust the X and Y axis to zoom in on the bad cells.

When you click on a bar, you will see those elements on the screen...
__________________
-----------------------------------------
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   March 11, 2012, 08:49
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: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Oh yea, what to do with what you find...

Look to see where the skewness is coming from. 9 times out of 10, it is due to over constrained geometry forcing the mesh into awkward configurations...

If the over-constrained geometry is just surface patches (like a sliver surface forcing the mesh to conform) you could try the patch independent tetra or you could try virtual topologies to merge the surface patches together...

If it is between regions, such as between your turbine and the boundary of the rotating region... That second boundary is arbitrary... and you could just increase the size of that disk to allow for more space (flexibility) for the mesh...

If it is something else, post the pic.

Best regards,

Simon
__________________
-----------------------------------------
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   March 11, 2012, 10:43
Default
  #6
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
I reached to bad elements , I will try to repair them
Many thanks

Last edited by m5edr; March 11, 2012 at 11:41.
m5edr is offline   Reply With Quote

Old   March 12, 2012, 08:52
Default
  #7
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Dear simon

I reached to bad elements in My geometry (attached photo)
It is because "Inflation" that used around the blade (this "Inflation" is nessary due to Boundary Layer consideration)

Without Inflation >>> Max Skewness is 0.87 (prefect)
With Inflation>>>> Max Skewness is 0.9999

I tried many types of inflation that result in same High Skewness any change.
Any suggestion,
Thanks
Attached Images
File Type: jpg bl.jpg (92.4 KB, 226 views)
m5edr is offline   Reply With Quote

Old   March 12, 2012, 09:03
Default
  #8
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You would have to zoom in to get a better idea of what is going on...

My guess is that the inflation at the top of the blade is meeting the inflation from the other side... Since they meet at a trailing edge, you get a sharp angle between them. No amount of smoothing or other "mesh" fixes will solve this problem because when you make one side better, the other side gets worse.

Some people fix this problem by putting a zero thickness baffle behind the trailing edge. This splits the angle (prism grows from both sides) and solves the problem... However, where the thin prism baffle ends, you may have other problems if you can't taper it out. (I know how to taper it out in ICEM CFD, but I don't know how in ANSYS Meshing, maybe someone else knows).

But you could also just try sending it to the solver as it is. The solver can often handle these sorts of poor quality prisms much better then it would handle poor tetras...
__________________
-----------------------------------------
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   March 12, 2012, 11:13
Default
  #9
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Many thanks for replay , i am really appreciated that

I attached more closer image , any change in your replay after this images
Note: there is no inflation at the top of the blade (Inflation at both sides of the blade)

thanks again
Attached Images
File Type: jpg 222.jpg (49.0 KB, 174 views)
File Type: jpg 11.jpg (57.1 KB, 191 views)
m5edr is offline   Reply With Quote

Old   March 12, 2012, 11:15
Default
  #10
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I had expected they were just along the trailing edge...

I guess the wing tip could be a similar problem where the prisms are tilting to miter around the tip...
__________________
-----------------------------------------
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   March 12, 2012, 11:37
Default
  #11
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
I had expected they were just along the trailing edge...

I guess the wing tip could be a similar problem where the prisms are tilting to miter around the tip...
Sorry
I didn't understand...Is the"wing tip" tutorial or form ??
thanks
m5edr is offline   Reply With Quote

Old   March 16, 2012, 13:06
Default try advanced size function and adjusting your max/min sizes
  #12
New Member
 
Join Date: Dec 2010
Posts: 5
Rep Power: 6
mrdelaunay is on a distinguished road
It looks like either your advanced size function is off or your are not setting the correct max/min sizes. Try setting the physics preference to CFD.
mrdelaunay is offline   Reply With Quote

Old   March 16, 2012, 13:17
Default
  #13
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
@m5edr, by "wing tip", I just meant the tip of the airfoil shown in your images... I guess it may not actually be a wing...
__________________
-----------------------------------------
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   March 16, 2012, 22:09
Default
  #14
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Quote:
Originally Posted by mrdelaunay View Post
It looks like either your advanced size function is off or your are not setting the correct max/min sizes. Try setting the physics preference to CFD.
On the contrary,
My advance size function is ON and also i tried many size function !!

Any way i started ICEM , May it comes new News
m5edr is offline   Reply With Quote

Old   March 16, 2012, 22:13
Default
  #15
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
@m5edr, by "wing tip", I just meant the tip of the airfoil shown in your images... I guess it may not actually be a wing...
Thanks Simon

I started ICEM , it provide many tools to fix the mesh
Till now I face same problem but i think solution is close and maybe i need your help if i stopped

thanks again
m5edr is offline   Reply With Quote

Old   January 5, 2014, 17:11
Default Very high skewness within two cell zone.
  #16
Senior Member
 
Tanjina Afrin
Join Date: May 2013
Location: South Carolina
Posts: 158
Rep Power: 4
Tanjina is on a distinguished road
Hi Simon,

I am modeling a 3D object. I found very high skewness in between two cell zone using workbench meshing. Before starting the "run Calculation" , I checked " check case" and it gives me this warning that 696 cell exceed 0.98 skewness. I found a way using Fluent 14.5 to repair the face mesh, but couldn't find any way how can I repair this skewness within the cell zone. Please find the attached image for details.

My model's mesh has high aspect ratio also i.e. 14.3, but Fluent didn't give any warning regarding this.

Any suggestion for lowering the skewness will be highly appreciated. Thanks in advance.

Regards,
Tanjina
Attached Images
File Type: jpg skewness.jpg (98.1 KB, 83 views)
Tanjina is offline   Reply With Quote

Old   March 31, 2015, 04:11
Default best way to reduce skewness and its successful, i tried
  #17
New Member
 
S.Frank Richarrd
Join Date: Mar 2015
Posts: 1
Rep Power: 0
sfrankricharrd is on a distinguished road
by using inflation> use auto inflation> programmed controlled and i generated my mesh. it shown the skewness value as 0.8999.

then i tried

inflation> use auto inflation> none

then i got the skewness value as 0.822
sfrankricharrd 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
[ANSYS Meshing] ANSYS Meshing hangs at "Preparing to model boundary for part" jonny_b ANSYS Meshing & Geometry 12 June 12, 2012 01:55
[ANSYS Meshing] ANSYS Meshing vs GAMBIT aerospain ANSYS Meshing & Geometry 0 September 28, 2011 06:05
Parallel Meshing in ANSYS 13 makkks ANSYS Meshing & Geometry 1 September 5, 2011 12:34
Interface between meshes and high skewness Danny FLUENT 0 September 13, 2005 11:23
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 09:55.