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

[ICEM] Volume Orientations Error In ICEM

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

Like Tree3Likes
  • 2 Post By PSYMN
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   July 17, 2013, 01:47
Default Volume Orientations Error In ICEM
  #1
Member
 
AhmadReza
Join Date: Jul 2012
Posts: 35
Rep Power: 4
ahmadreza is on a distinguished road
Hi
For My Master Project I need to have full structure Mesh on Ship Propeller


I can produce it but i have bad element (bad mesh) on tip of blade because of Leading edge of the blade is Sharp (Line)

Front of Leading edge I have Triangle Block ( I Know That is bad but i don't know How to modify it)

check Mesh ICEM 14.0 Shows:

ERROR:

the element is too bad and shows Volume Orientation Error

Please Help me How to Modify my Block

Thanks


http://upload7.ir/images/22350517418668597106.jpg
http://upload7.ir/images/08465106212636021821.jpg
http://upload7.ir/images/22447560473296158371.jpg
http://upload7.ir/images/35847535113813504727.jpg
http://upload7.ir/images/86102233848860599481.jpg
http://upload7.ir/images/54772143397342289193.png

Last edited by ahmadreza; July 17, 2013 at 05:05.
ahmadreza is offline   Reply With Quote

Old   July 17, 2013, 02:31
Default
  #2
Senior Member
 
Javi
Join Date: Jan 2013
Posts: 237
Rep Power: 7
FJSJ is on a distinguished road
Hi,

Did you delete the blocks inside the propeller?

Is your trailing edge sharp or blunt? I think is the second one, but Im not sure.

I think you can improve the blocking. Take a look in this thread:

Ralen Approach
FJSJ is offline   Reply With Quote

Old   July 17, 2013, 05:03
Default
  #3
Member
 
AhmadReza
Join Date: Jul 2012
Posts: 35
Rep Power: 4
ahmadreza is on a distinguished road
Thanks.

My Leading edge is sharp and my problem is here ///////////// and My trailing edge is blunt and it is good for me

(I write mistake tip propeller (MY tip Propeller is A little Blunk) )


Yes I Separate and delete Inside of Propeller


What your Idea about Block that is in the front of Picture

Regard
AhmadReza
ahmadreza is offline   Reply With Quote

Old   July 17, 2013, 10:14
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
Instead of a triangle block against your sharp edge, what if you collapsed it? (collapse the other side of the triangle also, so it is a sharp block...

With ICEM CFD Hexa, the best advice is to think schematically.

In profile, your blade is rounded, so you should be thinking of a CGrid...

Basically, your model is a wedge that is a bit twisty... Is the tip sharp or blunt?

Your model is tricky because the transition from sharp to round probably happens gradually as the blocking goes around the corner. You may need to make a judgement call to approximate it somewhere and give up some accuracy in exchange for quality. For instance, if the transition happens along the tip, you may need to pretend that the tip is like a thin wedge with a sharp front, flat back and flat tip... You can either modify the geometry or turn off the projection.

Also, part of your problem is because you have not tidied up your blocking further out from the blade... You are forcing blocks to fit to a curvy blade on one side without adjusting the very square layout away from the blades. You can massage that into place a lot better... If the blocking were to twist around the blade a bit, it would improve the quality.
Attached Images
File Type: jpg RoundedTipBlocking.jpg (77.0 KB, 44 views)
86682164 and FJSJ like 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   July 17, 2013, 10:53
Default
  #5
Member
 
AhmadReza
Join Date: Jul 2012
Posts: 35
Rep Power: 4
ahmadreza is on a distinguished road
Hi
Thanks for your Answer

My Tip is a little blunt
My leading edge is Sharp
My Trailing edge have fillet
I cant collapse it because I have a rotary domain ( I need Two Domain For Define In Fluent & ) and I Produce A total block and I segment it to 4 block
and next time I segment whole of block to O-block
So I have 1 Block for 7 blades I segment it and


http://upload7.ir/images/21111571856490580570.png
http://upload7.ir/images/03975327150012423368.png
http://upload7.ir/images/42967238947214923277.png
http://upload7.ir/images/66186523225767739262.png
ahmadreza is offline   Reply With Quote

Old   July 17, 2013, 11:29
Default
  #6
Member
 
AhmadReza
Join Date: Jul 2012
Posts: 35
Rep Power: 4
ahmadreza is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Instead of a triangle block against your sharp edge, what if you collapsed it? (collapse the other side of the triangle also, so it is a sharp block...

With ICEM CFD Hexa, the best advice is to think schematically.

In profile, your blade is rounded, so you should be thinking of a CGrid...

Basically, your model is a wedge that is a bit twisty... Is the tip sharp or blunt?

Your model is tricky because the transition from sharp to round probably happens gradually as the blocking goes around the corner. You may need to make a judgement call to approximate it somewhere and give up some accuracy in exchange for quality. For instance, if the transition happens along the tip, you may need to pretend that the tip is like a thin wedge with a sharp front, flat back and flat tip... You can either modify the geometry or turn off the projection.

Also, part of your problem is because you have not tidied up your blocking further out from the blade... You are forcing blocks to fit to a curvy blade on one side without adjusting the very square layout away from the blades. You can massage that into place a lot better... If the blocking were to twist around the blade a bit, it would improve the quality.


There is not possible because of my blade have minimum 18 degree skew and rake and ... this mean is my blade can't model with a Collapse block
ahmadreza is offline   Reply With Quote

Old   July 17, 2013, 12:24
Default
  #7
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 don't think that would stop you from collapsing the block, perhaps you do not understand what I mean... (Try the pipe blade tutorial for an example)

Also, I would suggest that you only model one segment of the problem (much less work) and then copy rotate it around to get the full geometry...
__________________
-----------------------------------------
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   July 17, 2013, 12:53
Default
  #8
Member
 
AhmadReza
Join Date: Jul 2012
Posts: 35
Rep Power: 4
ahmadreza is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Instead of a triangle block against your sharp edge, what if you collapsed it? (collapse the other side of the triangle also, so it is a sharp block...

With ICEM CFD Hexa, the best advice is to think schematically.

In profile, your blade is rounded, so you should be thinking of a CGrid...

Basically, your model is a wedge that is a bit twisty... Is the tip sharp or blunt?

Your model is tricky because the transition from sharp to round probably happens gradually as the blocking goes around the corner. You may need to make a judgement call to approximate it somewhere and give up some accuracy in exchange for quality. For instance, if the transition happens along the tip, you may need to pretend that the tip is like a thin wedge with a sharp front, flat back and flat tip... You can either modify the geometry or turn off the projection.

Also, part of your problem is because you have not tidied up your blocking further out from the blade... You are forcing blocks to fit to a curvy blade on one side without adjusting the very square layout away from the blades. You can massage that into place a lot better... If the blocking were to twist around the blade a bit, it would improve the quality.
Quote:
Originally Posted by PSYMN View Post
I don't think that would stop you from collapsing the block, perhaps you do not understand what I mean... (Try the pipe blade tutorial for an example)

Also, I would suggest that you only model one segment of the problem (much less work) and then copy rotate it around to get the full geometry...


thanks for Attention

My geometry is Contra Rotating propeller ( two propeller that rotate conter . the aft propeller are 5 blade and for propeller have 7 propeller ( the blade of for propeller are not same with aft propeller)

NOW
1-how i can make one blade or two blade and rotate ?

2- how i can make the farfeild forward and backward and Around of My Propeller?

3-How I can in this way make A cylinder around the propeller for produce two domain for Fluent?

Last edited by ahmadreza; July 17, 2013 at 15:20.
ahmadreza is offline   Reply With Quote

Old   July 17, 2013, 16:13
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: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You will need 3 volumes...

The large outer volume will be stationary.

The two inner volumes can be discs that will be meshed separately (non conformal)... Instead of a full disc, you can mesh a single blade for each. Use periodicity and then copy rotate them around.

Each of the three disks will be a separate volume material (FLUID1, FLUID2 and FLUID3 or whatever sensible names you choose). In Fluent, you would set up each zone and the wall boundaries to get the desired rotation.
ahmadreza 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   July 17, 2013, 16:43
Default
  #10
Member
 
AhmadReza
Join Date: Jul 2012
Posts: 35
Rep Power: 4
ahmadreza is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
You will need 3 volumes...

The large outer volume will be stationary.

The two inner volumes can be discs that will be meshed separately (non conformal)... Instead of a full disc, you can mesh a single blade for each. Use periodicity and then copy rotate them around.

Each of the three disks will be a separate volume material (FLUID1, FLUID2 and FLUID3 or whatever sensible names you choose). In Fluent, you would set up each zone and the wall boundaries to get the desired rotation.
So thanks For your Answer

I know We must have 3 Volume

IS it correct:

I Can Import My geometry ( AFT & FOR Propeller + FarFeild ) And Separate it (By Turn Off the block Of Them) And Have 3 different type Of Mesh (For Example Structure & UnStructure Mesh) And Save each of Volume separately;
And export them to Fluent ?


My Question is it When I Have different Type Of Mesh (both Have different Size Function Or Different type of Mesh)
Is it not problem(Error) On Interface of Volumes in Solvers (ex:Fluent or CFX)?

And How to Coordinate them on solvers ?( How Export them on ICEM or HOW to Import them to Solvers To Coupled Them (That The 3 Volume Mach Excatly )??
ahmadreza is offline   Reply With Quote

Old   July 17, 2013, 17:32
Default
  #11
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
CFX allows you to import multiple separate files, but Fluent wants you to import just one file with multiple zones.

This just means you need to combine them in another tool first. For instance, you could mesh all three files in separate ICEM CFD projects and then open a 4th project (or load them into TGrid or where ever) and combine them and then output a final combined project.

You could have 3 geometry sub models, or just a single geometry and only zoom in and mesh partial regions...

When you load 3 *.uns or *.msh files into ICEM CFD, they are concatenated. This means they are in one file, but nodes are not merged, etc. Perfect for output to Fluent.

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   July 18, 2013, 02:02
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
did you check this one?

Quarter O-grid topology for propeller blade
Far is offline   Reply With Quote

Old   July 18, 2013, 10:43
Default
  #13
Member
 
AhmadReza
Join Date: Jul 2012
Posts: 35
Rep Power: 4
ahmadreza is on a distinguished road
Quote:
Originally Posted by Far View Post

Hi
Thanks For Your Attention

I try It but a quality of mesh Was Not Good

Are You have Other Suggestion ??
ahmadreza is offline   Reply With Quote

Old   July 18, 2013, 10:54
Default
  #14
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Simon has already given very accurate suggestions.

Take one blade from both propeller and make mesh for them. You can get all blades in CFX-Pre and which can imported later to Fluent or you can copy mesh or blocking to get mesh for all blades as simon told you.

You need three volume (one for each rotating domain and one for farfield) as already indicated by Simon. But make sure that you have separate faces in fairfield volume for each blade volume. They should exactly match in axial extent.

Are you willing to share your project?
Far is offline   Reply With Quote

Old   July 18, 2013, 13:10
Default
  #15
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
http://www.forwind.de/sowe/Site/Prog...E2013_Dose.pdf


In first propeller you have round leading and trailing edge and also blade tip.

In 2nd propeller sharp leading edge and trailing edge with blade tip.

In both propellers you straight periodic boundaries, so make them according to blade shape.
Far is offline   Reply With Quote

Old   July 18, 2013, 13:18
Default
  #16
Member
 
AhmadReza
Join Date: Jul 2012
Posts: 35
Rep Power: 4
ahmadreza is on a distinguished road
Quote:
Originally Posted by Far View Post
http://www.forwind.de/sowe/Site/Prog...E2013_Dose.pdf


In first propeller you have round leading and trailing edge and also blade tip.

In 2nd propeller sharp leading edge and trailing edge with blade tip.

In both propellers you straight periodic boundaries, so make them according to blade shape.

Thanks

Can I Have One Request..

Please Send Me First Propeller With Block that you think it is good (block with boundary condition and Rotate)
(please Email to me)
ahmadreza is offline   Reply With Quote

Old   November 11, 2013, 23:44
Default sharp edge volume orientation error
  #17
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 4
handsome is on a distinguished road
Hi
Question
I want to mesh the body which have a sharp edge .but when the mesh was completed I see some element like the picture below. Some of this bad element is belong the body and when I invisible the body the disappear .but some of the bad element can be seen even when I invisible all parts of the body and when I use check mesh the put in added faces.
When I mesh the body by mesh size of 0.02 everything is ok but when reduce the max mesh size to 0.01 the bad element will appear.
(I have reduced the tri tolerance and edge criterion number )
handsome 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
[ICEM] Volume orientation MGF ANSYS Meshing & Geometry 2 September 19, 2012 11:55
minus volume mesh in ICEM Li CFX 6 August 3, 2008 04:56
ICEM CFD Mesh Quality "Volume change" Paul Brainerd CFX 1 May 25, 2008 23:37
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
help needed about phase change Yanhu Guo Main CFD Forum 4 January 24, 2001 00:16


All times are GMT -4. The time now is 14:13.