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

[ICEM] Meshing a blade inside air volume

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

Like Tree2Likes
  • 2 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   May 5, 2011, 15:39
Default Meshing a blade inside air volume
  #1
New Member
 
LittleBart
Join Date: Jan 2011
Posts: 20
Rep Power: 6
LittleBart is on a distinguished road
Hi there!

I'm trying to make a good-looking mesh for my wind turbine study. It's a blade and 120 deg sector of surrounding air. The airfoil is linearized with shorty lines in order to eliminate high-order NURBS surfaces problem, which I had suffered much from previously.

I want to mesh it in ICEM but not sure what strategy to use for blocking. Actually there are too many faces with different angles and locations to do this manually. Is there any techniques to associate inner o-grid block to the blade surface with minimum movements?


LittleBart is offline   Reply With Quote

Old   May 6, 2011, 09:31
Default
  #2
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
If you take a look thru my posts, we already went thru this with someone else and I posted a lot of blocking images...

Once your blocking is right, you may be able to snap fit (one click) the surface projected nodes around the airfoil down to the surface...
__________________
-----------------------------------------
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   May 6, 2011, 10:52
Default
  #3
New Member
 
LittleBart
Join Date: Jan 2011
Posts: 20
Rep Power: 6
LittleBart is on a distinguished road
Thanx for reply!

I've made a block as 3D bounding box around the air volume, then snapped the vertex to the corner points and linearized two top edges of the block to match the external surface of the geometry (it is seen on the second pic).

But then when I'm trying to use o-grid split, it always shows me "o-grid did not succeed" message and I'm not sure what to do, how to make o-grid properly?

I'll definitely look your posts through (doing now)...

thank you...
LittleBart is offline   Reply With Quote

Old   May 6, 2011, 11:36
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
Are you starting with a 3D block or just a surface block on the outside of the ff surface?

If you didn't start with a 3D block, try some of the hexa tutorials first before tackling this model or it will crush you
__________________
-----------------------------------------
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   May 6, 2011, 14:59
Default
  #5
New Member
 
LittleBart
Join Date: Jan 2011
Posts: 20
Rep Power: 6
LittleBart is on a distinguished road
started with "3D bounding box" block initialization. The external faces were ok, but still don't how to make o-grid inside. It looks like that on th pic attached when I'm trying.





still can't find the mentioned thread with similar case .. can you remember may the topic or the threader's name or some clue...
LittleBart is offline   Reply With Quote

Old   May 6, 2011, 16:03
Default Previous posts...
  #6
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 have collapsed the 3D block down to a wedge...

Don't do that.

Leave it as abox with three corners on corners and the 4th at the mid point of the arc.

Then Create the Ogrid with faces at the flat ends of the cylinder and the symmetry planes.

==================================

The previous thread was talking about "wind turbines"... I probably recommended "shifted periodic"... Some of the images had the name "Zaqie" on them... (that should give you some search terms)

here are some screen shots that were part of the previously posted threads.
Attached Images
File Type: jpg Rotor_1.jpg (94.6 KB, 137 views)
File Type: jpg ShiftedPeriodic2.jpg (46.9 KB, 138 views)
File Type: jpg Zaqie_19.jpg (94.0 KB, 114 views)
File Type: jpg Zaqie_16.jpg (79.3 KB, 105 views)
File Type: jpg Rotor_5.jpg (93.6 KB, 107 views)
__________________
-----------------------------------------
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   May 6, 2011, 16:16
Default
  #7
New Member
 
LittleBart
Join Date: Jan 2011
Posts: 20
Rep Power: 6
LittleBart is on a distinguished road
Many thanks. The pics are grate... I remember the second one from the meshing tutorial but shifted periodic is not clear to me yet. I'm working on that.

Have found "3D turbine blade modeling" thread, processing...

Will definitely try and post here.
LittleBart is offline   Reply With Quote

Old   May 13, 2011, 06:33
Default
  #8
New Member
 
LittleBart
Join Date: Jan 2011
Posts: 20
Rep Power: 6
LittleBart is on a distinguished road
Hello Simon and everyone who is interested in such a case!

Thanks to your instructions to Zaqie, I was able to deal with blocking of my geometry. But I'v faced some problems because of slightly different geometry than this of Zaqie's.

1. I have little bit different orientation of the blade because of small angles of attack and pretty twisted shape (angle difference between the root and the tip is deg). Because of that the strategy proposed for blocking has lead to some messy regions on the tip and on long-chord sections after I had snapped all edges of these splits to the curves.



2. But still, this blocking topology allowed my to build and tune premesh and I'm pretty satisfied with that. That's how I learned edge settings and splitting skills



But when I'm trying to calculate surface meshes it ignores the premesh and is trying to calculate according to the predefined edge params and global sizing. Furthermore, when I'm trying to change the global sizing for parts it seams to ignore that and still trying to calculate with very high density which I don't want to have. I left my comp for a day calculating the mesh and I got it after 15 hours of calculations and its sizing was about 1 mm for the air part when global setting 100. Global mesh coeff is 1.

So the question is how to force the settings I gained in the premesh to become settings of the surface mesher and volume as the next step?

Thank you,

LittleBart
LittleBart is offline   Reply With Quote

Old   May 14, 2011, 00:02
Default
  #9
Senior Member
 
Ahmed
Join Date: Mar 2009
Location: NY
Posts: 250
Rep Power: 9
Ahmed is on a distinguished road
http://www.ara.bme.hu/~lohasz/ICEM_t...blade_mesh.pdf
Ahmed is offline   Reply With Quote

Old   May 14, 2011, 05:01
Default
  #10
New Member
 
LittleBart
Join Date: Jan 2011
Posts: 20
Rep Power: 6
LittleBart is on a distinguished road
Thank you for reply and for the tutorial, it really was really helpful!

But it doesn't really show the transition from premesh settings to mesh params. Or I'm just do not understand the concept of premesh itself. Is it really like separate from the mash-tab mash and I don't need to calculate surface and volume meshes if I have pre-mesh done?
Here little context to make myself clear. I'm doing this mesh for my blade study which I want to do in CFX and therefore I want to output the mesh into CFX-readable file with separate regions for BCs.
So, do I need to calculate volume mesh on the mesh tab or I can just make premesh in bocking tab and then just output it into CFX file.


My apologies once again for probably stupid question but I'm really very new in it.
LittleBart is offline   Reply With Quote

Old   May 15, 2011, 20:37
Default Convert to unstructured mesh...
  #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
Yes, the premesh already has everything (surface and volume mesh), you just need to convert it into the right format for your solver. Check the quality while in premesh, make sure everything is good and then right click on Premesh to output to unstructured mesh...

Then do unstructured mesh checks, etc.

This unstructured mesh can then be output to CFX...

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   May 17, 2011, 09:20
Default
  #12
New Member
 
LittleBart
Join Date: Jan 2011
Posts: 20
Rep Power: 6
LittleBart is on a distinguished road
Hi !

Thanks Simon for help and patience! Little more question on unstructured mesh - will it preserve regions for inlet/outlet surfaces as separate 2D regions for CFX BCs ?


Btw, now I feel like ready for scripting, thanx to you .
LittleBart is offline   Reply With Quote

Old   May 17, 2011, 10:46
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
That is what PARTS are for...

If the blocking face is associated with (projects to) the geometry of part "INLET" then its premesh and subsequent unstructured mesh, will also be in the part "inlet". This is just the default behavior. When you output, the output will also have the faces in the inlet part ready for your bocos.

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   June 22, 2011, 09:50
Default
  #14
New Member
 
LittleBart
Join Date: Jan 2011
Posts: 20
Rep Power: 6
LittleBart is on a distinguished road
Hello everyone!

After long vacations I'm again face to face with my blade problem and again asking for your help. Thank to Simon now I can build relatively stable and adjustable unconstructed mesh for the blade. And now I'm trying to model the problem in CFX (13). Actualy, this problem is my old one, the one that made me turning to ICM CFD and master the Mesh Skill. Thats because I thought that the results I've received are bad because of the bad mesh quality.

In my previous problem I've made a blade geometry and meshed it with CFX Mesh. The CFX problem had the following parameters:


CF:
Z - rotational axis, X -

Domain:
1. Air - fluid domain - ref. pressure = 1 atm; fluid - air; CF - rotational cf with 13 rad/s velocity (expected velocity of the modeled blade at 10 m/s wind).
2. Blade - solid domain (Aluminum).



BCs:
1. Inlet - inlet surface of the air volume - Velocity = 10 m/s
2. Outlet - outlet surface of the air volume - Static pressure = 0 atm. (= ref. pressure)
3. External surface - wall - no slip wall (FF)
4. Side surfaces - domain interface Air/Air - rotational periodicity
5. Air/Blade - domain interface - fluid/solid - frozen rotor

That was the model. And these are the results:



But my main question is quality of the blade. In order to answer this question I've tried to evaluate the overall Lift Force of the blade and, as a result, Momentum or Torque. In order to compare this force with the one calculated with beam element theory.

I've calculated this with an expression

aveInt(Force X)@Blade_surf

and got the value of 13.4 N

Which made me sad.

And now I've made the same procedure with new mesh and result is 12.5 N which is proximately the same.
to be continue...
LittleBart is offline   Reply With Quote

Old   June 23, 2011, 03:51
Default
  #15
New Member
 
LittleBart
Join Date: Jan 2011
Posts: 20
Rep Power: 6
LittleBart is on a distinguished road
yeaah.. I'll better repost it to the CFX section
LittleBart is offline   Reply With Quote

Old   October 7, 2012, 10:43
Default
  #16
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: 38
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
Yes, the premesh already has everything (surface and volume mesh), you just need to convert it into the right format for your solver. Check the quality while in premesh, make sure everything is good and then right click on Premesh to output to unstructured mesh...

Then do unstructured mesh checks, etc.

This unstructured mesh can then be output to CFX...

Simon
Is there any difference between the quality in pre-mesh and unstructured mesh (which is also created from that premesh)?
Far is offline   Reply With Quote

Old   October 8, 2012, 03:44
Default
  #17
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
I think the pre-mesh doesn't check the quality for quads.
But the quality for unstructured mesh does check the quality for quads, unless you specify not to.
BrolY is offline   Reply With Quote

Old   October 9, 2012, 17:53
Default
  #18
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
Yea, depending on the metric, there may be some small differences that you will see, and some metrics are only available in one, but not the other. Or as BrolY says, the unstructured quality can include the quality of Quads or other element types.

The important thing is just to be reasonably confident that your mesh is good enough for your solver before you bother moving the files around.
__________________
-----------------------------------------
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   October 10, 2012, 05:51
Default
  #19
Member
 
Tamil Nadu
Join Date: Oct 2012
Posts: 44
Rep Power: 4
nkme2007 is on a distinguished road
Hello All,

I want to do analysis of heat transfer from water flowing through pipes submerged inside concrete. I am modelling in GAMBIT and wish to analyse it on Ansys FLUENT.

Can anybody help me out, how to model and simulate?

Does any tutorials exist?
nkme2007 is offline   Reply With Quote

Old   October 10, 2012, 09:20
Default
  #20
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
@ nkme2007

Quote:
I am modelling in GAMBIT
You hijacked a bunch of different threads with your question, please don't do that. it is annoying. Particularly when you jump on threads for ICEM CFD or ANSYS Meshing (we don't know much about Gambit anyway)...

Just create your own thread or possibly find a Gambit thread with a similar question and replay to that.

But in the end, you probably won't get any help anyway because your question is too broad, you may as well say "how do I do CFD?" Try some Fluent tutorials and start on your project. CFD-Online helps those who help themselves.
Far and BrolY 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

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
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
Gambit: Volume Meshing fluentnoob ANSYS Meshing & Geometry 4 May 20, 2009 05:21
Volume split -- Meshing Kantipudi FLUENT 0 July 27, 2008 12:18
Question on blade meshing Jeffrey CFX 0 March 7, 2008 18:13
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 20:16.