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

[ICEM] ICEM Hexa meshing tutorial - Wing with sharp trailing edge

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 1, 2013, 06:38
Default
  #21
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
For propeller blade, general strategy is same.
Far is offline   Reply With Quote

Old   October 1, 2013, 10:15
Default
  #22
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
Actually, it depends on the shape of the blade... If it has a rounded tip with a sharp edge, it will be more difficult to block. I really lean toward Multizone for those.
__________________
-----------------------------------------
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 8, 2013, 05:28
Default Working on similar problem but want your help in a different context..
  #23
Member
 
Join Date: Jan 2010
Posts: 53
Rep Power: 7
mariachi is on a distinguished road
Hi Far,
Referring to your tutorial of "Hexa meshing with sharp trailing edge", in this you have used 3D blocking to mesh the complete domain. The other approach can be to generate a regular mesh by setting Mesh...> Global Mesh parameter etc etc which will generate unstructured mesh i suppose.

I want to know whether combination of both these methods (in the same mesh) is possible or not? If YES, then please elaborate...

Just to explain the scenario: I have a geometry of wing+fuselage and i have meshed all of its surfaces by "2D Surface Blocking". Once done, i converted it into 'unstructured mesh' by right clicking on 'pre mesh'. No issues so far. In this way i get a very good structured mesh on all faces of my geometry and put on prism layer as well. Now i want to fill rest of my domain with 'tri' elements which should start growing from the ''existing mesh'' on geometry surface and gradually coarsen out towards domain boundaries. But, its not happening.

Hoping for a quick reply...
mariachi is offline   Reply With Quote

Old   October 8, 2013, 11:18
Default
  #24
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
Sure, but you want to avoid an overlap...

After generating the unstructured mesh from Hexa, you can convert the surface of that to facets (Edit (menu) => Mesh to Facets). Then place a material point the the region you want to mesh and generate your unstructured mesh. Then you can merge the meshes across the boundary and delete the boundary elements...

Another option is "MultiZone" hexa which creates unstructured blocks.
__________________
-----------------------------------------
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 8, 2013, 12:19
Default
  #25
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
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:
Sure, but you want to avoid an overlap...

After generating the unstructured mesh from Hexa, you can convert the surface of that to facets (Edit (menu) => Mesh to Facets). Then place a material point the the region you want to mesh and generate your unstructured mesh. Then you can merge the meshes across the boundary and delete the boundary elements...

Dear Simon

does this mesh represent the method you have just explained?

Far is offline   Reply With Quote

Old   October 8, 2013, 13:05
Default
  #26
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, now I see your image...

No, that is just surface meshing. This is simply hexa mesh and then conformal shell meshing with the option to respect the line elements.

I thought this user was interested in 3D meshing with a hexa boundary layer around the wing and then unstructured tetra beyond that.
__________________
-----------------------------------------
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 8, 2013, 13:17
Default
  #27
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
mariachi is interested in the volume mesh. But as he said he is using surface blocking (hexa layers on surfaces) and then he wants to grow prisms and volume tetra mesh. So I thought that this image is closely related to his requirements and the method explained by you.
Far is offline   Reply With Quote

Old   October 8, 2013, 13:19
Default
  #28
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
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:
No, that is just surface meshing. This is simply hexa mesh and then conformal shell meshing with the option to respect the line elements.

Would you like to please explain the method in bit detail ? I am not able to grasp the idea and have no idea how to proceed...
Far is offline   Reply With Quote

Old   October 8, 2013, 13:20
Default
  #29
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
Yea, you are probably right. At first I focused on the "3D" in the first paragraph, but reading it again...
__________________
-----------------------------------------
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 8, 2013, 13:27
Default
  #30
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
Quote:
Originally Posted by Far View Post
Would you like to please explain the method in bit detail ? I am not able to grasp the idea and have no idea how to proceed...

Oh, I am typing too fast for my own good. I was thinking it was the method where you use surface blocking first and then patch dependent surface meshing of adjacent surfaces with the option to respect line elements so everything would be conformal...

But for those images you posted (the rear wing of a Formula 1 car that I did years ago), I actually did a different method.

In that case, I generated a regular tetra mesh of the volume region. Then I went in and generated hexa blockings within the wings and generated "solid" mesh inside them. This gave me a nice an-isotropic quad mesh along the surface of the wings. I didn't bother worrying about the quality of the hexas inside, so no need to worry about Ogrids or anything... Just a hexa box inside the wing with the edges associated.

Then I just merged the Hexa meshes with the tetra meshes. Follow the rules of mesh merging (shared perimeter, shared surfaces in separate parts, similar size meshes, etc.) and it works well.

Then I deleted the volume mesh (all the hexas inside the wings, the tetras and pyramids outside the wings), and generated prisms and a new tetra volume mesh using bottom up methods.

Did I not explain it all in the ppt where you got that screen shot?
__________________
-----------------------------------------
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 8, 2013, 13:38
Default
  #31
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
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

Did I not explain it all in the ppt where you got that screen shot?
This screen shot is from the Simon's tip and tricks https://dl.dropboxusercontent.com/u/...Tricks2010.pdf


Quote:
Originally Posted by PSYMN View Post

h, I am typing too fast for my own good. I was thinking it was the method where you use surface blocking first and then patch dependent surface meshing of adjacent surfaces with the option to respect line elements so everything would be conformal...

But for those images you posted (the rear wing of a Formula 1 car that I did years ago), I actually did a different method.

In that case, I generated a regular tetra mesh of the volume region. Then I went in and generated hexa blockings within the wings and generated "solid" mesh inside them. This gave me a nice an-isotropic quad mesh along the surface of the wings. I didn't bother worrying about the quality of the hexas inside, so no need to worry about Ogrids or anything... Just a hexa box inside the wing with the edges associated.

Then I just merged the Hexa meshes with the tetra meshes. Follow the rules of mesh merging (shared perimeter, shared surfaces in separate parts, similar size meshes, etc.) and it works well.

Then I deleted the volume mesh (all the hexas inside the wings, the tetras and pyramids outside the wings), and generated prisms and a new tetra volume mesh using bottom up methods.

1. So you are making solid hexa mesh inside with nice quad surface on wing surfaces?

2. when we grow the tetra mesh on hexa mesh, will there be any difficulty?

3. You are merging the volume meshes, but effectively we are merging surface mesh (as we will discard volume mesh inside wings) with volume mesh . That is pretty very smart trick...

4. Is there any special consideration while making this mesh or it is just simple merging of volume meshes with usual settings?
Far is offline   Reply With Quote

Old   October 8, 2013, 13:45
Default
  #32
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Simon : Do you make meshes in ICEM? It looks like they are made using paint and brush so artistic and beautiful
Far is offline   Reply With Quote

Old   October 9, 2013, 00:39
Default
  #33
Member
 
Join Date: Jan 2010
Posts: 53
Rep Power: 7
mariachi is on a distinguished road
Hey PSYMN and Far: First of all thanks for your prompt replies and discussion. But my query is still hanging in there...

Let me post an arbitrary picture for discussion. There is a small red cube inside a larger cube as you can see. Now i want to mesh all the red faces by using PARTICULARLY "2D Surface Blocking". After that, i will grow Prism layer from all these red faces. That being done, now i want to fill the rest of big cube with Tri elements which should start growing from the ALREADY "existing surface mesh" on all red faces having "Prism layer" ALREADY grown on it. This is only possible if the nodes of first layer of "Tri elements" are the same as the last layer of Prism layer. But this is not happening in my case. And it is because in surface blocking, we actually define the node count etc for all Edges of Blocks and then associate these Edges to Curves. So probably the Tri mesher is not knowing about these ALREADY created nodes because these are actually on the Edges and not on Curves.

So is there any way to tell ICEM to get the node count and node spacing etc information from those already defined for the Edges during blocking? If YES, than please elaborate...

Regards,
Attached Images
File Type: jpg untitled.JPG (18.6 KB, 9 views)
mariachi is offline   Reply With Quote

Old   October 9, 2013, 03:13
Default
  #34
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
@mariachi
you want to grow prisms on the quad surface mesh?? strange isn't it....

normally we use quad surface mesh and hexa elements in the confined region around the body to capture the Boundary Layer effects and then fill the rest of the volume with the tetra elements to make what is known as "Hybrid Mesh". If you are looking for a thing like this then "ICEM Multizone" is the answer. If you don't know what is it the consult the thread I mean to say we gain nothing after growing prisms from the quad surface mesh. If you want to take advantage from Structured Boundary layer mesh then follow the guidelines in the above mentioned thread.

Hope it helps you.

Regards
cfd seeker is offline   Reply With Quote

Old   October 21, 2013, 05:46
Default
  #35
Member
 
Join Date: Jan 2010
Posts: 53
Rep Power: 7
mariachi is on a distinguished road
@cfdseeker

Thanks for the tip. I'll explore this "Multizone" option on my geometry and see how it goes. Will get back to you...
mariachi 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] ICEM Hexa Meshing Automation Haasini ANSYS Meshing & Geometry 1 April 24, 2012 22:46
[ANSYS Meshing] Icem cfd - hexa meshing arunkumarnd ANSYS Meshing & Geometry 9 April 12, 2012 05:47
[ICEM] Wing Trailing Edge Prism and prism width srad ANSYS Meshing & Geometry 2 March 12, 2012 10:10
ICEM aircraft mesh trailing edge difficulty MontyR ANSYS Meshing & Geometry 4 July 23, 2011 21:46
Structured mesh of a 3d sharp trailing edge Gilles Main CFD Forum 2 May 23, 2008 13:23


All times are GMT -4. The time now is 12:17.