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

[ICEM] How to tackle this problem?

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

Like Tree8Likes
  • 1 Post By PSYMN
  • 1 Post By PSYMN
  • 1 Post By BrolY
  • 1 Post By Far
  • 4 Post By diamondx

Reply
 
LinkBack Thread Tools Display Modes
Old   September 20, 2012, 02:17
Default How to tackle this problem?
  #1
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 412
Rep Power: 11
cfd seeker is on a distinguished road
I need to mesh the simple rectangular wing using Unstructured Mesh. I have to set finer node distributions near the leading edge all along the span. There is only one surface on suction side(upper), one surface on the pressure side(lower) and one surface in the wing tip region. I have set the finer node distribution on wing root curves and wing tip curves(shown in images) to get finer bunching on the leading edge but only these curves(wing root curve and wing tip curve) are respecting the finer node distribution not the whole span(from root to tip) as shown in attached images. I think I need to do some geometry operations on the upper and lower side of wing to tackle this problem but I have no idea about these operations. So how to tackle this? Thanks
Waiting for expert opinions of Diamondx and Simon

Regards
Attached Images
File Type: jpg 2.jpg (98.0 KB, 56 views)
File Type: jpg 3.jpg (94.8 KB, 48 views)
cfd seeker is offline   Reply With Quote

Old   September 20, 2012, 02:55
Default
  #2
New Member
 
R. Manigandan
Join Date: Jul 2012
Location: Pune
Posts: 5
Rep Power: 4
Manigandan is on a distinguished road
Quote:
Originally Posted by cfd seeker View Post
I need to mesh the simple rectangular wing using Unstructured Mesh. I have to set finer node distributions near the leading edge all along the span. There is only one surface on suction side(upper), one surface on the pressure side(lower) and one surface in the wing tip region. I have set the finer node distribution on wing root curves and wing tip curves(shown in images) to get finer bunching on the leading edge but only these curves(wing root curve and wing tip curve) are respecting the finer node distribution not the whole span(from root to tip) as shown in attached images. I think I need to do some geometry operations on the upper and lower side of wing to tackle this problem but I have no idea about these operations. So how to tackle this? Thanks
Waiting for expert opinions of Diamondx and Simon

Regards
In this problem you want to change the value
1. in Global mesh parameter -> Volume meshing parameters->reduce the edge criterion try it once or
2. sweep the surface mesh by Edit mesh-> Extrude mesh-> select mesh-> Give volume element name->give ->side surface mesh name->topsurface mesh name
on tht time you can the on two side will be tri surface mesh and top and bottom side quad mesh on it
Manigandan is offline   Reply With Quote

Old   September 20, 2012, 04:37
Default
  #3
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 412
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
2. sweep the surface mesh by Edit mesh-> Extrude mesh-> select mesh-> Give volume element name->give ->side surface mesh name->topsurface mesh name
on tht time you can the on two side will be tri surface mesh and top and bottom side quad mesh on it
Didn't get this point?
cfd seeker is offline   Reply With Quote

Old   September 20, 2012, 08:50
Default
  #4
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
what do you mean by geometry reparation, splitting the upper and bottom surfaces ?? i'm not much of an expert when it comes to unstructured mesh ! i can help you with geometry changing tough
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 20, 2012, 09:04
Default
  #5
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
i have a memory of a similar thread, may be you can find if make and advanced search, filter prefix "icem" and look for wing unstructured.... may be ...
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 20, 2012, 10:27
Default
  #6
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 412
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
hat do you mean by geometry reparation, splitting the upper and bottom surfaces ??
Yup by geometry operations I mean making many surfaces out of a single and also make extra curves on the surfaces for your needs....any suggestions?

Quote:
i'm not much of an expert when it comes to unstructured mesh
I myself don't like this but for a particular project of Flapping Wing Analysis I have it use it
cfd seeker is offline   Reply With Quote

Old   September 20, 2012, 10:31
Default
  #7
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
Try adding density to the leading edge line.

Mesh -> Create Mesh Density

In fact, if you go to the Ansys help on Create Mesh Density, it has leading edge on wing example. In that example, the density line was created in front of the leading edge but, in your case, you can just use the line dividing the upper and lower surface.
yonchong is offline   Reply With Quote

Old   September 20, 2012, 10:41
Default
  #8
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 412
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Originally Posted by yonchong View Post
Try adding density to the leading edge line.

Mesh -> Create Mesh Density

In fact, if you go to the Ansys help on Create Mesh Density, it has leading edge on wing example. In that example, the density line was created in front of the leading edge but, in your case, you can just use the line dividing the upper and lower surface.
If I am not wrong the Mesh Density Box only affects the Volume Mesh not the Surface Mesh isn't it? I am having problem with the Surface Mesh
cfd seeker is offline   Reply With Quote

Old   September 20, 2012, 10:51
Default
  #9
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
If you use the patch independant option the shell mesh will be affected as ICEM uses Octree volume mesher to create volume and surface mesh together and delete the volume mesh to leave the surface mesh.

If you use the patch dependant option then the density box will not do anything as the shell mesh is generated using surfaces.
yonchong is offline   Reply With Quote

Old   September 20, 2012, 12:26
Default
  #10
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 412
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
If you use the patch independant option the shell mesh will be affected as ICEM uses Octree volume mesher to create volume and surface mesh together and delete the volume mesh to leave the surface mesh
Thanks nice information
cfd seeker is offline   Reply With Quote

Old   September 22, 2012, 19:53
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
Some users like to run iso parametric curves along curving surfaces like this (or along fillets) to control the way the nodes fall... I am guessing that is what you are looking for.

Go into Geometry (tab) => Create/Modify Curves => Create Iso-Parametric curve... (or something similar to that, I don't have ICEM up to check the command)

An iso parametric curve is one that follows the UV space of a surface. If you set it to 0.5, it will create a curve exactly down the middle of the surface. In your case, you might want to try 0.05 (or 0.95) to get it just 5 percent from the edge... You may even want to create a few of these near each other...

If the curves are perpendicular to what you expect, then switch between u and v.

Then when you generate octree tetra mesh, it will be controlled by the curves... It is sort of like forcing the tetras to line up along the leading edge of the wing.

The downside is that the curves also constrain the smoother, etc. so you could have some reduced quality (but still good enough).

Post a pic when you are done so people can see what this did for you.
Far 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   September 23, 2012, 02:18
Default
  #12
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 412
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Some users like to run iso parametric curves along curving surfaces like this (or along fillets) to control the way the nodes fall... I am guessing that is what you are looking for.

Go into Geometry (tab) => Create/Modify Curves => Create Iso-Parametric curve... (or something similar to that, I don't have ICEM up to check the command)

An iso parametric curve is one that follows the UV space of a surface. If you set it to 0.5, it will create a curve exactly down the middle of the surface. In your case, you might want to try 0.05 (or 0.95) to get it just 5 percent from the edge... You may even want to create a few of these near each other...

If the curves are perpendicular to what you expect, then switch between u and v.

Then when you generate octree tetra mesh, it will be controlled by the curves... It is sort of like forcing the tetras to line up along the leading edge of the wing.

The downside is that the curves also constrain the smoother, etc. so you could have some reduced quality (but still good enough).

Post a pic when you are done so people can see what this did for you.
Yah Friday evening I was trying something like that but I was projecting curves on the already existing surface, that option seems to divide the surface into two parts by creating a curve at 50% location(using leading and trailing edge curves), again I applied the same process on the two parts separately to get four parts in total, then I deleted the main surface and with the help of created curves I made separate surfaces but this process was not giving me my desired result as I want a separate surface 30% from the leading edge. of course I don't have pics or geometry here to post my effort but I will post some pics what I was doing and will also try to implement what you said. Thanks
cfd seeker is offline   Reply With Quote

Old   September 23, 2012, 08:59
Default
  #13
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
Quote:
separate surface 30% from the leading edge
Another thing to try, i usually go to the create point option.
there is a very handy tool there, you can create point depending on a parameter of a curve, 30%=0.3 50%=0.5. when you create your point, you can project that point to several other parallel edges again using the option "project point on curve". once projected, create an edge with those point, then slice the surface using those edge in the option "split surface using edge" i hope it can help.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 23, 2012, 18:52
Default
  #14
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
Quote:
curve at 50% location
Iso parametric doesn't have to be 50%, you can use any percentage you want. And it doesn't have to cut the other surface... Just don't build topo...

You don't need to cut the surfaces for it to work.
__________________
-----------------------------------------
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 24, 2012, 09:50
Default
  #15
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 412
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Then when you generate octree tetra mesh, it will be controlled by the curves...
octree tetra mesh using Patch Dependent or Patch Independent method for surface mesh?
cfd seeker is offline   Reply With Quote

Old   September 24, 2012, 11:13
Default
  #16
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
Octree tetra uses the patch independent method... In fact, Octree tetra starts with the volume mesh (it is a top down method) and then figures out the surface mesh from there.

When you start with a patch conforming method, it actually generates the patch independent mesh as part of its process and then dumps it to make the octree volume mesh conformal with the surface mesh. This really combines the worst of both worlds, like having German Police and French Mechanics, instead of the other way around. There isn't really much good reason to do all the work required to get a good patch conforming surface mesh if you are going to fill it with Octree... The one good exception is when you have just a few patch conforming surfaces (perhaps coming from an adjacent model) that you want the octree to align with. Octree would then create all the other surface mesh that you need...

But in the end, I might still delete the octree mesh, smooth the surface mesh (alternating rounds of laplace and regular smoothing, ending with regular smoothing) and regenerate the volume mesh with a Delaunay Fill (with the TGlib and AF options).

In your case, patch conforming mesh on the difficult thin surfaces may be easier than octree (PI surface mesh) and then you can fill with delaunay.

If you have trouble with other surfaces in the model, just skip them with PI, and use Octree to capture them...
Far 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   September 25, 2012, 03:39
Default
  #17
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
You are right, German Police is awful
diamondx likes this.
BrolY is offline   Reply With Quote

Old   September 25, 2012, 05:47
Default
  #18
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
Quote:
Originally Posted by BrolY View Post
You are right, German Police is awful
Are they going to teach us unstructured meshing using ICEM
BrolY likes this.
Far is offline   Reply With Quote

Old   September 25, 2012, 09:09
Default
  #19
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
Broly, always there to start spaming threads and diverting subject, keep up the good work
Far, always there to support him.
Far, PSYMN, BrolY and 1 others like this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   October 3, 2012, 08:31
Default
  #20
New Member
 
R. Manigandan
Join Date: Jul 2012
Location: Pune
Posts: 5
Rep Power: 4
Manigandan is on a distinguished road
Contact me in my mail ID manirainbow61@gmail.com i can help u from thr.
Manigandan 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
UDF compiling problem Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43
Gambit - meshing over airfoil wrapping (?) problem JFDC FLUENT 1 July 11, 2011 05:59
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13
Is this problem well posed? Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52


All times are GMT -4. The time now is 16:06.