# [ICEM] How to tackle this problem?

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

September 20, 2012, 02:17
How to tackle this problem?
#1
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
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
 2.jpg (98.0 KB, 56 views) 3.jpg (94.8 KB, 48 views)

September 20, 2012, 02:55
#2
New Member

R. Manigandan
Join Date: Jul 2012
Location: Pune
Posts: 5
Rep Power: 5
Quote:
 Originally Posted by cfd seeker 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

September 20, 2012, 04:37
#3
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
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?

 September 20, 2012, 08:50 #4 Super Moderator     Ghazlani M. Ali Join Date: May 2011 Location: Canada Posts: 1,291 Blog Entries: 23 Rep Power: 20 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

 September 20, 2012, 09:04 #5 Super Moderator     Ghazlani M. Ali Join Date: May 2011 Location: Canada Posts: 1,291 Blog Entries: 23 Rep Power: 20 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

September 20, 2012, 10:27
#6
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
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

 September 20, 2012, 10:31 #7 Member   Yon Han Chong Join Date: Jun 2012 Posts: 77 Rep Power: 5 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.

September 20, 2012, 10:41
#8
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
Quote:
 Originally Posted by yonchong 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

 September 20, 2012, 10:51 #9 Member   Yon Han Chong Join Date: Jun 2012 Posts: 77 Rep Power: 5 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.

September 20, 2012, 12:26
#10
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
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

 September 22, 2012, 19:53 #11 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,662 Blog Entries: 1 Rep Power: 35 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

September 23, 2012, 02:18
#12
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
Quote:
 Originally Posted by PSYMN 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

September 23, 2012, 08:59
#13
Super Moderator

Ghazlani M. Ali
Join Date: May 2011
Posts: 1,291
Blog Entries: 23
Rep Power: 20
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

September 23, 2012, 18:52
#14
Senior Member

Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
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.
__________________
-----------------------------------------

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey

September 24, 2012, 09:50
#15
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
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?

 September 24, 2012, 11:13 #16 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,662 Blog Entries: 1 Rep Power: 35 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

 September 25, 2012, 03:39 #17 Senior Member   AB Join Date: Sep 2009 Location: France Posts: 323 Rep Power: 12 You are right, German Police is awful diamondx likes this.

September 25, 2012, 05:47
#18
Super Moderator

Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Quote:
 Originally Posted by BrolY You are right, German Police is awful
Are they going to teach us unstructured meshing using ICEM

 September 25, 2012, 09:09 #19 Super Moderator     Ghazlani M. Ali Join Date: May 2011 Location: Canada Posts: 1,291 Blog Entries: 23 Rep Power: 20 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

 October 3, 2012, 08:31 #20 New Member   R. Manigandan Join Date: Jul 2012 Location: Pune Posts: 5 Rep Power: 5 Contact me in my mail ID manirainbow61@gmail.com i can help u from thr.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43 JFDC FLUENT 1 July 11, 2011 05:59 Se-Hee CFX 2 June 10, 2007 06:29 ParodDav CFX 5 April 29, 2007 19:13 Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52

All times are GMT -4. The time now is 01:52.