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

[ICEM] How to generate sunstructured "all-tri patch-dependant" surface mesh in ICEM?

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

Like Tree4Likes
  • 3 Post By PSYMN
  • 1 Post By diamondx

Reply
 
LinkBack Thread Tools Display Modes
Old   December 3, 2010, 06:18
Default How to generate sunstructured "all-tri patch-dependant" surface mesh in ICEM?
  #1
New Member
 
jash's Avatar
 
Jason Sherlock
Join Date: Sep 2010
Posts: 2
Rep Power: 0
jash is on a distinguished road
Hi all,
Typically when I am running alpha-traverse studies, I am creating an unstructured symmetry mesh of my geometry (left half of the geometry, left half of the far field, and a symmetry plane). I have been using patch-independant surface meshing to create the surface mesh, then advancing-front (smooth) + prisms to fill in the volume mesh.

While I am quite happy with the surface mesh on the aircraft, I haven't been happy with the surface mesh generated on the symmetry plane. Since patch-independant surface meshing is using octree to generate the surface triangles, the growth rate on the symmetry plane going from the aircraft to the farfield is very octreeish: aggressive and "boxy". I haven't found a parameter that smooths this out in a nice way. The result is that the advancing-front volume mesh is constrained near the symmetry plane in a way that looks "odd/wrong" when compared to the volume growth away from the symmetry plane (see attached mesh cut-plane, this is looking down the length of the geometry, symmetry plane terminates the mesh on the left side, farfield is off screen on the right side).

I've got a feeling that patch-dependant surface meshing is going to generate a surface mesh on the symmetry plane that is more compatible with the advacing-front volume mesh, but I haven't completely gotten the hang of it. Parts of the surface mesh come out beautiful (just what I am hoping for) and others come out twisted. I've checked my surface normals and they are fine.

So my questions are:
1.)Is there a tutorial describing how to use patch-dependant surface meshing for unstructured meshes (I haven't been able to locate one in the official Ansys tutorials)?
or
2.)Is there an other way to create a surface mesh on the symmetry plane that has a smoother growth ratio going from the aircraft to the farfield?

Thanks for any help!
Attached Images
File Type: jpg cutplane.jpg (91.7 KB, 135 views)
jash is offline   Reply With Quote

Old   December 4, 2010, 14:08
Default Laplace...
  #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
There is a tutorial about patch conforming surface mesh on an aircraft, but I always found it more work... (The jist is that you must build topo first and set up sizes on all the curves. Then use the patch dependent surface mesher. You can just mesh a single surface, such as the symmetry plane and then use that when you Octree, or you could mesh the whole thing with patch dependent)

I can dig it up for you if you really want it.

In the mean time, I have another suggestion that is easier to implement...

Generate your Octree Mesh... (no need for Delaunay yet).

Delete all the volume elements (Delete Mesh, then select All volume elements with the selection tool bar). These will be deleted to replace with delaunay eventually, but if you get rid of them now, it is easier to smooth.

Then smooth the heck out of the surface mesh using the Laplace option. Make sure to turn on that laplace checkbox option... Try 50 iterations up to 0.6 or something like that. Laplace tries to smooth out angles between elements and the transition (surface area change) between elements. It ends up looking very "delaunay". But it doesn't focus on individual element quality, so... One more round of regular smoothing (10 iterations up to 0.4) (without Delaunay) to finish up.

Take a look at the surface on the symmetry plane. It should be pretty good.

Then go back to compute mesh => Delaunay to fill the volume and continue on with your regular process...



-----------------------------------------
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
Far, sharonyue and ank86it like this.
PSYMN is offline   Reply With Quote

Old   December 4, 2010, 16:23
Default
  #3
New Member
 
jash's Avatar
 
Jason Sherlock
Join Date: Sep 2010
Posts: 2
Rep Power: 0
jash is on a distinguished road
Excellent, thanks! I've never tried going that extreme on the smoothing options. Looking forward to trying this out on monday.
jash is offline   Reply With Quote

Old   April 19, 2013, 07:40
Default how to generate a mesh
  #4
New Member
 
tita
Join Date: Apr 2013
Posts: 27
Rep Power: 4
ok___ko is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
There is a tutorial about patch conforming surface mesh on an aircraft, but I always found it more work... (The jist is that you must build topo first and set up sizes on all the curves. Then use the patch dependent surface mesher. You can just mesh a single surface, such as the symmetry plane and then use that when you Octree, or you could mesh the whole thing with patch dependent)

I can dig it up for you if you really want it.

In the mean time, I have another suggestion that is easier to implement...

Generate your Octree Mesh... (no need for Delaunay yet).

Delete all the volume elements (Delete Mesh, then select All volume elements with the selection tool bar). These will be deleted to replace with delaunay eventually, but if you get rid of them now, it is easier to smooth.

Then smooth the heck out of the surface mesh using the Laplace option. Make sure to turn on that laplace checkbox option... Try 50 iterations up to 0.6 or something like that. Laplace tries to smooth out angles between elements and the transition (surface area change) between elements. It ends up looking very "delaunay". But it doesn't focus on individual element quality, so... One more round of regular smoothing (10 iterations up to 0.4) (without Delaunay) to finish up.

Take a look at the surface on the symmetry plane. It should be pretty good.

Then go back to compute mesh => Delaunay to fill the volume and continue on with your regular process...



-----------------------------------------
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
Hi, I just start to learn CFD. Now, I have such a problem, I have already draw a geometry in ICEM, how could I block it and mesh? Could you give me your email address do that I could send you my specific question?
Thanks
ok___ko is offline   Reply With Quote

Old   May 30, 2013, 11:30
Default triangular mesh generation
  #5
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
Hello friends. I want to make triangular mesh around 2D airfoil. By default it makes quadrilateral. How should I proceed for tri grid? Please help
star is offline   Reply With Quote

Old   May 30, 2013, 14:08
Default
  #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
What tool are you using? if ICEM CFD, go to the mesh tab and change the global settings for shell meshing... Or just go to Compute mesh and ask for all tri instead of quad dominant.
__________________
-----------------------------------------
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 31, 2013, 06:21
Default
  #7
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
Thanks PSYMN for your reply.
Yes I am using ICEM. Here I am posting a quick process of mine. I created airfoil and farfield (surface created) curves. Then I changed Shell meshing parameters to "All tri" type. Next, I created block and set some edge parameters under premesh parameters but it still create quad grid.. Also there is no option for 'All tri' under compute mesh... I 'll be really thankful for your help.
Here I attached the type of mesh which I want to generate..
Attached Images
File Type: jpg mesh.jpg (31.7 KB, 46 views)
star is offline   Reply With Quote

Old   May 31, 2013, 11:01
Default
  #8
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
Those shell meshing parameters are for shell meshing, not for blocking...

You probably just need unstructured shell meshing which you generate with the mesh tab => Compute mesh. Look for a shell meshing tutorial because you will also need to learn how to set the curve params, 2D inflation, etc.

If you actually want blocking, you can go to edit block to change the block type from mapped to free (mapped is the default). You can also set the free block to any type of unstructured mesh you want... All tri in your case. You probably want the gambit pave all tri for the smoothest mesh. Note, if you are using blocking, you will need to block out the airfoil interactively or use 2D surface blocking if you want it done automatically. Placing a single 2D block will not capture the airfoil.

Best regards,
__________________
-----------------------------------------
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 31, 2013, 12:14
Default
  #9
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
Thanks PSYMN for your suggestion. I am now reading tutorial relating to shell meshing. I think for unstructured mesh I will not need blocking. Am I right?


Kind Regards
star is offline   Reply With Quote

Old   May 31, 2013, 13:32
Default
  #10
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:
I think for unstructured mesh I will not need blocking. Am I right?
yes, you are right
PSYMN likes this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 1, 2013, 03:09
Default
  #11
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
Dear friends Diamondx and PSYMN, I started learning generating unstructured mesh around airfoil ICEM but one initial problem for me is that after computing it gives me some warning that there is hole in domain. I think it assume airfoil as hole because the mesh ignores the airfoil curves as boundaries and also crosses it. How should I specify the airfoil as walls? please help..

Kind Regards
star is offline   Reply With Quote

Old   June 1, 2013, 10:56
Default
  #12
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
hello Star,
To specify the airfoil as wall, name those curve "airfoil_wall", then in the output menu specify them as wall. First you have to fix the hole error...
would you mind sharing your project via dropbox. i can take a look at it this weed end...
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 1, 2013, 12:37
Default
  #13
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
Thanks diamondx for your reply. By wall i mean to make it solid boundary. I think i can go to output after completing my mesh. I am at the initial stage of mesh generation. I posted here photo of my mesh. you can see what I mean. My 2 main questions regarding my requirements are
1) how to make the airfoil as boundary so that the mesh lines couldn't pass it.
2) how to create more/dense mesh near airfoil boundary.

kind Regards
Attached Images
File Type: jpg Mesh.jpg.jpg.jpg (96.4 KB, 28 views)

Last edited by star; June 1, 2013 at 13:40.
star is offline   Reply With Quote

Old   June 1, 2013, 22:13
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
2) just set a smaller mesh size on the curves...

1) Delete the surface inside the airfoil and mesh won't generate there.
__________________
-----------------------------------------
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 2, 2013, 01:17
Default
  #15
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
Thanks PSYMN, your points were much helpful. I trimmed the surface inside airfoil and now it's better...
star is offline   Reply With Quote

Old   June 20, 2013, 13:27
Default
  #16
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 4
handsome is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
2) just set a smaller mesh size on the curves...

1) Delete the surface inside the airfoil and mesh won't generate there.
hi
how we can delete the surface inside the airfoil in icem cfd?
handsome is offline   Reply With Quote

Old   June 20, 2013, 13:39
Default
  #17
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
it is a very basic step, under the geometry tab, you have options to delete points, curves, and surface, or everything. just click on delete surface... Do some tutorials to learn more about it
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 20, 2013, 16:00
Default
  #18
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 4
handsome is on a distinguished road
Quote:
Originally Posted by diamondx View Post
it is a very basic step, under the geometry tab, you have options to delete points, curves, and surface, or everything. just click on delete surface... Do some tutorials to learn more about it
hi
thanks a lot for quick reply my friend

let me explain more about my problem

first i import the airfoil from point data(airfoil curves create not have surface now).then i create the farfield boundary for example like square and create surface in the square.
now for shell meshing what can i do?
at the moment icem can't recognize the surface inside and the outside of the airfoil?
how can split the boundary surface by airfoil curve?
i use segment/trim surfaces and select boundary surfaces and airfoil curve but it dose not work and i don't know why?

(i have the surface of the farfield boundary and the airfoil curve now )


Best regards
handsome is offline   Reply With Quote

Old   July 18, 2013, 15:45
Default
  #19
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 4
handsome is on a distinguished road
Geometry (tab) => Geometry Repair => Build Diagnostic Topology. This will trim the surface with the airfoil curves and probably turn them red. You can then delete the surface within the airfoil
this is the key that i dont know
handsome is offline   Reply With Quote

Old   July 23, 2013, 18:48
Default
  #20
New Member
 
Ankur
Join Date: Jan 2013
Location: Austin, USA
Posts: 26
Rep Power: 4
ankur_kr is on a distinguished road
Hi,

I needed a few suggestions regarding meshing in ICEMcfd. Currently I use unstructured tetrahedral mesh with following options, All Tri Shell Meshing, Tetra/Mixed Volume mesh type and Quick Delaunay Volume mesh method. I wanted to know the following

1) My geometry has a rectangular cuboid of dimension 12m X 3m X 3m with a couple of un-meshed cylindrical tubes (12m & 0.15m dia) through it. I entered the maximum size of mesh cell to be 0.3m. I end up getting about 3,000,000 cells!! which really slows down my simulations. [ I do have some inlet/outlet surfaces of dimensions 15 cm over which I applied prism layers of size 3 cm ]. Is there a way I can reduce the no. of cells considerably ?

2) Which one among Delaunay and Octree is better ?

3) Currently I create surface mesh first and the volume and prism together. Is this the correct sequence or directly computing volume mesh without first creating surface mesh is better ?

4) Does structured mesh gives considerable advantage over un-structured mesh ?

Thanks,
Ankur
ankur_kr 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] surface mesh merging problem everest ANSYS Meshing & Geometry 39 June 5, 2013 19:02
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
[ICEM] Unstructure Meshing Around Imported Plot3D Structured Mesh ICEM kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 12:45
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
Problem with rhoSimpleFoam matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51


All times are GMT -4. The time now is 22:52.