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

[ICEM] 2D tri mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 29, 2013, 05:32
Default 2D tri mesh
  #1
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
Hi friends, I posted about my problem before but i got no answer. I think my previous post was not very specific.
I want to create tri-mesh around 2d airfoil. I did the normal procedure and created surface from outer domain and then deleted the surface inside airfoil. it's ok for general grid. i want to create dense grid in some specific region on airfoil. In one thread Mr. Sajjad says, "For getting smaller mesh in particular regions in 2D, separate those regions in other surfaces and mesh them separately with smaller mesh size." I don't know how to do that.
In my case the airfoil is always just in 2 regions. I don't know how to create more regions. I created airfoil in 4 curves but later my specified size for them doesn't work and it works for just 2 parts (with the name "tmp00 and tmp001"). I don't know why.
I will be really thankful for help and suggestions..
star is offline   Reply With Quote

Old   September 30, 2013, 08:39
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
Are you using patch conforming (patch dependent) or patch independent (octree) mesh for the surface meshing?

Patch dependent mesh size can be controlled at the edge of a surface with the curve sizes. You can specify the exact number of elements you want on any curve segment and it will transition out from there. Right click on curves to view these curve sizes. You can also control the max size on any individual surface.

If you want to break your airfoil up into more surfaces, you could scale up the airfoil curves (say 2x about the centroid) and then use the new larger airfoil to trim its self out of the surface. Then you can set a finer max size on the area between the scaled curves and the original airfoil.

Patch independent is a bit different. You can control the max size (rounded down based on octree) on curves or surfaces. You can also use options such as "width" to transition between one entity and another. You can also take advantage of density regions to control the max size. These are typically used more for 3D, but can also help in this situation where you have one unbroken surface.

If you want more help than that, a picture of how far you have got would be a good idea.
__________________
-----------------------------------------
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 2, 2013, 04:16
Default
  #3
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
Thanks Simon for your reply. First thing is I am using Patch dependent Mesh method. I divided airfoil into 4 curves (shown in Pic1). I want to use different size elements on green and red color airfoil curves. Actually when i want to select curves of airfoil by "mesh curve setup" option there are two types of curves. one type of curves which i have created and it shows with the name "crv" but my specified element size doesn't work for it. There are also 2nd types of curves created with the name "tmp" (or may be surfaces which are created by default after i deleted surfaces inside airfoil by using trim surface option) and size elements works just for these curves. "Pic2" is after deleting the surface inside airfoil. In Pic3 you can see my Part mesh setup and the resulting mesh. you can see my element size doesn't work. In part mesh setup "Fluid" is the name given to the surface. In "Pic4" you can see it just worked by specifying the max element size to "Fluid" (surface) and it has no effect whatever curve size i specify for "Airfoil_up", "Airfoil_down" etc. What should i do? Thanks again
Attached Images
File Type: jpg Pic1.jpg (25.8 KB, 37 views)
File Type: jpg Pic2.jpg (28.8 KB, 31 views)
File Type: jpg Pic3.jpg (99.6 KB, 33 views)
File Type: jpg Pic4.jpg (97.0 KB, 37 views)
star is offline   Reply With Quote

Old   October 9, 2013, 05:12
Default
  #4
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
My above problem is still there. Please any suggestion from any friend will be highly appreciated..
star is offline   Reply With Quote

Old   October 9, 2013, 08:19
Default
  #5
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
Sorry, I can't guess what the issue is. It just looks like a generic airfoil (not a trade secret), would you like to post the tetin file and I will give it a try?
__________________
-----------------------------------------
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 9, 2013, 11:11
Default 2d tri-mesh part element size control
  #6
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
Thanks Simon. Here i am attaching the tetin file. The mesh file is a little big so couldn't upload. I can send you by email if you want to see. As i said before, my main problem is how to control element size over different parts of airfoil.
Regards
Tariq
Attached Files
File Type: zip naca0012.zip (3.7 KB, 7 views)
star is offline   Reply With Quote

Old   October 9, 2013, 12:58
Default
  #7
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
The example you sent has no sizes set on any of the entities.

CFD-Online_Star1.jpg

When I set 40 nodes on each curve, it very clearly worked.

CFD-Online_Star2.jpg

A better approach would use biasing... In this case, I set a height and number of layers on each curve also... (I am attaching this tetin file, just rename from *.txt to *.tin. Once in ICEM, hit compute (surface mesh only) to get this mesh).

CFD-Online_Star3.jpg

An even better approach would use hexa blocking.

If you plan to use unstructured mesh and add prisms, you may want to add a trailing edge curve.
Attached Files
File Type: txt naca0012.txt (16.5 KB, 14 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   October 10, 2013, 00:08
Default
  #8
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
Thanks Mr. Simon. I noticed that you haven't generated surfaces from outer domain. Well, I don't know the exact use of generating surfaces. May be the surfaces are to distribute the elements evenly. I also tried without generating surfaces like you did but when i changed the element size it always merges the previous mesh. For that i thought generating surfaces is must ( but i think i was wrong). Like in your tetin file i changed the inlet and outlet max size to 0.4 so it didn't overwrite the previous mesh rather it merged. Also, can we use prism option in 2D?
Thanks again

Edit: sorry, here i am attaching my tetin file again in which i generated surface.
Attached Files
File Type: zip naca0012.2.zip (9.0 KB, 6 views)
star 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
Star CCM Overset Mesh Error (Rotating Turbine) thezack CD-adapco 3 December 11, 2013 04:09
[ICEM] how to create a 2d tri mesh with quad mesh in the boundary layer seal2013 ANSYS Meshing & Geometry 3 October 6, 2013 16:09
[ICEM] 2D All Tri mesh, problem when reading into Fluent gogga ANSYS Meshing & Geometry 1 May 16, 2011 03:35
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43


All times are GMT -4. The time now is 03:09.