# [ICEM] Airfoils meshing, how create a more dense mesh region?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
September 9, 2011, 04:55
Airfoils meshing, how create a more dense mesh region?
#1
New Member

Andrea Bigliazzi
Join Date: Sep 2011
Location: Milano
Posts: 5
Rep Power: 8
Hi All,
I'm a student of Aerospace Engineering and I'm actually working about a thesis about two airfoils in tandem with the second one very close to the first. I have to solve the 2D fluid arond the airfoils and i'm trying to use ICEM CFD to prepare the mesh.
I have some problem because i'd want to do an unstructured mesh but i'm not able to guide the mesh in some regions of the environment, for example I don't know how to do a more dense mesh in the wake of the airofoils.
I attach an image of my problem.
I hope someone could help me.
Thanks a lot.
Attached Images
 mesh_a.jpg (90.6 KB, 157 views) mesh_b.jpg (75.5 KB, 117 views) mesh_d.jpg (61.1 KB, 93 views)

 September 10, 2011, 09:49 Insight #2 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,665 Blog Entries: 1 Rep Power: 39 ICEM CFD is really a collection of meshing technologies, each with their own advantages and some disadvantages. You are using the patch dependent surface meshing method (a recursive loop paving algorithm), so there isn't a really nice way to control the refinement between curves (no sizing function or back ground grid). You could control the refinement by creating a line or segmented region between the airfoils (gives you control over the sizes along the edge of a loop), then you could control the mesh refinement along this line or in this region. Alternativly, you could switch to patch independent tetra (based on the octree algorithm and hooked up to a sizing function) and use something called a "density region". This is usually intended to control the refinement in a region of a 3D volume, but it can be used on a 2D surface if you use this method... It is one of the options on the mesh tab. Note, it will not work with the patch dependent surface meshing method. Another alternative would be ANSYS Meshing. It can use a very nice sizing function and its patch conforming (a combination of the TGrid Delaunay paver and the next-gen Gambit sizing function) surface mesh method is probably better suited to CFD than the ICEM CFD Patch Dependent method. __________________ ----------------------------------------- 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 10, 2011, 10:42 #3 New Member   Andrea Bigliazzi Join Date: Sep 2011 Location: Milano Posts: 5 Rep Power: 8 Hy Simon, thanks a lot for your answer. I also thought to divide the field in regions with lines and refine the mesh in these region, but the problem is that later, when i run fluent these lines are seen like wall and i can't change the boundary conditions on these. Ansys assistance tell me to try to use Ansys Meshing, but i have a lot of difficulties to create the geometry in design modeler or to import it from Icem. I'll try to use the indipendent method refining the mesh with the 'density region' tab. I'll tell you if this work successfully, thans for the moment. Andrea

 September 10, 2011, 11:03 #4 New Member   Andrea Bigliazzi Join Date: Sep 2011 Location: Milano Posts: 5 Rep Power: 8 Hi Simon, I'll try use the indipendent method and in effective I'm able to use the density region tab to refine the mesh in some zones, but i loose the possibility to create the layers for the strucutred mesh in prossimity of the airfoils, where I have to capture the boundary layer. In fact, in the patch dependent method i'll use ' curve mesh setup--> ' Height, ratio, numbers of layers'. For the inpendent method this tab doesn't work.

 September 11, 2011, 14:22 #5 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,665 Blog Entries: 1 Rep Power: 39 1) With the patch dependent method using sub regions, you can just delete the line elements so there are no internal walls... Just use a name for those curves like "construction" or something like that, and then after the mesh is generated, Edit Mesh => Delete Elements; Select by Part => CONSTRUCTION... 2) With Patch Independent meshing, you need to insert a prism layer after the fact... Do a google search for "blayer2D" for specifics of how to insert a 2D boundary layer with ICEM CFD... __________________ ----------------------------------------- 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

 March 16, 2012, 06:47 #6 New Member   Eirikur Jonsson Join Date: Aug 2011 Posts: 5 Rep Power: 7 Hi Simon I am doing a very similar study as descibed in this thread and I would like you the patch independent method since is offers this excellent control of where to put density regions as well as it produces more "even" mesh in my case than the dependent method. Your last reply suggests a google search for blayer2d on how to insert a prism boundary layer into the independent method. I have done some research but I am unable to find anything. I have been using line elements with the dependent method to obtain the density I require but that is somewhat not very elegant. Could you please describe how to do this with the patch independent or what steps need to be taken in oder to achive a prism boundary layer with the independent method. It would be really helpful. Eiki

 March 16, 2012, 14:02 #7 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,665 Blog Entries: 1 Rep Power: 39 I have done a number of posts on CFD online on the subject of blayer2D. I had hoped that a google search would find those for you. I just tried and found many links... Basically, it is an option you can turn on under Advanced prism options that will allow you to insert ICEM CFD prism in a 2D mesh... (ICEM CFD Prism was intended for 3D so you need to turn on this option to get it to work for 2D). Best regards, Simon __________________ ----------------------------------------- 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

 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 DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42 tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24 james15 STAR-CCM+ 5 August 19, 2010 01:10 chelvistero OpenFOAM 11 January 15, 2010 20:43 Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09

All times are GMT -4. The time now is 05:00.

 Contact Us - CFD Online - Top