# [ICEM] Blocking of 2 cylinders

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

April 12, 2011, 07:13
Blocking of 2 cylinders
#1
Member

Frank Weise
Join Date: Mar 2009
Location: Germany
Posts: 39
Rep Power: 9
Hi,
i will mesh 2 cylinders with blocking. The problem is the cylinders have a common intersection point. See the pictures in the attachment.
How should i change my blocking to get the right mesh?

Thanks
Frank
Attached Images
 Bild1.jpg (89.5 KB, 89 views) Bild2.jpg (88.8 KB, 79 views)

 April 12, 2011, 07:19 #2 Senior Member   AB Join Date: Sep 2009 Location: France Posts: 323 Rep Power: 14 I guess you created an O-grid for your 1st (big) cylinder. Then split your O-grid around the curevs of your 2nd (small) cylinder. Then, do an O-grid for your 2nd (small) cylinder.

April 12, 2011, 10:41
#3
Member

Frank Weise
Join Date: Mar 2009
Location: Germany
Posts: 39
Rep Power: 9
Hi BrolY,
thanks for the fast reply. Can you explain how i split the o-grid around the curves of the 2nd small cylinder. In the attachmet i've finished step 1 at a test cylinder.

Thanks

Edit: I 've attached the geometric files
Attached Images
 Bild3.jpg (92.0 KB, 63 views)
Attached Files
 Test Netz.zip (11.5 KB, 17 views)

Last edited by FrankW; April 12, 2011 at 11:08.

 April 13, 2011, 08:39 #4 Senior Member   AB Join Date: Sep 2009 Location: France Posts: 323 Rep Power: 14 I found 2 solutions, but maybe other users may have other ideas: 1) Create 2 meshes, and do a conformal merge of the 2 meshes. 2) in your blocking, create another split along the 2nd (small) cylinder. Then merge the two nodes at the intersection point. Delete the block along your small cylinder (the one created by the previous split), and associate. At the end, the quality of the mesh will be bad ... I'll try to figure out another way to have a good mes quality without creating 2 meshes. Good luck !

April 13, 2011, 12:34
Solution
#5
Retired from CFD Online

Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
Hey Frank,

The difficulty here is because the smaller pipe is all the way at the end of the larger pipe. It can be done but it is a minor hassle...

Is this how you need the geometry to be? Do you plan to extend the large pipe anyway or does this represent the end wall of the pipe? If it is an end wall, does the actual model meet perfectly like this or does the larger pipe actually extend a little beyond the small pipe? The more complex the model, the more I would suggest you push these questions.

On the other hand, this is a pretty simple model. So lets just sort it out as it is. We will need to propagate the wedge shape back thru the larger pipe... Can you handle wedges (easiest solution) or does your solver require pure hexa? (Or maybe I should just ask; what is your solver?) I will start with wedges. The pure hexa solution involves replacing the wedge with a Yblock...

The basic approach should be to pretend there is a little lip at the end (I actually copied a point out by 0.1 to make it easier to pretend). You will need to split to capture both sides of the little pipe. Ogrid the large pipe as you did, then also Ogrid the smaller pipe (Select the pipe block and the block just inside the large pipe. Also select the face on the outer end of the small pipe and the symmetry planes.) Then come back and merge away the small edge and its parallel pairs (4 total pairs) back thru the model. This will collapse it into a wedge that goes back thru the model.

Anyway, it only takes 2 minutes (less time than to type this email actually), so here it is.

Run the replay file with the "always update" option to see my steps.

Best regards.
Attached Images
 FrankW_01.jpg (79.7 KB, 77 views) FrankW_02.jpg (66.8 KB, 63 views) FrankW_03.jpg (69.8 KB, 67 views)
Attached Files
 FrankWeise.zip (7.8 KB, 26 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

April 14, 2011, 10:49
#6
Member

Frank Weise
Join Date: Mar 2009
Location: Germany
Posts: 39
Rep Power: 9
Hi PSYMN,

thanks for your explanations. It helps me fine. The original geometry has similar dimensions and is more complicated. In the attachment are the files. The inlay called MG_Rahmen.. is a porus structure. This part was easily to mesh (MG_Rahmen.zip). My problem is the meshing of the rest of the fluidic part. In the past i used only Anys WB meshing and i'am so not confirm with ICEM. Because the small structures i think i can generate better meshs with ICEM with less elements.
The real stuctures has the same dimensions. And i need an adequate model to compare our Oxygen measurements with the theoretic model. Our Flowrate is moderate, we have a real laminar flow RE<10.

Best regards.
Attached Files
 Dfz_Mod4_1.zip (89.3 KB, 14 views) MG_Rahmen.zip (62.4 KB, 13 views)

 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 icemaniac178 ANSYS Meshing & Geometry 14 March 20, 2013 00:18 [ICEM] Blocking and Symmetry BrolY ANSYS Meshing & Geometry 32 August 24, 2012 03:13 [ICEM] Blocking strategy BrolY ANSYS Meshing & Geometry 0 July 22, 2010 04:46 karananand ANSYS Meshing & Geometry 2 July 9, 2010 16:34 Severin CFX 3 September 18, 2007 09:02

All times are GMT -4. The time now is 06:55.

 Contact Us - CFD Online - Top