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

separating top surfaces after extruding the 2D mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 30, 2010, 16:48
Default separating top surfaces after extruding the 2D mesh
  #1
New Member
 
Mario
Join Date: Dec 2010
Posts: 3
Rep Power: 6
Mario-CFD is on a distinguished road
Suppose a simple 2D rectangular geometry which is divided in the middle to have to separate zones with one interface. By keeping the "new top part name" as "inherited" when extrude the whole surface mesh, we can have all top surfaces together in one part. What shall we do to separate these top surfaces and have two individual top surfaces?
Mario-CFD is offline   Reply With Quote

Old   December 31, 2010, 12:53
Default Selection workaround...
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Yes, right now "inherited" means to use the volume name for the top surface. That is not ideal by any means. Instead it should use a variant of the original surface element part name...

Anyway, there are two easy work-arounds, this one is the easier of the two because the top surface starts broken into two and it is easy to separate out the volume elements...

A) Use inherited for the new volume part name. This means the volume elements and the top elements will all be in the same part name as the surface elements they were extruded from.

B) Then you can right click on parts => Create Part. Type in the new Part name for FLUID and use the selection tool bar to "select all volume elements" (second to last icon or hotkey 3).

C) If you also want the new top shells to be in unique names, you can right click on Parts again to Create Part, (You may want to turn off all the other parts first so it is easier to select). Type in a new part name (Such as OUTLET), then rotate the model on the screen so you can easily select the elements you want to move into the new part... MMB to apply. Done.

Note; if you play with the "Create Part" or "Add to Part" element selection you will be able to do lots of things (select by polygon or individual selection, etc.)
PSYMN is offline   Reply With Quote

Old   January 4, 2011, 15:35
Default
  #3
New Member
 
Mario
Join Date: Dec 2010
Posts: 3
Rep Power: 6
Mario-CFD is on a distinguished road
Thanks.

1. In figure-1 (attached), for extruding the 2D mesh, I use the 4th option from the left on the "select mesh elements". Am I choosing the correct option?

2. You said:
++++++++++
B) Then you can right click on parts => Create Part. Type in the new Part name for FLUID and use the selection tool bar to "select all volume elements" (second to last icon or hotkey 3).
++++++++++

For creating the new part, If I select "select all volume elements", and 'apply' it, i will have just one part (as shown in figure-2), instead of two. What should I do to have two distinct volume zones?

By the way, after doing this "create part", I get some unwanted curves. You may check figure-3, I have turned on just the lower geometry inlet to show what exactly i mean.

3. To have unique name for top shells, using right click on "Parts" and the 'Create part', and tried various option to create the outlets, but no luck!
Based on the figure-3, in order to create B-OUTLET, what option must be chosen from the "Select mesh elements"? And what pats should be turned-on/off ?
Attached Images
File Type: jpg 1.jpg (90.5 KB, 15 views)
File Type: jpg 2.jpg (88.2 KB, 10 views)
File Type: jpg 3.jpg (91.0 KB, 10 views)
Mario-CFD is offline   Reply With Quote

Old   January 8, 2011, 16:26
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Yes, the 4th option is "Select all". That is a good way to select everything for extrude.

If I assume that you followed my suggestion to set the volume to inherited, then all the volume elements should be in the part of their initial surface mesh. This makes it easy to control which volume elements you display and select, etc.

Instead of using the option to select all the volume elements, you can select visible, or selected or even select by polygon. Here is my suggestion...

1) Turn off all parts. Then turn on the one part that was extruded.
2) Turn off all shells and lines. Turn on the volume elements.
(at this point you should just have the volume elements from one region displayed on the screen)
3) Right click on parts => New Part. Give it a new name (FLUID1) and select all the visible elements (5th icon from the left) or just box select what is on the screen.

4) Adjust display to the next part that was extruded and repeat 4 for the next fluid.


Then handle shells in a similar way... Now when you turn on each part with shells only, you will see a matching pair of sides. Just create a new part and box select the elements on the one side. You may want to orient the model to make this selection easy...
PSYMN 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] Hexa mesh, curve mesh setup, bunching law Anorky ANSYS Meshing & Geometry 4 November 12, 2014 01:27
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
[ICEM] surface mesh merging problem everest ANSYS Meshing & Geometry 39 June 5, 2013 19:02
mesh refinement on top of existent mesh? jx FLUENT 10 January 11, 2004 05:32
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 17:06.