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

Is there any way to create a grid that looks like this?

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

Like Tree3Likes
  • 1 Post By PSYMN
  • 1 Post By PSYMN
  • 1 Post By RodriguezFatz

Reply
 
LinkBack Thread Tools Display Modes
Old   August 8, 2011, 06:37
Default Is there any way to create a grid that looks like this?
  #1
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,097
Rep Power: 16
RodriguezFatz will become famous soon enough
Hi guys,

I'm trying to get a grid that looks like this (see attached picture) in Ansys meshing 13. My problem is, that mapped face meshing in the center region leads to strongly distorted elements. Is there any way to do this more handmade instead of the auto-tools?

Thanks for any help!
Attached Images
File Type: jpg grid_picture.jpg (19.6 KB, 83 views)
RodriguezFatz is offline   Reply With Quote

Old   August 8, 2011, 09:43
Default
  #2
Member
 
Join Date: Mar 2009
Posts: 85
Rep Power: 8
husker is on a distinguished road
Hi Rodrigues,

Yes it is possible to create this type of mesh.

In Gambit:
Firstly, you should create or import the boundary edge geometries.
Secondarily, mesh these edges with gambit edge mesh menu.
Finally mesh the surface with structured quad elements.

In Gridgen: There is a tutorial about this geometry. (Tutorial 2: 2D Bump)
husker is offline   Reply With Quote

Old   August 8, 2011, 09:55
Default
  #3
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,097
Rep Power: 16
RodriguezFatz will become famous soon enough
Thanks husker,

I will try to do the tutorial first...
RodriguezFatz is offline   Reply With Quote

Old   August 9, 2011, 12:29
Default
  #4
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
In ICEM CFD hexa, it is just a CGRID around the bump.
amin_gls likes this.
__________________
-----------------------------------------
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   August 9, 2011, 15:17
Default
  #5
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,097
Rep Power: 16
RodriguezFatz will become famous soon enough
Quote:
Originally Posted by PSYMN View Post
In ICEM CFD hexa, it is just a CGRID around the bump.
I'm currently learning to mesh with ICEM... not too easy
What I tryed to do is:
-create and export the geometry with design modeler
-create the grid and all "named selections"
-export the setup for FLUENT
Is this the best way?
RodriguezFatz is offline   Reply With Quote

Old   August 9, 2011, 16:00
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
That is not ICEM CFD, that is ANSYS Meshing...

To do this in ANSYS Meshing, you could draw out the segments as you want, imprint them on the geometry in DM. Then once in ANSYS Meshing, you could right click on the mesh tab to insert a mapped method on these parts...

Then compute mesh and away you go.


In ICEM CFD (which does have some learning curve, but once you learn it is the most powerful hexa tool on the market), you would start with a rectangular 2D block and associate it with the "corners" of your geometry. Then split around the bump (3 simple split commands) and insert a CGrid (one command). Then delete the central HGrid portion of the CGrid (one command) and associate the edges to the curves. With some hexa practice, you could do it in a minute or two.
amin_gls likes this.
__________________
-----------------------------------------
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   August 9, 2011, 16:14
Default
  #7
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,097
Rep Power: 16
RodriguezFatz will become famous soon enough
I guess my post was missleading. Up to now I used ansys meshing. Now, I want to give ICEM a try. Thats why I used the geometry that I allready created with design modeler. I exported the geometry to open it with ICEM. My plan was to create and export a grid and open this with FLUENT. The question is: Is this way ok, or completely bad?
RodriguezFatz is offline   Reply With Quote

Old   August 9, 2011, 17:17
Default Sure...
  #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
Oh yea, thats fine. Save the AGDB file in DM, open that with ICEM CFD (File => Workbench Readers), then block it, convert to unstructured mesh, output to Fluent... Fluent Bocos and Zones are applied based on Parts in ICEM CFD. So if you want one end to be an inlet, make sure you create a new part named "INLET". If you create these as Named Selections in DM, they can be imported, but you need to check the right box. If they come in as geometry subsets instead of Parts, you can right click on subsets and turn them into parts.

Some things to watch out for... Fluent expects this in the Z=0 plane. Also make sure you associate all the perimeter edges to curves or you will get a null pointer error due to your uncovered edges.
__________________
-----------------------------------------
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   August 11, 2011, 03:37
Default
  #9
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,097
Rep Power: 16
RodriguezFatz will become famous soon enough
Great, this is the first time where I got it running. Thanks!!!

Update: Your youtube tutorial is great and solved nearly all of my problems!!!
amin_gls likes this.

Last edited by RodriguezFatz; August 12, 2011 at 04:31.
RodriguezFatz is offline   Reply With Quote

Old   August 12, 2011, 04:34
Default
  #10
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,097
Rep Power: 16
RodriguezFatz will become famous soon enough
I uploaded a picture of some random test. Just for my understanding: Why doesn't the grid line stick to the block in the middle part of the c-grid (but it is bended)? It seems to work at the left and right part and at all other block edges.
Attached Images
File Type: jpg screen.jpg (41.2 KB, 36 views)
RodriguezFatz is offline   Reply With Quote

Old   August 12, 2011, 11:06
Default
  #11
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
It is trying (and succeeding) to raise the quality in that acute 5 element corner.

You could slide the corner nodes a little so the angle is more balanced and you would get a more even result between the three edges. (my recommendation)

If you want to force it straight regardless of quality, just add an edge split in the middle of that edge and use it to straighten out the edge.

You could also just leave it alone. The quality is good enough for any solver. You don't actually need straight lines. You should probably adjust the o-grid edge distribution first and see how it looks then.
__________________
-----------------------------------------
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

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
Actuator disk model audrich FLUENT 0 September 21, 2009 07:06
Where's the singularity/mesh flaw? audrich FLUENT 3 August 4, 2009 01:07
2d irregular grid Remy Main CFD Forum 1 December 22, 2008 05:49
Obtain Geometry Data from a Grid File in CFX 10.0 ARJUN CFX 2 August 17, 2006 07:20
Troubles modelling flow through a grid Hans Klaufus CFX 1 June 28, 2000 16:43


All times are GMT -4. The time now is 07:54.