CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Pointwise & Gridgen

Normal Extrusion of Block Causes Skew Errors

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 25, 2013, 17:34
Default Normal Extrusion of Block Causes Skew Errors
  #1
New Member
 
Sean Quallen
Join Date: Dec 2011
Posts: 7
Rep Power: 5
SeanQuallen is on a distinguished road
Hello! I have a blade tip surface mesh that I'm trying to extrude into a 3d block (see the first attached picture). However, whenever I do so I get skew errors caused by lines overlapping each other on the extrusion front (see second picture).

I couldn't possibly list everything I've tried to correct this, but some parameters I should mention:
  • I'm using a very small splay value (1e-4) for the 'open' edges and poles on each half of the blade, otherwise they fold over themselves.
  • I get ~40 layers before skew if I use algebraic extrusion. I get skew immediately if I use hyperbolic. What I have been using is 10 layers of algebraic, and then switching to hyperbolic (I need 130 layers total). When I do this I get skew at ~70 hyperbolic layers in the form of the picture shown below.
  • I've played with all of the hyperbolic smoothing parameters, including setting them all to zero and setting them all to very high values (max for Volume and Kinsey-Barth), but still get skew problems.
If anyone has any ideas I'd really appreciate it. Note that I'm a Pointwise/meshing novice such that I might be missing something very basic. Please don't hesitate to point out something incredibly simple out of fear of condescension.



Thanks!


Sean
Attached Images
File Type: jpg Surface Mesh.jpg (76.5 KB, 29 views)
File Type: jpg Extrusion_Overlap.jpg (71.0 KB, 22 views)
SeanQuallen is offline   Reply With Quote

Old   April 26, 2013, 08:44
Default
  #2
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
cnsidero is on a distinguished road
Sean,

I see that you have a pole in your domain. My experience has been to avoid poles in domains that you want to use the hyperbolic extrusion from. They seem to make the algorithm unstable.

All is not lost though. It's relatively straightforward to replace the pole with an O-H topology. Briefly, the steps would be:

- split the domain along a circumferential grid line
- delete the pole, which will in turn delete the small domain resulting from the preceding split
- split the connector at the inner boundary of the remaining domain in two places. Split it such that the resulting first and third connectors have same number of points
- re-dimension the two free connectors left over from the deleted domain such that the sum of the number of points on both minus 1 equals the second connector from the preceding split
- assemble a structured domain from the four connectors
- smooth the two domains with the solver. Pick both domains, Grid>Solve, Edge Attributes, set the Boundary Conditions to Floating. Back to Solve tab and run 10-20 iterations.

The attached images demonstrate this idea on a simple domain.
Attached Images
File Type: jpg pole-replace-01.jpg (40.7 KB, 26 views)
File Type: jpg pole-replace-02.jpg (47.3 KB, 21 views)
File Type: jpg pole-replace-03.jpg (39.9 KB, 20 views)
File Type: jpg pole-replace-04.jpg (40.2 KB, 21 views)
File Type: jpg pole-replace-05.jpg (39.6 KB, 22 views)
cnsidero is offline   Reply With Quote

Old   April 29, 2013, 17:09
Default
  #3
New Member
 
Sean Quallen
Join Date: Dec 2011
Posts: 7
Rep Power: 5
SeanQuallen is on a distinguished road
Thanks Chris. I have moved away from using pole domains for my block extrusion as I need the result to be a single block. However I now have a new problem, but I'm creating a separate thread for it.

Last edited by SeanQuallen; April 29, 2013 at 18:12.
SeanQuallen 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
Building OpenFOAM1.7.0 from source ata OpenFOAM Installation 42 May 14, 2012 20:48
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 bookie56 OpenFOAM Installation 8 August 13, 2011 04:03
Icem Mesh to Foam jphandrigan OpenFOAM Mesh Utilities 4 March 9, 2010 03:58
NACA0012 geometry/design software needed Franny Main CFD Forum 13 July 7, 2007 15:57
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07


All times are GMT -4. The time now is 21:08.