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

Block initiation fails, Pointwise

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 18, 2010, 06:06
Default Block initiation fails, Pointwise
  #1
New Member
 
Filip Wallberg
Join Date: Oct 2010
Posts: 22
Rep Power: 6
filipwa is on a distinguished road
I need to do calculations on a plain wing and i am trying to do the mesh in pointwise. I chose to put the wing inside a cube, which will represent the far field, with the dimensions 20x20x20 m. The wing itself is 10 m long.

After building the surface mesh of the wing i built a block between the wing and the 6 domains representing the far field (cube). To do this i used the command "Create, Assemble Special, Block". Which seems to work without any problems.

However, when i try to initiate the block, half way through the process, i get an error message saying "There are intersecting triangle edges".

Why is this? And how should i go about correcting it?

Any suggestions would be very much appreciated!

Last edited by filipwa; November 18, 2010 at 22:59.
filipwa is offline   Reply With Quote

Old   November 19, 2010, 09:56
Default Causes of intersecting triangle edges
  #2
Member
 
rmatus's Avatar
 
Rick Matus
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 64
Rep Power: 8
rmatus is on a distinguished road
There are several things that could cause intersecting triangle edges:

1. There could be overlapping or intersecting surface grids. This is not too likely, since you were able to assemble a block, but it does not hurt too visually check for this when you are assembling the block.

2. If you have used any quadrilateral surface grids in the face of a tetrahedral block, Pointwise will automatically put pyramids on top of these to provide point-to-point matching between the quads and tetrahedra. It is possible for these pyramids to intersect with each other, particularly if they are on high aspect ratio quads near concave corners. You can visually check for this by selecting the block and going to the Grid, Solve panel. This will display the pyramids. You can adjust pyramid heights in the Attributes, Pyramid pane if necessary.

3. Highly skewed triangles on the surface grids could also cause this message since they could cause odd tetrahedra to be generated in the volume. It is a good idea to check the surface mesh quality before generating a volume mesh. You can use your quality criteria of choice. I usually try to get all the equ-iarea skews below 0.9.

If none of these help, could you post some pictures of your grid or the actual surface grid files? To get more specific in diagnosing this problem, I would need more detail.

Thanks,
Rick
rmatus is offline   Reply With Quote

Old   November 23, 2010, 23:51
Default
  #3
New Member
 
Filip Wallberg
Join Date: Oct 2010
Posts: 22
Rep Power: 6
filipwa is on a distinguished road
Thanks for your reply! Keeping the equiarea skewness to below 0.9 helped me in this case! However, i ran into a new problem though...

I was trying to redo the whole thing and instead looking at only half the wing utilizing a symmetry plane.. Again the block initiation crashes half way through the process saying "There are intersecting edges and triangles".. (The equiarea skewness is kept below 0.9.)

Have been trying the make the mesh finer but it doesnt help. How can I see where those intersecting edges and triangles are?

(Rick, I would be happy to send you the file! Email?)
filipwa is offline   Reply With Quote

Old   November 24, 2010, 00:42
Default
  #4
New Member
 
Filip Wallberg
Join Date: Oct 2010
Posts: 22
Rep Power: 6
filipwa is on a distinguished road
Tried to upload the file here but it was too large.

Last edited by filipwa; November 24, 2010 at 01:23.
filipwa is offline   Reply With Quote

Old   November 24, 2010, 02:36
Default
  #5
Member
 
Join Date: Oct 2010
Posts: 44
Rep Power: 6
siri is on a distinguished road
Did you try to control the mesh skewness further at the interface of wing & plane of symmetry; see if it helps to reduce skewness criteria to less than 0.65 ( i once used a max limit of 0.7 for meshing of airfoil sections in Fluent). does pointwise have other quality metrics like aspect ratio etc
siri is offline   Reply With Quote

Old   November 24, 2010, 05:36
Default
  #6
New Member
 
Filip Wallberg
Join Date: Oct 2010
Posts: 22
Rep Power: 6
filipwa is on a distinguished road
Quote:
Originally Posted by siri View Post
Did you try to control the mesh skewness further at the interface of wing & plane of symmetry; see if it helps to reduce skewness criteria to less than 0.65 ( i once used a max limit of 0.7 for meshing of airfoil sections in Fluent). does pointwise have other quality metrics like aspect ratio etc
yes, the aspect ratio can be controlled.. what would you recommend as a highest value?
filipwa is offline   Reply With Quote

Old   November 24, 2010, 10:11
Default What type of surface mesh?
  #7
Member
 
rmatus's Avatar
 
Rick Matus
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 64
Rep Power: 8
rmatus is on a distinguished road
Is your surface mesh all triangles or does it have some quads in it?

I PM'ed my email address to you in case you want to send me the files.
rmatus 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
Native OpenFOAM interface in Pointwise cnsidero OpenFOAM Meshing & Mesh Conversion 41 May 20, 2012 18:30
[ICEM] Hexa to Sweep block conversion pertupd ANSYS Meshing & Geometry 1 June 19, 2010 21:37
Icem Mesh to Foam jphandrigan OpenFOAM Mesh Utilities 4 March 9, 2010 03:58
blockMesh: block with 6 vertexes dani OpenFOAM 3 June 25, 2009 13:13
Native OpenFOAM interface in Pointwise Chris Sideroff Main CFD Forum 0 January 16, 2009 13:37


All times are GMT -4. The time now is 09:12.