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

initialize problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 2, 2014, 08:09
Default initialize problem
  #1
New Member
 
Fabrizio
Join Date: Feb 2014
Posts: 7
Rep Power: 3
kasto89 is on a distinguished road
hello all,

i have a problem in initialization of a block. I can not understand why pointwise builds some pyramids on the external side of the surfaces. I attach a picture.

thanks
Attached Images
File Type: jpg celle.jpg (98.5 KB, 32 views)
kasto89 is offline   Reply With Quote

Old   April 2, 2014, 08:35
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
Quote:
Originally Posted by kasto89 View Post
hello all,

i have a problem in initialization of a block. I can not understand why pointwise builds some pyramids on the external side of the surfaces. I attach a picture.

thanks
Can you give us a little more information. Is it unstructured, structured or hybrid (prism+unstructured)? Did you examine the mesh in Pointwise? Is it OK there?
cnsidero is online now   Reply With Quote

Old   April 2, 2014, 08:49
Default initialize problem
  #3
New Member
 
Fabrizio
Join Date: Feb 2014
Posts: 7
Rep Power: 3
kasto89 is on a distinguished road
the external surfaces of the cylinder are structured domains, the base circular area of the cylinder is an unstructured domain; the block is unstructured.

I built an other cylinder in the same way and i have not this issue.

I attach some pictures for a better explanation.
In the first picture you can see how i built the block, in the second one it is possible to observe the "external" pyramids on the surface.


thanks
Attached Images
File Type: jpg Schermata del 2014-04-02 14:43:16.jpg (77.1 KB, 32 views)
File Type: jpg Schermata del 2014-04-02 14:48:01.jpg (70.6 KB, 27 views)
kasto89 is offline   Reply With Quote

Old   April 2, 2014, 09:03
Default
  #4
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
cnsidero is on a distinguished road
Quote:
Originally Posted by kasto89 View Post
the external surfaces of the cylinder are structured domains, the base circular area of the cylinder is an unstructured domain; the block is unstructured.

I built an other cylinder in the same way and i have not this issue.

I attach some pictures for a better explanation.
In the first picture you can see how i built the block, in the second one it is possible to observe the "external" pyramids on the surface.

thanks
Thanks. Much clearer. Somehow the block face normal got flipped. To confirm, select the block with pyramids pointing out and go into the block solver. You'll probably see the pyramids (dark grey outlines) on the wrong side of the wall. To fix it, get out of the solver, go to Edit > Add/Remove Faces ..., click Begin Flip Face Orientation, pick the (only) face, click End Flip Face Orientation, and OK. Re-export the mesh.

That should fix it.

I see you're using OpenFOAM so I'll offer another tip. If you haven't already, I highly recommend using renumberMesh, e.g.:

Code:
renumberMesh -overwrite
to reduce the matrix bandwidth. Pointwise meshes rarely, if ever, have even close to optimal point ordering and renumbering the mesh will help convergence. I've found cases where the solution won't converge without renumbering first.
cnsidero is online now   Reply With Quote

Old   April 2, 2014, 10:19
Default perfect
  #5
New Member
 
Fabrizio
Join Date: Feb 2014
Posts: 7
Rep Power: 3
kasto89 is on a distinguished road
thank you very much, you resolved me a very annoying problem.

Can you help me to obtain the block extruding the base circular area? if i try to use as path one of the connector on lateral surface I can not match the other circular base, so the real stl.

thanks
kasto89 is offline   Reply With Quote

Old   April 2, 2014, 15:39
Default
  #6
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
cnsidero is on a distinguished road
Quote:
Originally Posted by kasto89 View Post
thank you very much, you resolved me a very annoying problem.

Can you help me to obtain the block extruding the base circular area? if i try to use as path one of the connector on lateral surface I can not match the other circular base, so the real stl.

thanks
I believe you're trying extrude the triangles along the length of the curving pipe, correct? If the pipe is truly circular along the path, you will need to find/create the curve that's the pipe axis and use the pipe axis to Extrude by Path along. Be sure to enable to the Path Rotation option during the extrude so the face stays perpendicular to the path direction.

If this doesn't work, I would suggest making a structured mesh on the circular ends of the pipe, then along with the domains on the side of the pipe assemble a structured block.
cnsidero is online now   Reply With Quote

Old   April 2, 2014, 16:49
Default Extrusion
  #7
New Member
 
Fabrizio
Join Date: Feb 2014
Posts: 7
Rep Power: 3
kasto89 is on a distinguished road
Yes, It is correct! I have already though to extrude the base using the "axys curve" as path, but i do not know how to draw it, is there a strategy?

I does not build a structured block because the other one downside contains a valve, so i have to make it unstructured and I do not want a strength change of shape of cells at the interface between the 2 blocks.
Sorry for my poor English and thank you very much.

Last edited by kasto89; April 3, 2014 at 09:08.
kasto89 is offline   Reply With Quote

Old   April 3, 2014, 16:17
Default
  #8
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
cnsidero is on a distinguished road
Quote:
Originally Posted by kasto89 View Post
Yes, It is correct! I have already though to extrude the base using the "axys curve" as path, but i do not know how to draw it, is there a strategy?
My first suggestion would be to see if you can extract it or rebuild it using the original CAD software that generated the geometry.

If this is not option, you can try to rebuild it in Pointwise. The success of doing so depends on the how the pipe's trajectory changes shape. If does something simple like a circular bend that this shouldn't be hard. If however it's a more general shape it'll be harder.

This difficult to explain in words so here it is in pictures (the number refers the image name suffix)

01: my pipe has a straight section, followed by a circular bend, followed by another straight section.
02: create a straight 2 pt curve across the diameter of the circular cross section
03: split the previous 2 pt curve in the middle
04: create a db point at split location (delete two curves). the point will be at the center of the cross section.
05: repeat 02 thru 04 for each cross section. Mine has 4.
06: draw appropriate curve type between each point. Mine is straight 2 pt curve, circular arc and another 2 pt curve.
07: final trajectory. create a connector(s) on trajectory that canbe used to drive path based extrusion

As I mentioned the trick will be knowing the trajectory path. If it's simple things like straight lines or circular bends, it should be no problem. Otherwise you'll have to guess and use a more general curve type (Bezier or Conic).

Good luck, Chris
Attached Images
File Type: jpg cl-traj-01.jpg (12.5 KB, 17 views)
File Type: jpg cl-traj-02.jpg (33.4 KB, 14 views)
File Type: jpg cl-traj-03.jpg (32.7 KB, 13 views)
File Type: jpg cl-traj-04.jpg (31.1 KB, 9 views)
File Type: jpg cl-traj-05.jpg (32.3 KB, 10 views)
cnsidero is online now   Reply With Quote

Old   April 3, 2014, 16:18
Default
  #9
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
cnsidero is on a distinguished road
Last two images.
Attached Images
File Type: jpg cl-traj-06.jpg (33.6 KB, 9 views)
File Type: jpg cl-traj-07.jpg (32.5 KB, 9 views)
cnsidero is online now   Reply With Quote

Old   April 4, 2014, 04:36
Default
  #10
New Member
 
Fabrizio
Join Date: Feb 2014
Posts: 7
Rep Power: 3
kasto89 is on a distinguished road
ok, thank you very much, i have already tried something like that.
now I have an other problem, I cannot initialized an unstructured block, "one or more entities could not be initialize";

ok solved, i had a bad surface
kasto89 is offline   Reply With Quote

Old   March 27, 2015, 06:40
Default One or more entities could not be initialized
  #11
New Member
 
Bharatesh
Join Date: Mar 2015
Posts: 25
Rep Power: 2
bharatesh is on a distinguished road
Hi guys,
even i have similar problem. I'm using Windows platform(32 bit), and the total cells are roughly 2 million, after creating the Block, when tried to 'initialize', the file is processed for some time and i get an error saying "One or more entities could not be initialized", i don't understand which entities could not be initialized!.


System info:
platform: Windows XP (32bit)
RAM: 1GB

Can somebody help me please..
bharatesh is offline   Reply With Quote

Old   March 29, 2015, 19:02
Default
  #12
Senior Member
 
John Chawner
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 219
Rep Power: 9
jchawner is on a distinguished road
When an unstructured volume mesh cannot be initialized it's usually because the mesher cannot recover the surface cells. Therefore, check the quality of all the surface meshes on the block's faces.

Hope this helps.
__________________
John Chawner / jrc@pointwise.com / www.pointwise.com
Blog: http://blog.pointwise.com/
on Twitter: @jchawner
jchawner is offline   Reply With Quote

Old   March 31, 2015, 00:03
Default How to reduce Skewness in pointwise 17.2
  #13
New Member
 
Bharatesh
Join Date: Mar 2015
Posts: 25
Rep Power: 2
bharatesh is on a distinguished road
Quote:
Originally Posted by jchawner View Post
When an unstructured volume mesh cannot be initialized it's usually because the mesher cannot recover the surface cells. Therefore, check the quality of all the surface meshes on the block's faces.

Hope this helps.
Thanks John Chawner,
I got the issue resolved, however i'm facing new one.. What I did is:-
1. Completed the meshing with 1.44 million cells (approx.),
2. Imported mesh file in .cas format to Ansys Fluent 14
3. Did Mesh Check, appears to be okay, and Orthogonal Quality is 0.12
4. When I try to Run the file in the solver, it says that the Max Skewness is more than 0.98. Since I did not get any warning message while doing mesh check, its now bothering me alot..
5. How can I reduce the Skewness??

I examined the mesh file in Pointwise, the 'Max. Included Angle' appears to be well below 173. Attaching the 'Centroid Skewness' screenshot.
Attached Images
File Type: jpg Capture.jpg (69.4 KB, 9 views)
bharatesh is offline   Reply With Quote

Old   March 31, 2015, 09:01
Default
  #14
Senior Member
 
John Chawner
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 219
Rep Power: 9
jchawner is on a distinguished road
It seems that your best approach would be to determine which of Pointwise's skewness metrics best matches what Fluent calls "Max Skewness" and look at it in the Examine command and use the Extrema function to zoom in to it's maximum value. See what's going on there and take appropriate action.
__________________
John Chawner / jrc@pointwise.com / www.pointwise.com
Blog: http://blog.pointwise.com/
on Twitter: @jchawner
jchawner 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
Problem with interFoam; Wave/wiggle alpha1 behavior JonW OpenFOAM 3 February 23, 2013 21:41
Gambit - meshing over airfoil wrapping (?) problem JFDC FLUENT 1 July 11, 2011 05:59
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13
Is this problem well posed? Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52


All times are GMT -4. The time now is 06:42.