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

Interior Face Extraction in Volume Mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 29, 2014, 18:52
Default Interior Face Extraction in Volume Mesh
  #1
Member
 
Join Date: Jul 2012
Location: Wisconsin,USA
Posts: 34
Rep Power: 5
AA29 is on a distinguished road
Hi everyone,

I have a hybrid mesh for an engine in ICEM . I need to extract some internal faces around the valves in the volume mesh and export those as .STL . I need the internal faces to create faceSets and cellsets later in OpenFOAM.

I have been trying in vain to do this using create subsets in ICEM, but I couldnt find a way to do it.

Hence I am planning to read my mesh in PointWise and see if I can get the job done in PointWise. My first question is:

I just want to know if it is possible in PointWise to extract internal faces in the mesh?
Also , how can I read the mesh in PointWise (I tried to export my mesh in CGNS and read the grid it in PointWise, but I am getting error - Cannot open File.)
If anyone has experience, I would be really grateful if you share your thoughts.

Thank you in advance !
AA29 is offline   Reply With Quote

Old   March 30, 2014, 19:30
Default
  #2
Senior Member
 
John Chawner
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 221
Rep Power: 9
jchawner is on a distinguished road
There is no tool in Pointwise for selecting a set of faces from the interior of a volume mesh and exporting them as STL. However, there's a tool in the Examine command for looking at mesh quality metrics than can export an X, Y, or Z constant cut through a mesh to STL. Of course, the implication is that the faces you desire all lie on the same plane.

However, the difficulty will be getting the hybrid mesh into Pointwise due to restrictions on the mesh topology in each block.
__________________
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, 2014, 13:25
Default
  #3
Member
 
David Garlisch
Join Date: Jan 2013
Location: Pointwise HQ
Posts: 82
Rep Power: 4
dgarlisch is on a distinguished road
The Pointwise OpenFOAM CAE exporter has some support for face sets and cell sets.

It can export:
  1. cell sets:
    • one per volume condition (VC)
  2. face sets as:
    • boundary faces of a VC
    • interior faces of a VC
    • all faces of a VC

If you cannot import your ICEM grid into Pointwise, you could rebuild it using Pointwise and then export.

As an example, I have attached an OpenFOAM export for a simple Pointwise grid. The forum wouldn't let me attach the PW model (it was too big at 100k!).
Attached Images
File Type: png screenshot.png (37.8 KB, 14 views)
Attached Files
File Type: zip spinner-baffle.zip (79.2 KB, 4 views)
dgarlisch is offline   Reply With Quote

Old   March 31, 2014, 13:37
Default
  #4
Member
 
Join Date: Jul 2012
Location: Wisconsin,USA
Posts: 34
Rep Power: 5
AA29 is on a distinguished road
Thank you guys for the prompt response. It has been helpful !
But i decide to create the surfaces in the geometry and ICEM has the capability to export them as .STL .

Anways, thanks a lot !
AA29 is offline   Reply With Quote

Old   April 10, 2014, 07:15
Default
  #5
Member
 
Payam D.
Join Date: Aug 2011
Posts: 79
Blog Entries: 3
Rep Power: 5
pdp.aero is on a distinguished road
Quote:
Originally Posted by AA29 View Post
Hi everyone,

I have a hybrid mesh for an engine in ICEM . I need to extract some internal faces around the valves in the volume mesh and export those as .STL . I need the internal faces to create faceSets and cellsets later in OpenFOAM.

I have been trying in vain to do this using create subsets in ICEM, but I couldnt find a way to do it.

Hence I am planning to read my mesh in PointWise and see if I can get the job done in PointWise. My first question is:

I just want to know if it is possible in PointWise to extract internal faces in the mesh?
Also , how can I read the mesh in PointWise (I tried to export my mesh in CGNS and read the grid it in PointWise, but I am getting error - Cannot open File.)
If anyone has experience, I would be really grateful if you share your thoughts.

Thank you in advance !
There is a trickery way to extract i, j or k constant surface from the structured volume mesh in Pointwise.
My suggestion is:
1- Create your volume mesh around whatever you are working on or in the whatever you are working on. After successful creation of 3D structured volume mesh or successful importation of your 3D structured volume mesh.
2- Split your volume mesh in your desired i, j or k.
3- Change the set dimension from 3D to 2D.
4- Select your surface mesh.
5- Extract your desired surface mesh in STL format.

Most of the time due to the topology of the blocks, splitting the volume mesh creates non-flat surface mesh, so if you are planning to extract your surface mesh as a flat surface, you need to create a plane from three points of your non-flat surface. Then by projecting the non-flat mesh surface on the defined plane you will reach a flat surface mesh with constant x, y or z that depends on your location for extraction.
However, please note every time, you can just extract one surface mesh from structured volume mesh.
pdp.aero 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
dynamic Mesh is faster than MRF???? sharonyue OpenFOAM Running, Solving & CFD 14 August 26, 2013 07:47
channelFoam for a 3D pipe AlmostSurelyRob OpenFOAM 3 June 24, 2011 13:06
engrid: Internal volume mesh becoming coarser during boundayr layer addition Arnoldinho OpenFOAM 1 January 22, 2011 05:31
BlockMesh FOAM warning gaottino OpenFOAM Native Meshers: blockMesh 7 July 19, 2010 14:11
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09


All times are GMT -4. The time now is 05:34.