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

zero-thickness wall

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

Like Tree3Likes
  • 1 Post By dgarlisch
  • 1 Post By tcarrigan
  • 1 Post By dgarlisch

Reply
 
LinkBack Thread Tools Display Modes
Old   January 24, 2014, 11:20
Default zero-thickness wall
  #1
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
Hi,

Is pointwise able to generate a zero-thickness wall and then mesh around it? How? Thanks
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   January 25, 2014, 12:29
Default
  #2
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 369
Rep Power: 12
cnsidero is on a distinguished road
Daniel.

Yes. For domains, once the first edge is defined (which has to be closed) for addtional (internal) edges you simply need to choose the connectors twice. For blocks, once the first face is defined (which has to be closed), for additional (internal) faces there is an option to add the face as a baffle.

See the attached sequence of images for an example on domains. You'll notice in the first one I chose two connectors for the internal edge and in the second image I've chosen the same two connectors again (see how the arrows double back).

Quote:
Originally Posted by lakeat View Post
Hi,

Is pointwise able to generate a zero-thickness wall and then mesh around it? How? Thanks
Attached Images
File Type: jpg zero-thk-wall-01.jpg (13.7 KB, 57 views)
File Type: jpg zero-thk-wall-02.jpg (13.8 KB, 37 views)
File Type: jpg zero-thk-wall-03.jpg (13.9 KB, 37 views)
File Type: jpg zero-thk-wall-04.jpg (31.0 KB, 39 views)
cnsidero is offline   Reply With Quote

Old   January 28, 2014, 14:43
Default
  #3
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
Thank you Chris, I will try it out.
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   January 30, 2014, 12:53
Default
  #4
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
I made it.
testMesh.jpg

Hmm, I am confused now how to convert the t-rex mesh to prisms, why it is always in grey. Did I miss something here?

PS: Are there any macros available that can build quickly a rectangular topology or a circular topology?
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   January 30, 2014, 16:40
Default
  #5
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
Hi Chris,

In order to generate a mesh for OpenFOAM with baffles, I have to extrude the 2D mesh in the 3rd direction. And then export the CAE. But now, it seems to me that the extrusion does not work for the baffles. What I'm saying is this, normally, you extrude a mesh, then connector becomes a surface, a surface becomes a domain, right? But now a baffle is not extruded to be a surface. The problem with that is that I can't in CAE boundary condition set tab to assign the b.c. to the baffles. Of cause I can manually extrude the connector here to create a surface and then set the boundary condition, but still in exporting to the openfoam mesh, there is no such boundary patch. Any ideas? Thanks!
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   February 2, 2014, 12:22
Default
  #6
Member
 
David Garlisch
Join Date: Jan 2013
Location: Pointwise HQ
Posts: 83
Rep Power: 4
dgarlisch is on a distinguished road
Pointwise has a great collection of scripts available on GitHub. I think this is the script you want.

I also have some good/bad news...

GOOD:
There is a script in my personal GitHub account that thickens a 2D grid into a 1 cell deep (or more) 3D grid. All boundary conditions in the 2D grid are automatically transferred to the corresponding extruded domains in the resulting 3D grid.

BAD:
This script will only work directly with solvers that support both 3D and 2D grid mode. OpenFOAM does not support 2D mode.

WORKAROUND:
If you want to avoid thickening the grid manually, you will need to:
  • Load your 2D OpenFOAM grid into Pointwise.
  • Change the solver to one that supports 2D mode (e.g. CGNS).
  • Switch the mode to 2D (menu CAE/Set Dimension/2D).
  • Thicken the 2D grid with the script.
  • Switch solver back to OpenFOAM.
  • Reset the BC and VC types.
Good luck!
lakeat likes this.
dgarlisch is offline   Reply With Quote

Old   February 2, 2014, 12:59
Default
  #7
Member
 
David Garlisch
Join Date: Jan 2013
Location: Pointwise HQ
Posts: 83
Rep Power: 4
dgarlisch is on a distinguished road
Converting trex tets to prisms is done during export. To enable, select the Combine Aniso checkbox on the export options dialog.
dgarlisch is offline   Reply With Quote

Old   February 3, 2014, 12:44
Default
  #8
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
Thank you David. But I still don't know how to set the boundary condition for a baffle? (As I have mentioned in post #5) This seems to have nothing to do with OpenFOAM. Let's me give an simple example:

In a 2D CAE case, say it is a CGNS mesh. And there is a baffle inside, and I can set one connector as inlet, another as outlet, and so on, but I can't select the baffle to set it as a boundary condition. Why?
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   February 3, 2014, 13:36
Default
  #9
Senior Member
 
Travis Carrigan
Join Date: Jul 2010
Location: Arlington, TX
Posts: 127
Rep Power: 7
tcarrigan is on a distinguished road
Daniel,

You need to check the box "Select Connections" when assigning boundary conditions.
lakeat likes this.
tcarrigan is offline   Reply With Quote

Old   February 3, 2014, 14:01
Default
  #10
Member
 
David Garlisch
Join Date: Jan 2013
Location: Pointwise HQ
Posts: 83
Rep Power: 4
dgarlisch is on a distinguished road
Quote:
Originally Posted by lakeat View Post
Thank you David. But I still don't know how to set the boundary condition for a baffle? (As I have mentioned in post #5) This seems to have nothing to do with OpenFOAM. Let's me give an simple example:

In a 2D CAE case, say it is a CGNS mesh. And there is a baffle inside, and I can set one connector as inlet, another as outlet, and so on, but I can't select the baffle to set it as a boundary condition. Why?
In Pointwise, a baffle is considered to be a connection between two blocks. In the case of a baffle, it is the same block on both sides.

In CAE/Set Boundary Conditions..., you should see a listing of two-sided "connections" at the bottom of the BC dialog box. You must select the Select Connections check box to set BCs on these connectors.

I have attached an image.
Attached Images
File Type: jpg cfdOnline.jpg (56.2 KB, 31 views)
lakeat likes this.

Last edited by dgarlisch; February 3, 2014 at 14:03. Reason: Add attachment
dgarlisch 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
Wall treatment with OpenFOAM roby OpenFOAM Running, Solving & CFD 39 May 4, 2015 13:00
UDF for wall slipping HFLUENT Fluent UDF and Scheme Programming 0 April 27, 2011 12:03
modelling wall thickness coupling (like fluent) in cfx suryawanshi_nitin CFX 3 April 13, 2009 01:25
first wall layer thickness and droplet size itchie CFX 3 May 14, 2008 09:03
thickness off wall Ahlem FLUENT 1 February 20, 2007 23:45


All times are GMT -4. The time now is 20:57.