CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Mesh Generation & Pre-Processing Software > Pointwise & Gridgen

" a negative cell volume error " when import into fluent

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

Like Tree1Likes
  • 1 Post By Abhinand

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 1, 2017, 17:50
Default " a negative cell volume error " when import into fluent
  #1
New Member
 
muhamad elberens
Join Date: Feb 2017
Posts: 10
Rep Power: 7
mlberens is on a distinguished road
i am working on a 2d vawt ( structure and unstructured doamins ) simulation using mesh motion technique and pointwise for mesh generation.
however i am already double checked the orientation of the structured and made sure that unstructured domains are oriented to +z, i examine also the area ratio.
still get a negative cell volume error in fluent

Sent from my SM-N920C using CFD Online Forum mobile app
mlberens is offline   Reply With Quote

Old   October 1, 2017, 17:55
Default
  #2
Member
 
Abhinand
Join Date: Jun 2016
Posts: 75
Rep Power: 8
Abhinand is on a distinguished road
Please attach PW file for a rough idea to get to know the real problem
The problem could be unnoticed empty domains or blocks, or could be orientation error between structured and unstructured meshes
mlberens likes this.
Abhinand is offline   Reply With Quote

Old   October 1, 2017, 18:05
Default
  #3
New Member
 
muhamad elberens
Join Date: Feb 2017
Posts: 10
Rep Power: 7
mlberens is on a distinguished road
your email please so i can send it to you

Sent from my SM-N920C using CFD Online Forum mobile app
mlberens is offline   Reply With Quote

Old   October 1, 2017, 21:50
Default
  #4
New Member
 
muhamad elberens
Join Date: Feb 2017
Posts: 10
Rep Power: 7
mlberens is on a distinguished road
Quote:
Originally Posted by Abhinand View Post
Please attach PW file for a rough idea to get to know the real problem
The problem could be unnoticed empty domains or blocks, or could be orientation error between structured and unstructured meshes
https://www.dropbox.com/s/bzpvgwq0tk...29-9pw.pw?dl=0

Sent from my SM-N920C using CFD Online Forum mobile app
mlberens is offline   Reply With Quote

Old   October 2, 2017, 13:15
Default
  #5
Senior Member
 
David Garlisch
Join Date: Jan 2013
Location: Fidelity Pointwise, Cadence Design Systems (Fort Worth, Texas Office)
Posts: 307
Rep Power: 13
dgarlisch is on a distinguished road
I exported the grid to a cas file using File, export, CAE... in Pointwise V18.0R4.

I was able to import the cas file into fluent V18 without any reported negative cell volumes.

Are you setting the double precision option during fluent cas import?
dgarlisch is offline   Reply With Quote

Old   October 2, 2017, 13:28
Default
  #6
New Member
 
muhamad elberens
Join Date: Feb 2017
Posts: 10
Rep Power: 7
mlberens is on a distinguished road
I imported cas file into fluent V15, double percision without negative cell error but when i click calculate it is only calculate two iteration then it gives me negative cell volume error
- i am using S-A model
- velocity inlet 5m/s
- 0.0005 timestep

Sent from my SM-N920C using CFD Online Forum mobile app
mlberens is offline   Reply With Quote

Old   October 2, 2017, 14:02
Default
  #7
Senior Member
 
David Garlisch
Join Date: Jan 2013
Location: Fidelity Pointwise, Cadence Design Systems (Fort Worth, Texas Office)
Posts: 307
Rep Power: 13
dgarlisch is on a distinguished road
One other thing that I noticed is that the two sliding interface connectors are sharing end nodes. Topologically, this makes the grid point at this location shared by both the rotating near field domain AND the stationary far field domain.

I suspect that as the solution is running, this grid point is getting rotated by the inner domain. Since this point is also used by the outer domain, the outer domain becomes distorted resulting in the negative cells.

You see this in Pointwise by rotating the near field domains a few degrees. The far field domain will become distorted.


One way to fix this:
  • Select the large, near field domain and File, Save Selection... to Inner.pw
  • File, New...
  • File, Open... Inner.pw and Edit, Transform, Rotate... the interface connector by 180 degrees around (0,0,0)
  • File, Save... Inner.pw
  • File, New...
  • File, Open... the original file
  • Delete the large, near field domain and its outer (interface) connector.
  • File, Open... (append) Inner.pw.
  • Clean up the BCs and VCs
dgarlisch is offline   Reply With Quote

Old   October 2, 2017, 16:53
Default
  #8
New Member
 
muhamad elberens
Join Date: Feb 2017
Posts: 10
Rep Power: 7
mlberens is on a distinguished road
mr.david thanks so much for your support, that way is working well.



Sent from my SM-N920C using CFD Online Forum mobile app
mlberens is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[Other] refineWallLayer Error Yuby OpenFOAM Meshing & Mesh Conversion 2 November 11, 2021 12:04
how to set periodic boundary conditions Ganesh FLUENT 15 November 18, 2020 07:09
Negative Volume - apprentice madboy19 FLUENT 0 November 4, 2015 22:08
Cell centroid and cell volume in general, and in Fluent zmester Main CFD Forum 3 October 17, 2009 12:05
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55


All times are GMT -4. The time now is 20:44.