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

Non positive volume exist - How to find where ??!!

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 20, 2006, 05:02
Default Non positive volume exist - How to find where ??!!
  #1
Cyril
Guest
 
Posts: n/a
I've just finished my mesh, and fluent tells me that "non positive volume exists".

Houw can I do to find where, and correct it ???

Many thanks !
  Reply With Quote

Old   July 20, 2006, 07:21
Default Re: Non positive volume exist - How to find where
  #2
Zafer Zeren
Guest
 
Posts: n/a
When I got the same problem, I always make smoothing and then read the mesh file into fluent again. I use ICEM CFD. That can work.

zafer
  Reply With Quote

Old   July 20, 2006, 07:59
Default Re: Non positive volume exist - How to find where
  #3
Cyril
Guest
 
Posts: n/a
How do you smoth ??

(the part of my geometry which causes the problem is a single parallelogram, meshed in tri...! there is no curve!)
  Reply With Quote

Old   July 20, 2006, 08:28
Default Re: Non positive volume exist - How to find where
  #4
Zafer Zeren
Guest
 
Posts: n/a
I use ICEM CFD to generate mesh. Smoothing is under "edit mesh" menu. I have structured + unstructured hybrid mesh around a bluff body. You can there smooth you mesh.

  Reply With Quote

Old   July 20, 2006, 08:34
Default Grrrr !
  #5
Cyril
Guest
 
Posts: n/a
The problem, is that I'm running a 2D case... I don't understand why I've got a volume (negative or positive...)

I'don't have icem cfd...
  Reply With Quote

Old   July 20, 2006, 09:07
Default Re: Grrrr !
  #6
Jason
Guest
 
Posts: n/a
Is it axisymmetric? If so, then you're problem is that you're below the X-Axis. In Fluent 2Daxi model, you must use the X-Axis as your axis of rotation, and your geometry must all lie in the +Y direction (above the X Axis).

Hope this helps, and good luck, Jason
misagh and Pacific like this.
  Reply With Quote

Old   July 20, 2006, 09:27
Default Re: Grrrr !
  #7
Cyril
Guest
 
Posts: n/a
Thanks, but the face involved is far from the X axis. when I export the face alone (no mesh) everything's ok.

And when I mesh it -> I get a neg volume...
  Reply With Quote

Old   July 20, 2006, 10:35
Default find out !
  #8
Cyril
Guest
 
Posts: n/a
"Gambit error, not found in gambit, but detected by fluent" the hotline said !
  Reply With Quote

Old   July 21, 2006, 03:24
Default Re: find out !
  #9
Tayfun
Guest
 
Posts: n/a
I had the same problem in FLUENT, here is the way I solve it:

In FLUENT, you type(!) the following;

1. g 2. mz 3. rfh

This converts the negative volumes to positive for 2D case.

NOTE: "g" means "grid", "mz" means "modify zones" and "rfh" means "right face handedness"

  Reply With Quote

Old   October 30, 2009, 09:50
Default
  #10
New Member
 
Join Date: Oct 2009
Posts: 26
Rep Power: 7
mayur is on a distinguished road
Dear Tayfun,

I tried to follow the steps of Grid, modify zones, rfh. It says the negative volume have been converted but after checking the grid, it still says negative volume exists. Can you please help me in this.
mayur is offline   Reply With Quote

Old   November 4, 2009, 01:17
Default
  #11
Senior Member
 
herntan's Avatar
 
YH Tan
Join Date: Mar 2009
Location: Malaysia
Posts: 119
Rep Power: 8
herntan is on a distinguished road
I think maybe u can try to round/fillet all those edges.
sharp edges can give many problem while meshing.

Anyhow, just a suggestion.
__________________
Herntan,

Add Reputation if I am right
herntan is offline   Reply With Quote

Old   November 4, 2009, 07:46
Default
  #12
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
If you have negative volume, the best way is to correct your mesh.
If you work with Gambit go back over there, and see where are those cells
Examine Mesh / Volume ... set the upper limit to 0
It will show you all the negative cells
Then correct your topology for avoiding this issue
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   November 4, 2009, 08:01
Default
  #13
New Member
 
Join Date: Oct 2009
Posts: 26
Rep Power: 7
mayur is on a distinguished road
Actually when I create the mesh, it shows positive volume. but as soon as I start the iteration in Fluent, it shows negative volume detected. I even checked the mesh parameters. The Grid info before iteration shows, Xmin = 0, Xmax=0.084 and Ymin=0, Ymax=0.09. After starting iterations, when I check the grid values, the values of Xmin and Ymin are changed. I even tried translation of the coordinates in Fluent, but it doesnt help.
mayur is offline   Reply With Quote

Old   November 4, 2009, 08:16
Default
  #14
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
*moving mesh?
*2d-axi?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   November 4, 2009, 08:22
Default
  #15
New Member
 
Join Date: Oct 2009
Posts: 26
Rep Power: 7
mayur is on a distinguished road
Ya.. I am trying a moving mesh. Actually I am trying to compress fluid using fluent. I am using a simple rectangular geometry. The top wall, the side walls which are deforming and the bottom wall is the moving wall. I have drawn the geometry in a positive XY co-ordinate system.
mayur is offline   Reply With Quote

Old   November 4, 2009, 08:34
Default
  #16
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
ok, then your initial grid is ok, and your issue remains in the MDM-set up.
you have to set the moving wall as rigid body (here you have to give the motion with a profile or a UDF)
The side walls (adjacent to moving wall) as deforming
and the last one as stationnary.
Pay attention to meshing options panel, bad values will generate bad mesh
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   November 4, 2009, 08:38
Default
  #17
New Member
 
Join Date: Oct 2009
Posts: 26
Rep Power: 7
mayur is on a distinguished road
Thanks a lot max.

I will try these steps.
If I have any trouble, I will ask you again
mayur is offline   Reply With Quote

Old   November 4, 2009, 08:44
Default
  #18
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
Tutorial 12 from Help may help you (Using Dynamic Meshes)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   November 4, 2009, 08:45
Default
  #19
New Member
 
Join Date: Oct 2009
Posts: 26
Rep Power: 7
mayur is on a distinguished road
Max,

I have one more query, I am defining the zones as you explained. While,defining the meshing options, we have to describe the cell height. Is there any way to find the optimum value as per the geometry. My current geometry is 84mm in length and 90 mm in height.

Thanks for your help.
mayur is offline   Reply With Quote

Old   November 4, 2009, 09:16
Default
  #20
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
I don't know anymore (I switched to OpenFOAM, I am not using Fluent anymore)
But I think there is a Panel "Geometry Definition" or something like that, which gives you some info about cell height.
But basically, if you have meshd your stuff you can remember the cell height.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- 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
[ICEM] Negative volume error in hybrid mesh siw ANSYS Meshing & Geometry 4 September 3, 2014 05:25
Find volume bulk temperature gandesk FLUENT 0 November 29, 2010 18:50
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
Splitting Up Volume George Gardner FLUENT 0 January 13, 2006 12:08
the Eulerian model and the lower volume fraction hx li FLUENT 2 October 27, 2005 06:17


All times are GMT -4. The time now is 17:42.