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

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

 July 20, 2006, 05:02 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 !

 July 20, 2006, 07:21 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

 July 20, 2006, 07:59 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!)

 July 20, 2006, 08:28 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.

 July 20, 2006, 08:34 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...

 July 20, 2006, 09:07 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.

 July 20, 2006, 09:27 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...

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

 July 21, 2006, 03:24 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"

 October 30, 2009, 09:50 #10 New Member   Join Date: Oct 2009 Posts: 26 Rep Power: 7 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.

 November 4, 2009, 01:17 #11 Senior Member     YH Tan Join Date: Mar 2009 Location: Malaysia Posts: 119 Rep Power: 8 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

 November 4, 2009, 07:46 #12 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 2,972 Rep Power: 30 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

 November 4, 2009, 08:01 #13 New Member   Join Date: Oct 2009 Posts: 26 Rep Power: 7 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.

 November 4, 2009, 08:16 #14 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 2,972 Rep Power: 30 *moving mesh? *2d-axi? __________________ In memory of my friend Hervé: CFD engineer & freerider

 November 4, 2009, 08:22 #15 New Member   Join Date: Oct 2009 Posts: 26 Rep Power: 7 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.

 November 4, 2009, 08:34 #16 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 2,972 Rep Power: 30 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

 November 4, 2009, 08:38 #17 New Member   Join Date: Oct 2009 Posts: 26 Rep Power: 7 Thanks a lot max. I will try these steps. If I have any trouble, I will ask you again

 November 4, 2009, 08:44 #18 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 2,972 Rep Power: 30 Tutorial 12 from Help may help you (Using Dynamic Meshes) __________________ In memory of my friend Hervé: CFD engineer & freerider

 November 4, 2009, 08:45 #19 New Member   Join Date: Oct 2009 Posts: 26 Rep Power: 7 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.

 November 4, 2009, 09:16 #20 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 2,972 Rep Power: 30 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post siw ANSYS Meshing & Geometry 4 September 3, 2014 05:25 gandesk FLUENT 0 November 29, 2010 18:50 SSL FLUENT 2 January 26, 2008 12:55 George Gardner FLUENT 0 January 13, 2006 12:08 hx li FLUENT 2 October 27, 2005 06:17

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