negative cells

yorelchr · April 1, 2014, 06:58

hello everyone,

I am working on an imported surface mesh generated by ANSA.
Importation is ok.
Then volume meshing with STARCCM+ is ok and when I check the mesh, no problem.
Then I put all my boundary conditions, models etc (these same conditions and models were ok on another case) then I directly have an overflow and the run stops. Then I have a message telling me that 2 cells have negative volume, how can it be possible if before launching the case, I had no errors?
Do someone kno how to deal with that?
Thank you very much.

ping · April 1, 2014, 10:01

did you do a mesh diagnostics after volume meshing, since this will report any negative volume cells - nothing to do with physics and boundary settings
so it could be cured earlier but the solve does not like them and does a check before iterating
use a threshold to find out where they are and preferably refine the mesh locally to rid them. otherwise use the remove invalid cell tool
i would alway suggest surface meshing again in starccm+ as a start before volume meshing and you will probably find the problem cells are where the mesh from ansa was not well made

yannaos · April 1, 2014, 15:35

One possible explanation is that the negative volume cells come directly after initialisation: if you have interfaces in your model then the interface matching is done during the initialisation and that matching could create negative volume cells. Big intersection tolerances (propery of the interface) could generate negative volume cells.
Another possibility: matching is between two surfaces with a great difference in cell size.

vangelis · April 3, 2014, 03:51

Hi Christine,

Have you checked the mesh in ANSA for negative elements?
Check>Mesh>Negative Volume
Does ANSA report anything?

Also do you have very small and large elements, for example
very thin high aspect ratio layers.
ANSA generates the mesh with double precision accuracy.
In such a case you would need to start Star in double precision also
as rounding up xyz coordinates may lead in negative elements
that did not really exist

Hope this helps

Vangelis

yorelchr · April 4, 2014, 07:48

Thank you all of you for your replies.
The check before running was ok, no errors reported; it's only after initalisation that problems occured. I have checked the mesh at the interfaces and indeed, there was too big differences between cells; I think problem was coming from that.
I have a new geometry now and I hope I won't have the same problem again.
Thanks!!!!

April 1, 2014, 06:58	negative cells	#1
yorelchr Senior Member christine Join Date: Jul 2009 Location: europe Posts: 125 Rep Power: 17	hello everyone, I am working on an imported surface mesh generated by ANSA. Importation is ok. Then volume meshing with STARCCM+ is ok and when I check the mesh, no problem. Then I put all my boundary conditions, models etc (these same conditions and models were ok on another case) then I directly have an overflow and the run stops. Then I have a message telling me that 2 cells have negative volume, how can it be possible if before launching the case, I had no errors? Do someone kno how to deal with that? Thank you very much.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Foam::error::PrintStack	almir	OpenFOAM Running, Solving & CFD	92	May 21, 2024 08:56
[snappyHexMesh] Snappy creates strange cells far away from boundary	vainilreb	OpenFOAM Meshing & Mesh Conversion	3	December 16, 2020 06:11
Negative cells in AutoGrid	funmaker	Fidelity CFD	4	July 17, 2012 06:34
Negative cells in AutoGrid5	sunset	Fidelity CFD	2	October 25, 2011 07:34
About negative volume of cells!	xhliu1	Siemens	0	April 16, 2005 00:49

April 1, 2014, 10:01		#2
ping Senior Member Ping Join Date: Mar 2009 Posts: 556 Rep Power: 20	did you do a mesh diagnostics after volume meshing, since this will report any negative volume cells - nothing to do with physics and boundary settings so it could be cured earlier but the solve does not like them and does a check before iterating use a threshold to find out where they are and preferably refine the mesh locally to rid them. otherwise use the remove invalid cell tool i would alway suggest surface meshing again in starccm+ as a start before volume meshing and you will probably find the problem cells are where the mesh from ansa was not well made

April 1, 2014, 15:35		#3
yannaos New Member Philhellene Ithaca Join Date: Mar 2014 Posts: 10 Rep Power: 12	One possible explanation is that the negative volume cells come directly after initialisation: if you have interfaces in your model then the interface matching is done during the initialisation and that matching could create negative volume cells. Big intersection tolerances (propery of the interface) could generate negative volume cells. Another possibility: matching is between two surfaces with a great difference in cell size.

April 3, 2014, 03:51		#4
vangelis Senior Member Vangelis Skaperdas Join Date: Mar 2009 Location: Thessaloniki, Greece Posts: 287 Rep Power: 21	Hi Christine, Have you checked the mesh in ANSA for negative elements? Check>Mesh>Negative Volume Does ANSA report anything? Also do you have very small and large elements, for example very thin high aspect ratio layers. ANSA generates the mesh with double precision accuracy. In such a case you would need to start Star in double precision also as rounding up xyz coordinates may lead in negative elements that did not really exist Hope this helps Vangelis

April 4, 2014, 07:48		#5
yorelchr Senior Member christine Join Date: Jul 2009 Location: europe Posts: 125 Rep Power: 17	Thank you all of you for your replies. The check before running was ok, no errors reported; it's only after initalisation that problems occured. I have checked the mesh at the interfaces and indeed, there was too big differences between cells; I think problem was coming from that. I have a new geometry now and I hope I won't have the same problem again. Thanks!!!!