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

Cell pair was created...

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 14, 2021, 02:54
Default Cell pair was created...
  #1
New Member
 
Guillaume Beardsell
Join Date: Aug 2012
Posts: 17
Rep Power: 10
magicbretzel is on a distinguished road
Hi all,

I am running simulations of IC engines (moving boundaries) and shortly after I start the simulation I get this warning many times:

A cell pair was created with 16 cells at 0.00789812 0.00815266 0.00135936. This cell may reduce accuracy and/or stability. Consider refining the grid in this region. This warning will only be printed 50 times per process

What does it mean and how can I fix my mesh? I tried to refine the mesh as suggested but I keep getting the warning, so I am thinking that it might have something to do with my boundaries...

Cheers,
Guillaume
magicbretzel is offline   Reply With Quote

Old   February 16, 2021, 09:25
Default
  #2
Member
 
jetcheve's Avatar
 
John Etcheverry
Join Date: Dec 2018
Posts: 49
Rep Power: 4
jetcheve is on a distinguished road
Quote:
Originally Posted by magicbretzel View Post
Hi all,

I am running simulations of IC engines (moving boundaries) and shortly after I start the simulation I get this warning many times:

A cell pair was created with 16 cells at 0.00789812 0.00815266 0.00135936. This cell may reduce accuracy and/or stability. Consider refining the grid in this region. This warning will only be printed 50 times per process

What does it mean and how can I fix my mesh? I tried to refine the mesh as suggested but I keep getting the warning, so I am thinking that it might have something to do with my boundaries...

Cheers,
Guillaume

Hi, Guillaume!

When CONVERGE creates a mesh it looks at the volume of a cell cut by a surface compared to a normal neighboring cell. If the cut cell is less than 30% of the volume of the neighbor, the two are combined. If more cells are needed it combines more neighbors. If too many are needed the quality of the mesh can suffer - this is the warning you are seeing.

Often, in a ICE simulation this can occur in the valve gap. Does the coordinate provided match with the valves? Also, how big is the gap in your simulation and how big are the cells in it?

Thanks!

- John
__________________
John Etcheverry
Research Engineer
CONVERGECFD
jetcheve is offline   Reply With Quote

Old   February 16, 2021, 12:55
Default
  #3
New Member
 
Guillaume Beardsell
Join Date: Aug 2012
Posts: 17
Rep Power: 10
magicbretzel is on a distinguished road
Hi John,

Thanks for your answer! Here is a slice showing the mesh around the valves.

https://drive.google.com/file/d/1gmG...ew?usp=sharing

The cell size is 1mm around the valves, and the valve gap is 0.2 mm initially (closed position). When fully valve is fully open, the gap is about 6mm. I don't understand what you mean when you ask if the coordinate provided match with the valves. I believe that I need to refine the mesh locally around the valve gap?
magicbretzel is offline   Reply With Quote

Old   February 16, 2021, 13:58
Default
  #4
Member
 
jetcheve's Avatar
 
John Etcheverry
Join Date: Dec 2018
Posts: 49
Rep Power: 4
jetcheve is on a distinguished road
Quote:
Originally Posted by magicbretzel View Post
Hi John,

Thanks for your answer! Here is a slice showing the mesh around the valves.

https://drive.google.com/file/d/1gmG...ew?usp=sharing

The cell size is 1mm around the valves, and the valve gap is 0.2 mm initially (closed position). When fully valve is fully open, the gap is about 6mm. I don't understand what you mean when you ask if the coordinate provided match with the valves. I believe that I need to refine the mesh locally around the valve gap?
Guillaume - It looks like your embedding isn't fine enough in the area of the valve. I would increase embed scale on the valve angle and seat embedding by 2. Studio should also warn you if your embedding is too coarse resulting in possible pairing.

As for the point about checking if the coordinate provided is in the area of the valve - you can copy that coordinate and make a vertex at that point to see where it is. If it is in or close to the valve gap that would tell you if the valve is a possible culprit in your problem.

Thanks!

- John
__________________
John Etcheverry
Research Engineer
CONVERGECFD
jetcheve is offline   Reply With Quote

Old   February 16, 2021, 14:48
Default
  #5
New Member
 
Guillaume Beardsell
Join Date: Aug 2012
Posts: 17
Rep Power: 10
magicbretzel is on a distinguished road
John,

Indeed the coordinate of the problematic cell is very close to the valve angle. Adding embedding at the valve angle and seat solved the issue, I am not getting the cell pairing warning message anymore.

Thank you for your help!

Guillaume
magicbretzel is offline   Reply With Quote

Old   February 16, 2021, 14:51
Default
  #6
Member
 
jetcheve's Avatar
 
John Etcheverry
Join Date: Dec 2018
Posts: 49
Rep Power: 4
jetcheve is on a distinguished road
Quote:
Originally Posted by magicbretzel View Post
John,

Indeed the coordinate of the problematic cell is very close to the valve angle. Adding embedding at the valve angle and seat solved the issue, I am not getting the cell pairing warning message anymore.

Thank you for your help!

Guillaume
Great! Glad we could work that out for you.

- John
__________________
John Etcheverry
Research Engineer
CONVERGECFD
jetcheve 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
Error when running BuoyantBoussinesqSimpleFoam b.simpson OpenFOAM Running, Solving & CFD 8 June 26, 2020 09:18
Neighboring cells in tetrahedral mesh vishwesh OpenFOAM Programming & Development 9 November 10, 2017 07:06
[snappyHexMesh] Unwanted mesh created by snappyHexMesh--baffle bieshuxuhe OpenFOAM Meshing & Mesh Conversion 2 April 23, 2014 01:59
[Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Meshing & Mesh Conversion 2 July 15, 2005 04:15
cell to cell relation CMB Siemens 1 December 4, 2003 04:05


All times are GMT -4. The time now is 15:51.