CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT > Fluent UDF and Scheme Programming

How to eliminate error "Update-Dynamic-Mesh failed. Negative cell volume detected" in

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

Like Tree6Likes
  • 3 Post By `e`
  • 3 Post By Ved1994

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 14, 2016, 13:52
Post How to eliminate error "Update-Dynamic-Mesh failed. Negative cell volume detected" in
  #1
New Member
 
khairil hafizi
Join Date: Sep 2015
Posts: 6
Rep Power: 6
bobdorm14 is on a distinguished road
Hi everyone,

I am doing aeroelasticity simulation for 2D airfoil.I'm trying to do a simulation of a wing that is both pluging*and pitching.


I have created 2 types of mesh using GAMBIT sotware

1)structured mesh (consist of square grid)

2)unstructured mesh consist of triangles shape grid.

I run the simulation in fluent by compiling the UDF .c file for both type of mesh.

everything goes well for unstructured mesh.when I click "preview mesh motion" button under dynamic mesh I can see the movement of the airfoil.but the quality for this type of mesh is very low.

for structured mesh,fluent gives me an error "Update-Dynamic-Mesh failed". Negative cell volume detected" for the same model.I enable the 3 methods (layering,smoothing and remeshing) under "mesh method"

can anybody help me on this.

How to eliminate error "Update-Dynamic-Mesh failed. Negative cell volume detected" in Fluent? - ResearchGate. Available from: https://www.researchgate.net/post/Ho...cted_in_Fluent [accessed Jun 15, 2016].
bobdorm14 is offline   Reply With Quote

Old   June 14, 2016, 18:20
Default
  #2
`e`
Senior Member
 
Join Date: Mar 2015
Posts: 892
Rep Power: 13
`e` is on a distinguished road
The dynamic mesh model in Fluent can handle both structured and unstructured meshes. However, MDM does not remesh structured cells -- only unstructured cells.

What degree of motion is your aerofoil experiencing? You may be able to employ the smoothing mesh method (no modifications of the mesh; only moves nodes based on either a diffusion equation or spring system).

There are three zones to specify as dynamic mesh zones: (1) aerofoil (probably a user-defined type which both translates and rotates the aerofoil boundary); (2) sides of domain (set as deforming); and (3) interior (also set as deforming).

The negative cell volume error is shown when the mesh has been updated in a way to cause a negative cell volume (non-physical). Possible factors for causing this error include: (1) overlapping nodes; and (2) significant mesh motion (relative to cell size) per step. These factors are related and you could try to reduce the time step to avoid major mesh displacements (see also: implicit mesh update).
`e` is offline   Reply With Quote

Old   April 6, 2017, 03:24
Default
  #3
New Member
 
Join Date: Dec 2015
Location: Japan
Posts: 25
Rep Power: 5
kywong5 is on a distinguished road
Hi bobdorm14, are you able to solve the problem as mentioned?
I'm facing the same situation too.
kywong5 is offline   Reply With Quote

Old   May 31, 2017, 05:14
Default
  #4
New Member
 
srcredchi
Join Date: May 2017
Posts: 20
Rep Power: 4
Sandeep Reddy is on a distinguished road
Quote:
Originally Posted by kywong5 View Post
Hi bobdorm14, are you able to solve the problem as mentioned?
I'm facing the same situation too.
Me too, did you get any solution?
Sandeep Reddy is offline   Reply With Quote

Old   August 12, 2017, 13:41
Default
  #5
New Member
 
flanag
Join Date: Jun 2017
Posts: 12
Rep Power: 4
lfla is on a distinguished road
Encountering the same problem have you got a solution for this? As the only one i have had was to put a very coarse mesh which i would rather not. Thank you
lfla is offline   Reply With Quote

Old   September 15, 2017, 16:06
Default
  #6
New Member
 
VM
Join Date: Jun 2017
Posts: 5
Rep Power: 4
Ved1994 is on a distinguished road
I assume most of us get this error because the moving boundary is travelling more than half of the adjacent cell height in one time step. So, if you are limited by hardware, a solution would be to coarsen the mesh. If you have good firepower at your disposal, you can further decrease the time step to a point so that at any time step during the simulation time your object is not travelling more than the adjacent cell height in one time step.
fondexx, dengdeng and mahdihasan like this.
Ved1994 is offline   Reply With Quote

Old   September 22, 2017, 20:58
Lightbulb
  #7
New Member
 
Ian Carlo M. Lositaņo
Join Date: Mar 2017
Location: Legazpi City, Philippines
Posts: 14
Rep Power: 4
iancmlositano is on a distinguished road
Quote:
Originally Posted by bobdorm14 View Post
Hi everyone,

I am doing aeroelasticity simulation for 2D airfoil.I'm trying to do a simulation of a wing that is both pluging*and pitching.


I have created 2 types of mesh using GAMBIT sotware

1)structured mesh (consist of square grid)

2)unstructured mesh consist of triangles shape grid.

I run the simulation in fluent by compiling the UDF .c file for both type of mesh.

everything goes well for unstructured mesh.when I click "preview mesh motion" button under dynamic mesh I can see the movement of the airfoil.but the quality for this type of mesh is very low.

for structured mesh,fluent gives me an error "Update-Dynamic-Mesh failed". Negative cell volume detected" for the same model.I enable the 3 methods (layering,smoothing and remeshing) under "mesh method"

can anybody help me on this.

How to eliminate error "Update-Dynamic-Mesh failed. Negative cell volume detected" in Fluent? - ResearchGate. Available from: https://www.researchgate.net/post/Ho...cted_in_Fluent [accessed Jun 15, 2016].

Negative cells mean such cells do not follow the right hand rule (RHR). Can you check the orientation of those blocks of cells? It may be that during meshing, these cells have been oriented to go against the flow. The solution would be to just re-orient them.
iancmlositano is offline   Reply With Quote

Reply

Tags
dynamic mesh;, fluent - udf, gambit 2.2.30

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
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 32 February 7, 2018 09:26
Negative cell volume detected, dynamic mesh tony25800 FLUENT 6 September 17, 2014 20:50
[blockMesh] error message with modeling a cube with a hold at the center hsingtzu OpenFOAM Meshing & Mesh Conversion 2 March 14, 2012 10:56
[Other] mesh airfoil NACA0012 anand_30 OpenFOAM Meshing & Mesh Conversion 12 December 12, 2011 05:16
[OpenFOAM] ParaView/Parafoam error when making animation Disco_Caine ParaView 6 September 28, 2010 10:54


All times are GMT -4. The time now is 21:53.