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

Issue of divergence

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

Like Tree4Likes
  • 1 Post By Jeff P.
  • 1 Post By FMDenaro
  • 1 Post By arjun
  • 1 Post By FMDenaro

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 15, 2016, 02:32
Default Issue of divergence
  #1
New Member
 
hemant mittal
Join Date: Feb 2016
Posts: 21
Rep Power: 10
hemmt is on a distinguished road
Hello every one,
I m simulating wind flow around rectangular buildings using LES on Ansys/Fluent.the problem of divergence is detected during the simulation after
flow time of 3 sec.
time step size = .0005
Vortex method (no. of vortices = 190) for turbulence generation
Polyhedral mesh is being used
So please guide me how to resolve this issue.


Thanks
hemmt is offline   Reply With Quote

Old   July 15, 2016, 12:02
Default
  #2
New Member
 
Jeff
Join Date: Jun 2016
Posts: 20
Rep Power: 9
Jeff P. is on a distinguished road
Your time step may be too long to capture the vorticies forming at the building edges depending on flow speed and mesh density. Without further info and assuming your mesh is good, its my best idea.
hemmt likes this.
Jeff P. is offline   Reply With Quote

Old   July 15, 2016, 12:29
Default
  #3
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,760
Rep Power: 71
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Depending on the SGS model, cell dimension, cfl, the added eddy viscosity can drive to numerical instability for that time-step....

Could you address all the details of your LES setting?
hemmt likes this.
FMDenaro is offline   Reply With Quote

Old   July 15, 2016, 13:31
Default
  #4
New Member
 
hemant mittal
Join Date: Feb 2016
Posts: 21
Rep Power: 10
hemmt is on a distinguished road
Hello sir.
thanks for reply,

I m using dynamic subgrid scale model.
first cell height is 0.000125m
wind speed at building height=9.5 m/s
vortex method is used to add turbulence and of vortices =190
CFL condition for most of cell around building is <1
no. of polyhedral cells are about 1.9 million
hemmt is offline   Reply With Quote

Old   July 15, 2016, 13:36
Default
  #5
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,760
Rep Power: 71
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
what kind of method are you using? did you set second order in time and space? is the numerical instability onset after many time steps?
FMDenaro is offline   Reply With Quote

Old   July 15, 2016, 13:37
Default
  #6
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,273
Rep Power: 34
arjun will become famous soon enougharjun will become famous soon enough
Quote:
Originally Posted by hemmt View Post
Hello every one,
I m simulating wind flow around rectangular buildings using LES on Ansys/Fluent.the problem of divergence is detected during the simulation after
flow time of 3 sec.
time step size = .0005
Vortex method (no. of vortices = 190) for turbulence generation
Polyhedral mesh is being used
So please guide me how to resolve this issue.


Thanks
Seeing how fluent is, if I have to guess, I would guess that your mesh is too coarse. When the grid is coarse, specially when we are talking of buildings, the disspation that keeps velocity and pressure coupled is too low and equations decouple.

Refine the mesh a bit further and see, how it behaves.

I guess to make things worse times step is too low too (which also reduces dissipation).
hemmt likes this.
arjun is offline   Reply With Quote

Old   July 15, 2016, 13:47
Default
  #7
New Member
 
hemant mittal
Join Date: Feb 2016
Posts: 21
Rep Power: 10
hemmt is on a distinguished road
spatial discretization for Pressure is second order and for momentum it is bounded central differencing.
time discretization scheme is second order implicit.

Numerical instability occurred after 6880 time steps.
hemmt is offline   Reply With Quote

Old   July 15, 2016, 13:58
Default
  #8
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,760
Rep Power: 71
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
have you tried setting a smaller dt?
you should check some typical variable such as rms and spectra to see if you get energy pile-up.

Just as check of validation, try the same discretization setting the static smagorinsky model but with Cs=0 (no-model) and reduce the Reynolds number. See if you get a stable unsteady solution.
hemmt likes this.
FMDenaro is offline   Reply With Quote

Old   July 15, 2016, 13:59
Default
  #9
New Member
 
hemant mittal
Join Date: Feb 2016
Posts: 21
Rep Power: 10
hemmt is on a distinguished road
Quote:
Originally Posted by arjun View Post
Seeing how fluent is, if I have to guess, I would guess that your mesh is too coarse. When the grid is coarse, specially when we are talking of buildings, the disspation that keeps velocity and pressure coupled is too low and equations decouple.

Refine the mesh a bit further and see, how it behaves.

I guess to make things worse times step is too low too (which also reduces dissipation).
Thank You sir
I will do this..........
hemmt 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
PEMFC model with FLUENT brahimchoice FLUENT 22 April 19, 2020 16:44
[ANSYS Meshing] Help with element size sandri_92 ANSYS Meshing & Geometry 14 November 14, 2018 08:54
fluent divergence for no reason sufjanst FLUENT 2 March 23, 2016 17:08
Divergence problem Smaras FLUENT 13 February 21, 2013 06:03
3d vof Smaras FLUENT 2 February 19, 2013 07:58


All times are GMT -4. The time now is 09:45.