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

Solver Settings for transient flow past circular cylinders

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 18, 2012, 13:12
Default Solver Settings for transient flow past circular cylinders
  #1
Member
 
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4
mahi007 is an unknown quantity at this point
Hello all

I am newbie in CFD. I am working on flow past circular cylinder. I finished steady regimes in the flow. Now I turned to transient regime where vortex shedding starts.

As I am new to CFD, I am worried about the solver settings. Can someone explain me the best solver settings or how to start to arrive at the best settings?

Thanks

Regards
Mahindra
mahi007 is offline   Reply With Quote

Old   March 19, 2012, 04:38
Default
  #2
Senior Member
 
Amir's Avatar
 
Amir
Join Date: May 2009
Location: Shiraz, Iran
Posts: 739
Blog Entries: 1
Rep Power: 14
Amir is on a distinguished road
Dear Mahindra,

Regarding the solver settings, for such range of Re No. in vortex shedding (~90) the pressure based algorithm is adequate. The other settings which can help are:
- set Green-Gauss node based in gradient option
- using coupled or PISO algorithm are more adequate than SIMPLE in unsteady flows
- you can also improve accuracy by performing high order schemes
About setting proper time step/number of grid cell No., you have to use time step/grid study; i.e., you need to perform finer grids or time steps in order that the results would be independent of cell No. or time step size...

Bests,
__________________
Amir
Amir is offline   Reply With Quote

Old   March 19, 2012, 07:44
Default
  #3
Member
 
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4
mahi007 is an unknown quantity at this point
Hello Amir

Thanks for your reply. Can you tell me more about Non-iterative Time Advancement and Frozen Flux Formulation? Do I need to select one during simulation. I chose Non-iterative Time Advancement with rest of the settings you mentioned. My time step was random that time ie 5e-05. I noticed residuals oscillating with those settings. What can I do?

Regards
Mahindra
mahi007 is offline   Reply With Quote

Old   March 19, 2012, 09:07
Default
  #4
Senior Member
 
Amir's Avatar
 
Amir
Join Date: May 2009
Location: Shiraz, Iran
Posts: 739
Blog Entries: 1
Rep Power: 14
Amir is on a distinguished road
Quote:
Originally Posted by mahi007 View Post
Hello Amir

Thanks for your reply. Can you tell me more about Non-iterative Time Advancement and Frozen Flux Formulation? Do I need to select one during simulation. I chose Non-iterative Time Advancement with rest of the settings you mentioned. My time step was random that time ie 5e-05. I noticed residuals oscillating with those settings. What can I do?

Regards
Mahindra
Non-iterative Time Advancement: In this procedure, the equations are solved sequentially. As a general rule, these algorithms reduce the coupled nature of equations and may cause instabilities but obviously improve the numerical required time.
Frozen Flux Formulation: This procedure uses previous flux formulation in order to cancel non-linearity. This method also should be avoided in high non-linear cases (high Re No.)
As a first try I think you don't need these methods; you can think about them in latter steps for improving computational effort which obviously case dependent. So I suggest not to activate these methods first. About time step, as I said you have to perform time step study in order to find proper time step.
About oscillating residuals, you can use lower relaxation factors or more diffusive schemes like upwind or use SIMPLE algorithm as your first try. (Also activating a turbulent model to capture vortices may help)

Bests,
__________________
Amir
Amir is offline   Reply With Quote

Old   March 19, 2012, 11:57
Default
  #5
Member
 
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4
mahi007 is an unknown quantity at this point
Hello Amir

I tried with the settings you mentioned, but residuals are increasing after every time step. I am attaching graph of residuals. How the residuals are supposed to change for a convergent solution?

Also how many iterations are good enough for each time step?

Regards
Mahindra
Attached Images
File Type: jpg fluent.jpg (55.7 KB, 22 views)
mahi007 is offline   Reply With Quote

Old   March 19, 2012, 12:18
Default
  #6
Senior Member
 
Join Date: May 2011
Location: Germany
Posts: 130
Rep Power: 6
Zigainer is on a distinguished road
Have a look into the USER'S GUIDE.

The ideal number of iterations per time step is about 5-10. If FLUENT needs more, you should decrease your time step. If FLUENT needs less you can increase your time step. You can also start with a smaller time step for the first couple of iterations and then increase your time step.
Zigainer is offline   Reply With Quote

Old   March 19, 2012, 12:29
Default
  #7
Member
 
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4
mahi007 is an unknown quantity at this point
Quote:
Originally Posted by Zigainer View Post
Have a look into the USER'S GUIDE.

The ideal number of iterations per time step is about 5-10. If FLUENT needs more, you should decrease your time step. If FLUENT needs less you can increase your time step. You can also start with a smaller time step for the first couple of iterations and then increase your time step.
Hey thank you for your reply. Do you have idea about variation trend of residuals in unsteady flow?

I have attached the residual variation I got. Does it make sense?

Regards
Mahindra
mahi007 is offline   Reply With Quote

Old   March 19, 2012, 12:57
Default
  #8
hda
New Member
 
Join Date: Jan 2012
Posts: 4
Rep Power: 0
hda is on a distinguished road
The trend of your residuals looks as expected.

To determine the time-step dt, consider the expected shedding frequency. You can approximately know the shedding frequency (f_shed [Hz]) using Strouhal number at that Re. (look it up online). The shedding period (in seconds [s]) is T=1/f_shed. You should have about 10-20 or more time steps per one shedding period. So dt=T/10, and smaller is better.

10-20 iterations per timestep is adequate.

Last edited by hda; March 19, 2012 at 12:58. Reason: grammar
hda is offline   Reply With Quote

Old   March 19, 2012, 14:06
Default
  #9
Senior Member
 
Amir's Avatar
 
Amir
Join Date: May 2009
Location: Shiraz, Iran
Posts: 739
Blog Entries: 1
Rep Power: 14
Amir is on a distinguished road
Quote:
Originally Posted by mahi007 View Post
Hello Amir

I tried with the settings you mentioned, but residuals are increasing after every time step. I am attaching graph of residuals. How the residuals are supposed to change for a convergent solution?

Also how many iterations are good enough for each time step?

Regards
Mahindra
The trend is correct; after each time step it has a jump. increase iteration per time step in a manner to decrease the residuals in each time step.

Bests,
__________________
Amir
Amir is offline   Reply With Quote

Old   March 19, 2012, 14:12
Default
  #10
Senior Member
 
Amir's Avatar
 
Amir
Join Date: May 2009
Location: Shiraz, Iran
Posts: 739
Blog Entries: 1
Rep Power: 14
Amir is on a distinguished road
Quote:
Originally Posted by Zigainer View Post
The ideal number of iterations per time step is about 5-10. If FLUENT needs more, you should decrease your time step. If FLUENT needs less you can increase your time step. You can also start with a smaller time step for the first couple of iterations and then increase your time step.
Dear Zigainer,

The reason of suggesting ideal iteration per time step is different! 5-10 time step is ideal for reducing computational effort. Generally, the correct number of iteration per time step should be specified with a try & error procedure to justify the accuracy and computational effort. seems that you've mixed accuracy and convergency!

Bests,
__________________
Amir
Amir is offline   Reply With Quote

Old   March 20, 2012, 05:49
Default
  #11
Member
 
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4
mahi007 is an unknown quantity at this point
Hello

I am doing simulation and it will take some time. My query is do I need to select Skewnes-Neighbor Coupling? What does it do?


Also lift coefficient is not varying in sinusoidal fashion. Actually my simulation hasnt completed a vortex shedding time. But my initial feeling is it is varying randomly. What can i do?

Thanks

Regards
MAhindra
mahi007 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
compressible flow calculation error using rhoSimpleFoam solver student4326 OpenFOAM 6 February 10, 2012 10:36
pre-conditioning for low mach number compressible flow solver Shenren_CN Main CFD Forum 0 April 29, 2011 21:07
flow past abdominal aorta. Complex BC problem. ziemowitzima OpenFOAM Running, Solving & CFD 0 April 5, 2010 13:30
Tubulent flow past circular cylinder at Re=3900 Jinglei Main CFD Forum 1 September 11, 2007 06:05
flow past circular cylinder E.le stanc Main CFD Forum 16 November 24, 2006 09:48


All times are GMT -4. The time now is 07:25.