
[Sponsors] 
March 18, 2012, 13:12 
Solver Settings for transient flow past circular cylinders

#1 
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4 
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 

March 19, 2012, 04:38 

#2 
Senior Member

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 GreenGauss 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 

March 19, 2012, 07:44 

#3 
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4 
Hello Amir
Thanks for your reply. Can you tell me more about Noniterative Time Advancement and Frozen Flux Formulation? Do I need to select one during simulation. I chose Noniterative Time Advancement with rest of the settings you mentioned. My time step was random that time ie 5e05. I noticed residuals oscillating with those settings. What can I do? Regards Mahindra 

March 19, 2012, 09:07 

#4  
Senior Member

Quote:
Frozen Flux Formulation: This procedure uses previous flux formulation in order to cancel nonlinearity. This method also should be avoided in high nonlinear 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 

March 19, 2012, 11:57 

#5 
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4 
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 

March 19, 2012, 12:18 

#6 
Senior Member
Join Date: May 2011
Location: Germany
Posts: 130
Rep Power: 6 
Have a look into the USER'S GUIDE.
The ideal number of iterations per time step is about 510. 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. 

March 19, 2012, 12:29 

#7  
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4 
Quote:
I have attached the residual variation I got. Does it make sense? Regards Mahindra 

March 19, 2012, 12:57 

#8 
New Member
Join Date: Jan 2012
Posts: 4
Rep Power: 0 
The trend of your residuals looks as expected.
To determine the timestep 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 1020 or more time steps per one shedding period. So dt=T/10, and smaller is better. 1020 iterations per timestep is adequate. Last edited by hda; March 19, 2012 at 12:58. Reason: grammar 

March 19, 2012, 14:06 

#9  
Senior Member

Quote:
Bests,
__________________
Amir 

March 19, 2012, 14:12 

#10  
Senior Member

Quote:
The reason of suggesting ideal iteration per time step is different! 510 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 

March 20, 2012, 05:49 

#11 
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4 
Hello
I am doing simulation and it will take some time. My query is do I need to select SkewnesNeighbor 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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
compressible flow calculation error using rhoSimpleFoam solver  student4326  OpenFOAM  6  February 10, 2012 10:36 
preconditioning 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 