[mahi007]

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

[Amir]

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,

[mahi007]

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

[Amir]

Originally Posted by mahi007

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,

[mahi007]

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

[Zigainer]

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.

[mahi007]

Originally Posted by Zigainer

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

[hda]

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.

[Amir]

Originally Posted by mahi007

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]

Originally Posted by Zigainer

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,

[mahi007]

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