CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   1st - 2nd order - convergence (https://www.cfd-online.com/Forums/fluent/35288-1st-2nd-order-convergence.html)

 antonio December 15, 2004 13:04

1st - 2nd order - convergence

Hi everybody, I'm running a simple 2D simulation. A cylinder (D=1 m) is placed on the ground (contact point in x=0, y=0). Air is entering the domain at 10 m/s. The domain is: [(x=-3 to 5), y=0 to 4]. Viscous model: Laminar.

I Run a simulation with the following scheme: [Pressure: Standard; P-V Coupling: SimpleC; Momentum: First Order Upwind] and the problem easily finds a convergence (1e-06).

If I change Momentum to [Second Order Upwind], the continuity residual shows an oscillatory behaviour at around 1e-04.

Do you have an idea what is this due to? Thank you very much,

antonio

 Jason December 15, 2004 13:15

Re: 1st - 2nd order - convergence

It's an unsteady problem. Bluff bodies are notoriously difficult to converge, especially cylinders because they lack a defined separation point. If you monitor your forces they'll oscillate as well. Your lift will have a regular oscillation while the drag looks more random, but still has underlying periodicity. If you plot your velocity vectors every so many iterations you'll notice the uneven vortices being shed by the body.

You can try switching to the coupled solver, with 2nd order discretization on flow. Since it's a density based solver, sometimes it can flatten out those oscillations. It's not a sure fix though.

I hope this helps.

Goodluck, Jason

 antonio December 15, 2004 17:38

Re: 1st - 2nd order - convergence

thank you very much. I monitored lift and drag coefficients and they do oscillate quite regurarly. Do you know if there is a way to relate the frequency of the "numerical" oscillation to the physical frequency?

 Jason December 16, 2004 09:21

Re: 1st - 2nd order - convergence

I've never been able to... I've been asked a few times to do that, but I haven't found a way to do it. If you do find a way can you post it on here?

If you've got the time, I would try running an unsteady solution. You can pull frequencies out of that.

Goodluck, Jason

 he December 16, 2004 09:37

Re: 1st - 2nd order - convergence

I would not waste time trying steady simulation on an unsteady flow problem. Why don't you switch to the unsteady solver which is just a few buttons away?

(1) Choose the second-order temporal scheme (2) Use SIMPLEC (3) Estimate time-step size based on, say, strouhal number of 0.2 such that would give scores of (>20) time steps in a period (4) Jack up the under-relaxation factors (e.g., 0.9 and 0.95 for pressure and momentum respectively) (5) Monitor and write CD and CL history (6) Use the built-in FFT capability in FLUENT

 All times are GMT -4. The time now is 07:06.