[ghorrocks]

Massflow: Your third image. Sorry, it is actually velocity at some location, not massflow.

Convergence: Try loosening the convergence tolerance and see if it makes any difference. I suspect it will not make any difference, and it will allow you to run with larger time steps.

What for example can trigger instability?: Many, many things CFX is a numerical solver, and numerics needs to be stable to converge. For more details look in a numerical analysis or CFD textbook.

Damping in LES: LES models try to model the larger turbulence scales directly, and model the dissipation of the sub-grid scale turbulence with a sub grid model. For this to work you need to have low dissipation on the resolved scales and high dissipation in the sub grid model. This allows you to correctly model the turbulence energy spectrum and other turbulence dissipation features. If you add too much dissipation you will loose energy to a sloppy numerical method and you won't get the spectrum right, and you won't get turbulence at all in extreme cases. So you need to ensure you have very low dissipation to avoid these problems in LES. LES is much more sensitive to this than normal RANS simulations.

[balrog_f]

thanks four your answer. On the third image you can see the local velocity at the fictional inlet and outlet at the center of the respective faces.

[balrog_f]

Really struggling with this one ... can't figure out where this behaviour comes from and how it can be avoided.

[balrog_f]

Can this behaviour really be caused by bad mesh? Why is it stable then for such a "long" time? Can it be a problem of my dimpled plate, which I investigate, because the dimples work like a vortex generator? Has anybody experienced this behaviour? Is it possible that I just did too many timesteps?

[ghorrocks]

When a simulation goes unstable it can be from two sources: Physical instability or numerical instability.

Physical instabilities are generally well known, such as vortex streets, bluff bodies, Rayliegh-Taylor instabilities, turbulence transition in boundary layers. So you should be able to look at your results and know whether you have one of those.

Numerical instabilities are not real, and are caused by the solver not having adequate numerical stability to converge. They give impossible, non-physical results. You address these by improving the numerical stability: improve mesh quality, smaller time steps, better initial conditions, double precision solver and so on.

So your first step is to determine whether the instability is physical or numerical.

[balrog_f]

I did a mistake in my description of the case. My reynolds number calculated with the half the channel height is around 1200!! Could this be a problem as i am not investigating a fully turbulent flow? Reminder: i am investigating a channelflow with two infinite plates (periodic boundary) but one of the plates has dimples on it.


Sent from my iPhone using CFD Online Forum mobile app

[ghorrocks]

If the flow is laminar or transitional that is unlikely to change any issues of divergence at a boundary. I assume divergence at the outlet boundary remains the problem you wish to solve.

[balrog_f]

Thanks for your answer glenn but i have no outlet as i am using translational periodic boundary conditions. But i guess you meant the fictional outlet. The error also occurs on the fictional inlet.

I also tried a run with upwind as advection scheme which is way more dissipative, this one overcomes the error. But i guess the turbulence features i want to investigate is damped out by upwind schemes




Sent from my iPhone using CFD Online Forum mobile app

[ghorrocks]

You should be able to see the upwind advection scheme killing the turbulence spectrum. If you aren't looking at the turbulence spectrums, then you should be....