Convergence too fast
 

Hi. I'm simulating the rear spoiler of a car. My problem is that my solution converges too fast, after 150 iterations. My turbulence model is k-ω SST, double precision. Coupled scheme, second order discretization. Y+ is around 1, under-relaxation factors in default. Mesh size is around 8000000 (spoiler total length is around 650mm). Velocity residuals 10^-6, omega 10^-4, k 10^-3, continuity ~0.5*10^-3

Is it normal to converge so quick? Should I increase the mesh size in order to get a more accurate solution? Am I missing something?

I would rather stick to at least 1e-4 for continuity. Why don't you try a finer mesh to see if there is a change in the solution?
Assuming the fluid is air!, the Reynolds number should be around 3-5M (for velocities around 40-50 m/s). For an external flow! it's not a high-intensity turbulence problem. I can't see why 150 iterations cannot be right.

I guess you are using the pressure-based solver with the COUPLED scheme for the pressure-velocity coupling?

Actually, considering 8 million cells, 150 iterations does sound too fast. It's possible if you have a really good initial guess (for all variables: pressure, velocity, k, omega), or if you already had a converged solution to a similar problem and made a minor tweak to a boundary condition, but that doesn't seem to be the case. I would run it some more to check and be safe.

But two things to consider:

After the governing equations are linearized, each local cell does not feel the influence of far away cells. Far in this sense means more than 1 or 2 cells away. Each cell only feels its far neighbors after the solution is updated at the next iteration. Although the AMG accelerates this process, you can imagine it takes many iterations for this propagation to take place. For example, it generally takes 30-100 iterations for the pressure field to even look right when you initialize it with a bad initial guess, i.e. a constant pressure field.

The other thing is coupling between the continuity & momentum w/ the turbulence model. Even if you used the coupled scheme for the pressure-velocity coupling (continuity & momentum are coupled), the turbulence model is still segregated. The coupling between equations only happens after the updated solution is available at the next iteration.

Thanks for your replies! Yes I'm using the pressure-based solver with the coupled scheme. I didn't use anything as an initial guess.
I set the continuity residuum in 1e-4 like sina_mech suggested and now I'm getting oscillating residuals.

Try to decrease the under-relaxation factors for the oscillating residuals.
However, remember to have some monitor points in your domain so you can make sure you achieve a locally fair convergence too. Small scaled residuals are not sufficient and sometimes can be actually misleading.

I'll give it a try. I am also monitoring the drag and lift coefficients. After I get a convergence with the decreased under-relaxation factor, should I set them back in default and recalculate?

I would leave the urf's default and never reduce them unless you have a floating point error.

Watch your monitors to see whether they oscillate with a high amplitude and become periodic or if they are more or less monotonic/asymptotic. Look for how many iterations it takes to enter this state.

It's very typical for residuals to drop really nicely in early iterations and then increase or oscillate later. This is because you usually initialize with a uniform flow that already satisfies the transport equations, but not the boundary conditions. It's not until you do several iterations that the flow "learns" it is in the wrong state.