Source

This what I use as a starting point for the height of the first layer (source: Fluid Mechanics 101):

What I found from Wolf Dynamics. I'm not sure if its related to what you mentionned.

Somehow the reference length does matter I think, as it depends on if a body is bluff or streamlined, I find this kind of definitions a bit vague

This is good for a start, make a coarse mesh and see where your y+ within that mesh is.

This might help but I don't know anything about mr. or his extended family

What I do is to set up monitoring of quantities of interest and stop the simulation when they stop changing. Still it's good to have residuals as low as possible and min(p), max(U), max(p) within physically possible values

With pump simulations I monitor head, torque and forces, you would probably need to monitor drag and lift coefficients. In any case, if you use steady-state simulation as an initial guess for a transient, it doesn't matter that it converged properly, transient stuff will do that for you in the next few time steps

Your are mixing up stuff here. The Reynolds number of a flow in the common sense is just a measure of the inertial to viscous forces and is a global non-dimensional number. y+ is a non-dimensional measure of scale based on the viscosity and the wall normal velocity gradient and is thus a local number. This is completely decoupled from the definition of the Reynolds number thus decouple from your length scale. Now the equations @t_bo99 posted are an approximation of the wall normal velocity gradient for the FLAT PLATE. This can be APPROXIMATED by the Reynolds number of the flow. There is no other place the reference length of the Reynolds number goes into y+ except for the flat plate APPROXIMATION.

It's a thumb rule and the thumb is BIG

This is what I did basically and the values you see there is the exact one I used. And the mesh has non-orhtogonality < 60 and skewness < 4. I'm in a good range imo. The only things where it could have an issue, like I mentionned, are the schemes, BC or IC. But if I stick to what you said, even if the residuals don't reach the target, it make sense that the results at that point can be a relatively good IC in transient mode.

however you intend to refine your mesh, don't make boundary layers thinner than 1/4 or your current size

Is there a rational explaination behind this? Or its just by experience?

You have to capture laminar sublayer, buffer layer and transition to turbulent bulk flow. Laminar sublayer is somewhere within y+ < 5, and since flow there is laminar it makes no difference if you model it with 5 cells or 50 except that you'll waste resources

But it is important that you capture other stuff correctly

Assuming your y+ = ~4...5 with current mesh

I mean, you don't need to refine below y+ < 1

Ok, yes..I totaly understand what you mean. It's will decrease the size of the layer simply because I'll need to increase the velocity, but that doesn't influence de fact that if y+ = ~4...5 is respected, I still don't need that much layers in this zone..

If you change velocity, y+ will change and you'll have to adapt your mesh

Yes...that what I said but in more confusing way! So, finally, for the reason you just mentionned about the steady-state simulation, should I still try to validate or getting closer to the real value of y+ or just running a steady-state simulation, accepting the results and then going in transient mode right away to validate y+?

That depends, if you have validation data you can try with steady-state and see where it takes you. Most probably the results won't be the best and you'll continue with transient but even that doesn't guarantee better results

You'll have to get your hands dirty and see, I speak from my experience, yours will most probably be much different 🙂

What would be another way to get this gradient?

Instead of using an approximation based upon the reynolds number

Thanks for your answer btw, it is insightful 🙂

You solve the flow equations. Either numerically or analytical for something like coutte flow

You make me debating why I'm doing all that! 😆 I can't imagine that with transient simulation like IDDES I wouldnt be able to have decent results....

Here is a brief results I got by trying to make the Spalart-Allmaras turbulence model converge for a 3d geometry(disk). At iteration=500, we can see that from the result of velocity U that its look really symmetrical. But at around iter=800, something seems happening (behind the disk on the left portion(or top)) and seems to go toward another solution. By looking at the results at iter=1500 for instance, its clear that it become asymmetrical. We know that from the nature of the flow, there is a von Karman effect happening at a certain level of Re number. But, is that possible to reach a state of convergence for that type of geometry in RANS showing a symmetrical velocity field? The Re number is Re=24 500 (reference: diameter of the disk) or Re=7 950 (reference: thickness of the disk). Thank you for your insight.

you won't get a steady state solution