[eilloo]

Hi all,

I am trying to understand whether we would expect to see the same results in a 2D simulation of an aerofoil, as we would if that same 2D mesh was extruded by a few cells in the z direction?

Boundary conditions wise, the 3D case would have zero velocity in the z direction prescribed for the front and back faces (in the spanwise direction), a velocity inlet with no z component, and a zero pressure outlet.

Would you expect to see flow (for instance, vortices) develop in the z direction in a 3D case like this?
On one hand, it seems like this should represent an infinite wing case, so the flow would be identical to a 2D aerofoil.
On the other, I can imagine things such as round off errors or imperfections in the mesh inducing some z-velocity as the flow develops. Once this starts, perhaps the simulation would become sensitive to things such as resolution in the z direction?

Two questions are:
1. Does the simulation setup described actually represent an infinite wing?
2. Would you expect to see different results compared to the purely 2D case?

Thanks in advance for the insight!

[FMDenaro]

Originally Posted by eilloo

Hi all,

I am trying to understand whether we would expect to see the same results in a 2D simulation of an aerofoil, as we would if that same 2D mesh was extruded by a few cells in the z direction?

Boundary conditions wise, the 3D case would have zero velocity in the z direction prescribed for the front and back faces (in the spanwise direction), a velocity inlet with no z component, and a zero pressure outlet.

Would you expect to see flow (for instance, vortices) develop in the z direction in a 3D case like this?
On one hand, it seems like this should represent an infinite wing case, so the flow would be identical to a 2D aerofoil.
On the other, I can imagine things such as round off errors or imperfections in the mesh inducing some z-velocity as the flow develops. Once this starts, perhaps the simulation would become sensitive to things such as resolution in the z direction?

Two questions are:
1. Does the simulation setup described actually represent an infinite wing?
2. Would you expect to see different results compared to the purely 2D case?

Thanks in advance for the insight!

Infinite wing is represented in 2d.
On the other hand, a small spanwise extension can resolve only vortical structures of that integral lenght. Be aware that if you prescribe a periodi al condition the flow repeats itself infinitely.

However, first of all that male sense only if you perform DNS or LES. Otherwise there is no meaning, the statistical steady solution is 2d.

[eilloo]

Thanks Filippo,

Supposing we use DNS or LES, how might span-wise vortical structures be introduced to the flow?
The inlet condition is for flow velocities only in x and y, and there are no-slip conditions imposed on the 'front' and 'back' faces as described above.

Would small, numerical errors be enough to induce this, or might there be other mechanisms? Or perhaps this would not be expected at all...

[sbaffini]

Originally Posted by eilloo

Thanks Filippo,

Supposing we use DNS or LES, how might span-wise vortical structures be introduced to the flow?
The inlet condition is for flow velocities only in x and y, and there are no-slip conditions imposed on the 'front' and 'back' faces as described above.

Would small, numerical errors be enough to induce this, or might there be other mechanisms? Or perhaps this would not be expected at all...

Formally, for a DNS or LES to be called so, being both unsteady and 3D, you HAVE TO provide them the sufficient computational conditions to behave in that way. Said otherwise, actual flows, which DNS and LES pretend to describe down to "very small scales", are ALWAYS 3D and unsteady for at least few of those scales. In this sense, it is up to you to understand what those scales are, how they interact with other scales and, in summary, the largest and smallest length scale that need to be represented in each spatial direction and in time for your DNS and LES to be correct.

For example, if it is a creeping flow, it may be possible that the actual flow is truly 2D, so you don't really need a 3rd dimension in your computation and still formally call your simulation a DNS (altough, a very simple one that doesn't involve turbulence). In contrast, for a sufficiently high Re number, any sort of small disturbance will eventually drive the flow toward 3D and unsteadyness. It might still be laminar to a very large extent, but once instabilities kick in you can say goodbye to a pure 2D setting, at least formally. For some intermediate Re numbers it might still be possible in controlled laboratory experiments to somehow keep the flow stable, but that just shifts the problem to an higher Re number (still, quite low in absolute terms) and, in the end, you typically want to reproduce the most probable flow outcome, not some weird laboratory setting which is practically irreproducible in real life.

Hence, if you are chasing turbulent flows over wings, even if at relatively low Re numbers, you need to start from the fact that they are 3D and unsteady and so must be their relative LES/DNS. Is it possible to achieve a laboratory condition where they are instead 2D and steady? I cannot exclude it, but then you need to reeplicate that exact laboratory condition in your simulation, not a generic flow over a 3D wing. You could still call it a DNS in that case (I don't think there is space or need anymore for the LES term in such simpified laminar cases), altough a very simplified one.

So, for your turbulent flow over a generic 3D wing (altough with constant cross section along the third direction), you need a 3D unsteady approach. Where does the 3D unsteady content comes from? In the real flow, from boundary conditions, surface imperfections and instability will take it from there. To what extent those inputs will be converted into transverse motion? Depends from the specific flow and Re number. Do you need to take them into account for your DNS/LES? Yes, if you want to consider the most probable flow condition.

All of them? Probably not. I think I never saw a DNS/LES study on the effect of surface imperfections (but those will have an effect also on a RANS or inviscid computation). Typically, it is at inlet where DNS/LES simulations provide their 3D/unsteady content.

It is less obvious and seen in practice, but even simple asymmetries always present in actual codes could actually promote instabilities for sufficiently resolved and high re DNS cases (I have serious doubts for LES).

[sbaffini]

Getting more specifically to your questions:

- your 2D simulation won't correctly become a 3D one with just few cells in z. You need a minimum z extension for the domain to accomodate the largest structures expected and a certain number of points to accomodate the smallest ones.

- boundary conditions on front-back faces should be periodic, not symmetry or fixed velocity to call for a true 3D simulation. Same for pressure outlet, you need something that allows flow structures to leave the domain without reflections

With this proper setting, as said, you could even expect the constant inlet do develop an instability and become 3D, but you need the right mesh with the right accuracy. Practically, it might not happen and the flow could stay steady and 2D, but we know it is not correct, so people typically provide also the right turbulent inflow for this

[aerosayan]

Originally Posted by eilloo

... was extruded by a few cells in the z direction?

Few cells are not needed. For steady state simulations, one cell in the spanwise z direction is enough to represent a 2D infinite wing.

OpenFOAM represents such thin 3D domains with just one cell in the spanwise z direction too.

If you use few cells, yeah it would be a good enough approximation of an infinite wing, but some streamwise flow between the cells will happen. Though wing-tip leakage won't happen, so yeah it would be a good enough approximation for an infinite wing.

[FMDenaro]

Originally Posted by eilloo

Thanks Filippo,

Supposing we use DNS or LES, how might span-wise vortical structures be introduced to the flow?
The inlet condition is for flow velocities only in x and y, and there are no-slip conditions imposed on the 'front' and 'back' faces as described above.

Would small, numerical errors be enough to induce this, or might there be other mechanisms? Or perhaps this would not be expected at all...

Paolo already addressed the issues. You do not introduce vortical structures in the flow, they generate naturally provided a grid resolution and an accurate scheme is used.

However, you have to be careful in considering the spanwise extension, that determine arbitrarily the property of the structures. Too low extension can prevent the 3D flow as well as determine structures that have a length determined by your arbitrary BCs, thus not physically relevant.

The correct extension along z should be determined by ensuring the 1D correlations reach zero.