[holgerbre]

Hi,


I simulate a flow through a squared duct, Re=2E9 (I set the kinematic viscosity to 1.46E-10 in order to have a fast transition to a turbulent flow), periodic bc in streamwise direction. Some pertubation is added initially to the flow field. The duct width is resolved by 240 grid points. The convective terms are approximated by a 5-th order scheme. No turbulence model is used, thus, I perform kind of a implicit LES. After simulation of 0.05 s I see only very small fluctuations, about 1000 times smaller than what I would expect to see in fully developed turbulence.


My question is: after which time span can I expect to see turbulent fluctuations? Do I need too simulate longer, or is it already clear that there is a problem with my simulation?


Best,
Holger

[FMDenaro]

Originally Posted by holgerbre

Hi,


I simulate a flow through a squared duct, Re=2E9 (I set the kinematic viscosity to 1.46E-10 in order to have a fast transition to a turbulent flow), periodic bc in streamwise direction. Some pertubation is added initially to the flow field. The duct width is resolved by 240 grid points. The convective terms are approximated by a 5-th order scheme. No turbulence model is used, thus, I perform kind of a implicit LES. After simulation of 0.05 s I see only very small fluctuations, about 1000 times smaller than what I would expect to see in fully developed turbulence.


My question is: after which time span can I expect to see turbulent fluctuations? Do I need too simulate longer, or is it already clear that there is a problem with my simulation?


Best,
Holger

If I understand, you are simulating a full confined rectangular duct having only inflow/outflow periodic, right? Are you starting from the laminar solution with a perturbation? Consider also that the lateral walls requires to use a very fine grid, therefore compute the y+ of you first celle close to the walls. Then, you must use the non-dimensional numbers based on wall velocity, then the time must be non dimensional using the corresponding reference time.

Compute the total kinetic energy versus the time, you should find an energy equilibrium (indicating a fully developped flow) after some dozens of non dimensional time units. At this time you can collect the samples for the statistics.

[holgerbre]

yes, I have a full confined rectangular duct having only inflow/outflow periodic bc and I start from the laminar solution with a perturbation.
The grid is refined at the walls. However, due to nu=1.46E-10 m**2/s the first point is at y+=1000, and the simulation time of 0.05 s is 8E6 non-dimensional time units.



I anticipate your answer might be that with y+=1000 I do not resolve the relevant processes to initiate turbulence, so I will start a simulation with a more realistic value for nu.

[FMDenaro]

Originally Posted by holgerbre

yes, I have a full confined rectangular duct having only inflow/outflow periodic bc and I start from the laminar solution with a perturbation.
The grid is refined at the walls. However, due to nu=1.46E-10 m**2/s the first point is at y+=1000, and the simulation time of 0.05 s is 8E6 non-dimensional time units.



I anticipate your answer might be that with y+=1000 I do not resolve the relevant processes to initiate turbulence, so I will start a simulation with a more realistic value for nu.

yes, start first a case at low Re number in such a way that you have at least 3-4 nodes at y+<=1.

[LuckyTran]

The high frequency parts develop quite fast, around 6-8 eddy turnover times which you can estimate using nu*L/U^3. After this time you should see appreciable velocity fluctuations. The large eddies of course take longer and go like the flow-thru time and it will take many many flow-thru times to establish the proper statistics for the fully developed state.

How long is 0.05 s relative to the streamwise length? Maybe you just need to run it a lot longer.


y+ of 1000 is nearing the edge of the boundary layer (if this was like freestream flow over a plate). But you have flow in a channel, the y+ shouldn't be that high except the cells in the centerline. Something does not sound right if your first cell is at a y+ of 1000... But supposing it is true, you probably have an x+ and z+ of 1000 or more which is far too coarse to resolve anything.

[holgerbre]

I started a new simulation setting nu to 1.46E-5. For this condition there are 8 grid points at y+<1. I run for 1s which corresponds to 13 flow through times or 580 non-dimensional time units based on wall quantities. However, I develop very very little fluctuations, of the order of 1E-9 m/s while the bulk flow velocity is 1.5 m/s. Btw, Re based on the duct width and the bulk velocity is 4100.
I assume now I should actually see a fully developed flow, or?

[FMDenaro]

Originally Posted by holgerbre

I started a new simulation setting nu to 1.46E-5. For this condition there are 8 grid points at y+<1. I run for 1s which corresponds to 13 flow through times or 580 non-dimensional time units based on wall quantities. However, I develop very very little fluctuations, of the order of 1E-9 m/s while the bulk flow velocity is 1.5 m/s. Btw, Re based on the duct width and the bulk velocity is 4100.
I assume now I should actually see a fully developed flow, or?

Could you plot the total kinetic energy versus the non-dimensional time? Then, what about the profile u+(y+), it is still like a laminar profile?

[FMDenaro]

Just to add that a fully confined duct can produce suppression of oscillations, you could need to run for longer time than the two-periodical channel. That could depends on the ratio W/H.
Paolo (@sbaffini) could tell us more, he did some simulations for this case

[LuckyTran]

Originally Posted by holgerbre

I run for 1s which corresponds to 13 flow through times or 580 non-dimensional time units based on wall quantities.

So your streamwise length is 58 wall units? That barely fits even 1 large streamwise eddy. Or do I make some mistake?

What's the length to height ratio? It needs to be some big integer like 5,10, 15, etc.

Originally Posted by FMDenaro

That could depends on the ratio W/H.
Paolo (@sbaffini) could tell us more, he did some simulations for this case

The square duct is quite similar to the circular pipe.

[FMDenaro]

Originally Posted by LuckyTran

The square duct is quite similar to the circular pipe.

well, could somehow similar if W/H = O(1) but I have no idea of the geometry of the asked problem ...



From what was written above, I estimated a Re_tau of about 200 but what about the domain extension?

[holgerbre]

Attached I plot the u(y) velocity profiles for 2 time instances and the average and max streamwise velocity over time. It is all in SI units because, to be honest, I have some trouble to establish the non-dimensional parameters:


The domain size is 2*delta x 2*delta x 8*delta and delta is 0.02, nu=1.46E-5, rho=1.2 (again, all written in SI units). So Re based on the max u velocity and delta is about 3500 which should lead to a turbulent flow.

I apply a pressure gradient of dp/dx=-0.36.
tau_w=-dp/dx*0.5*delta (for pipes) = 0.0036
u_tau=sqrt(tau_w/rho)= 0.055

Re_tau=u_tau*delta/nu=75 (I would expect 150 based on Re ???)


now, I calculate it based on the velocity gradient obtained from the average streamwise velocity at the first grid point:
du/dy=4444
tau_w=rho*nu*du/dy=0.078
u_tau=sqrt(tau_w/rho)=0.25
Re_tau=350 ???


Obviously I make some mistake. Your opinion is very appreciated.

[FMDenaro]

Have you averaged the velocity profile along the streamwise direction? It appears smoothed so I suppose that is a statistical profile obtianed by the pointwise LES profiles, right?


However, I strongly suggest to work solving directly the non-dimensional equation. If you use u_tau = [Delta p*H /(rho0*Lx)]^0.5 the nondimensional equations solves directly in terms of u+ vector field and you have a forcing term in the momentum equation along x to be prescribed simply as -1 and you can set directly the value of 1/Re_tau in the diffusion parameter.
More details can be found in Sec.5 here
https://www.researchgate.net/publica...ection_methods

[holgerbre]

yes, I averaged in streamwise direction. But the profile is anyhow the same at each cross-section.
If I use the equation you posted (u_tau = [Delta p*H /(rho0*Lx)]^0.5) I receive Re_tau=150 as expected. But for a channel flow it should be u_tau = [Delta p*H/2 /(rho0*Lx)]^0.5, or?

[FMDenaro]

Originally Posted by holgerbre

yes, I averaged in streamwise direction. But the profile is anyhow the same at each cross-section.
If I use the equation you posted (u_tau = [Delta p*H /(rho0*Lx)]^0.5) I receive Re_tau=150 as expected. But for a channel flow it should be u_tau = [Delta p*H/2 /(rho0*Lx)]^0.5, or?

I used the full height of the channel in my paper

[holgerbre]

I understand, that's why in the equation for u_tau there should be H/2, or? at least according to Pope: -dp/dx = tau_w/delta where delta = H/2 and u_tau=sqrt(tau_w/rho)

[FMDenaro]

Originally Posted by holgerbre

I understand, that's why in the equation for u_tau there should be H/2, or? at least according to Pope: -dp/dx = tau_w/delta where delta = H/2 and u_tau=sqrt(tau_w/rho)

no matter about H or H/2, you just need to be congruent in the equations and you will see a factor 2 or 1 in the forcing term