[jrrelx]

Dear all,

First post so maybe stupid question, but I have encountered some problems when modeling a fully developed pipe flow with periodic boundary conditions using LES in Fluent 6.3. I aim to get a realistic transient inlet BC for my problem (particle deposition in a bend).

I'm considering a circular pipe (5*D long) with periodic BCs (mass flow rate), using a hexa-mesh with Y+ at wall around 0.5, growth ratio around 1,1. Re = 10000, Courant number < 1, setting residuals under 10^-5, using central differencing for velocity dicr. and PISO scheme for Pres-vel coupling.

It seems that the case is converged but when I take a look to the vel. profiles they are unphysical because they are parabolic and this case of profiles are characteristic for laminar flow. Additionaly, the pressure gradient shown in the PC window is far away from the theoretical value.

Probably I went wrong somewhere. I don't know that it has something to do but when I plot cell Reynolds number of my case, it's highly lower than the 10000 I wanted to model.

Thanks in advance.

Javier

[sbaffini]

Dear Javier,

if i understood well, you are simulating the pipe flow at Re_tau = 320 (DNS of Wagner and Huttl, C&F).

The first issue, in your case, is probably the velocity field initialization. I suggest you to first get a steady k-eps solution, use the Fluent internal initializator via TUI (solve/init/init-instantaneous...) and then switch to unsteady LES without re-initializing your case.

Secondly, you have to be aware that in wall-bounded LES all the grid spacings are important, not only the wall-normal at wall. Hence, you need to check them too.

Finally, when using the unbounded central scheme, there are some issues concerning the discretization for the pressure. For the unbounded scheme in the plane channel i found the PRESTO! to be be the only reliable choice.

Hope this helps

[jrrelx]

Dear Paolo,
Thanks for your reply.

I've taken the average velocity as a initialization value. However, I'll start from a converged k-epsilon as you suggest.
I think the gris is not the problem because I'm using a 2 milion cell hexa grid.
I'll try PRESTO! scheme.

Regards.

PS: I lowered the time step one order of magnitude and the profiles looked like more to a turbulent profile but the pressure gradient is still far from the theretical (300 Pa/m vs 655 Pa/m).
i'm sorry but I don't know exactely what you meant whith the Re_tau = 320. My flow Re num is equal to 10^5.

[sbaffini]

In my experience, the grid size requirements for a wall bounded LES are (for a low order code like Fluent):

streamwise: dx+ <=30-60
wall-normal: dy+_min <1 - dy+_max < = 30 (probably it can be relaxed if far away from the wall)
span-wise: dz+ <= 15

As long as your grid respects these values without too strong grid stretchings, then the grid is ok. The absolute value of the number of cells is not of any relevance as they can be concentrated in a wrong place (especially in the pipe).

I don't think the time step is of any relevance as long as your Courant number is below 1. Still, i suggest to have values around 0.1.

If your flow has Re = rho * Ub * D / mu = 10^4 (as you previously wrote), then the equivalent friction reynolds number is Re_tau = rho * u_tau * D / mu = 640 circa (=320 if based on the radius).

Here Ub is the bulk flow velocity while u_tau is the friction velocity. A simple formula for the pipe is:

Re_tau = 0.199 * Re^0.875 (both Re based on diameter)

It is important to know about the friction Reynolds number because the previously cited grid spacings are computed as:

delta+ = delta/D * Re_tau (based on diameter)

Hence, imagine having Nx=64 cells along the pipe axis, the corresponding dx+ in your case is:

dx+ = L/(Nx*D) * Re_tau = 5/64 * 640 = 50

[jrrelx]

Dear Paolo,
After cheking the grid requirements and having assessed that they respect the values provided by you, I've obtained a realistic velocity contours by following your instructions.
Many thanks for that.
However I have a last question about the convergence criterion. I've read somewhere that the convergence criterion should be when the simulation has run at least 2 or 3 cicles defining the cicle as the ratio between the time taken by a fluid particle to travel across the pipe to the time step. Imagine my time step being equal to 1e-5 and the ratio L (pipe lenght)/U (mean vel)=0.0025 s. According to the above mentioned criterion I should run 250 number of time steps. Nevertheless I've run more than 3000 and the pressure gradient is different than the theory. Thus for converging a time step I must run more than 50 iterations.

Is a good criterion for convergence the one I told to you?
Should I reduce my t step?

Thanks in advance.
Regards.

[sbaffini]

Dear Javier, if you are using periodic boundary conditions the main criterion to check about the convergence toward a statistically steady state is to monitor the volume average of the resolved kinetic energy (0.5 * rho * V_magnitude^2). At some time it will start to flap around some mean value.

This is especially true for a fixed pressure gradient periodic condition. For fixed mass flow, as you can understand, the fact that the mass flow is fixed will strongly affect the time history of the volume averaged kinetic energy, but you should still see a flapping.

Another criterion usually used is based on monitoring the terms present in the time averaged axial momentum equation (turbulent + viscous stresses) and check that their sum respect the expected linear behaviour.

Finally, the time step is just limited by the courant number. If you are below 1 everything should be fine (in my experience). Usually, i use the following criterion:

dt * u_tau^2 / nu = 0.1

which is based on the viscous scales but usually ensures the satisfaction of the courant criterion as well.

[jrrelx]

Dear Paolo.
I want to thank you for the given help.
I was finally able to converge both cases, the straight and the curved pipe with reasonable results for the LES simulations.

Now I'm performing a LES simulation in a rectangular duct. When defining the number of cells I reached a dead end because I don't know how to calculate the friction Re number (Re_tau). My question is if I can use the above mentioned expresion for the pipe (Re_tau = 0.199 * Re^0.875 based on the diameter) with the hydraulic diameter of the duct.

I.e. imagine the duct having 1.5H and H (height and width), U=5 m/s and air kinematic viscosity 1.4e-5m2/s. Therefore for H=0.0125 (D_h=1.2H) Re=5136.
Is then the Re_tau=351?
Any help would be apreciatted.
Thanks in advance.
Regards.

[sbaffini]

Dear Javier,

the main fact to know about the square/ractangular channel is that the wall stress distribution along the section perimeter is, of course, not constant. Especially in the middle of the channel there usually is a value higher than the average one (which defines your pressure drop). Hence, even with a perfect correlation, a precise local match of the friction Reynolds number can't be expected.

The second fact is that going from the square duct to the plane channel flow there are a range of intermediate cases (rectangular ducts which are very different from the pipe and from the channel).

In the works i did on the rectangular ducts i never needed such a correlation as i always started from a given pressure drop hence i actually fixed the Re_tau (based on hydraulic diameter).

As a matter of fact, i don't know the answer but i think that you can compare the value you obtained with your correlation with that based on the channel half-height and the Dean correlation (plane channels). This would give you a sensitivity on the Re_tau from which you could decide if the value you already obtained is reliable or not.

I expect them to be very similar hence, considering the purpose of such a computation (obtaining the proper grid spacings), you could probably proceed with it without harms (with the understanding that you always have to check it a posteriori).

I have some cases i already did from which i could try extracting such information (i never needed it) but today i can't as i am out of office. I will give you this information as soon i can.

Regards

[rasoulb]

Hi,
Dear Paolo
I want to simulate fully developed channel flow by using fluent-LES at Re_t=180. first I ran steady state flow simulation using k-e model. when the flow field is converged, I used the solve/initialize/ init-instantaneous-vel text command to generate the instantaneous velocity field. then I ran LES-WAlE model.
the C_f (=8.0931 E-3) & pressure gradient obtained by k-e is good but when I ran LES the C_f (=5.50 E-3) and pressure gradient decrease constantly.the domain dimension is 2 meshed by 76*64*64 grid. the B.C is periodic in streamwise and spanwise direction.
x=14
y=0.4-14
z=8.8
Please guide me why C is decreasing? I also have this problem by constant pressure gradient.

thanks

[sbaffini]

Dear Rasoul,

as a first guess i suggest you to proceed with the fixed pressure gradient periodic boundary condition, just to check that everything is fine (than, possibly, use a fixed mass flow rate if you need it). Here you can find several details on setting up LES in Fluent:

http://www.lamc.ing.unibo.it/aimeta2.../MEM-273-0.pdf

If you have:

delta (half-channel height) = 1
rho (density) = 1
mu (dynamic viscosity)= 1/Re_tau = 1/180

than the pressure gradient in the streamwise direction to sustain this flow is simply -1 (and also the friction velocity is simply 1).

Having said so, your grid looks fine (almost a DNS actually). However you should also have a courant below one to achieve the necessary temporal resolution/accuracy. Under the previous settings, i usually use dt=0.1/Re_tau.

If this is all fine, than i suggest using the following numerical setting:

2nd order time integration
nita - fractional step with basic settings
(bounded) central scheme for convective terms
PRESTO! for pressure
Least squares for gradients

If this is also fine than you need to consider that of course the Cf will change from the RANS value. At some point, after the proper temporal variation, it will start oscillating around a mean value which you can consider the definitive one. In no way this is necessarily better than the RANS one. You can see my results above for a higher Reynolds number.


Best regards

[rasoulb]

Dear paolo
thanks for your suggestion, I did what you said. my Cf now oscillates around a mean value 0.00855 which have 5.5% error with DNS results [Abe 2001]. Is it good?
I will compare Rms of velocity fluctuations by DNS Data.

[sbaffini]

Dear rasoulb,

notice that in the work of Abe et al., the flow is driven by a fixed pressure gradient. As a consequence, while it is perfectly fine to compare the skin friction coefficient, its discrepancy is only due to the mean velocity. In the past, i compared my LES results with those of Kim, Moser and Mansour and the discrepancy for a grid even corser than your was lower (64x65x64 cells in a 4pi x 2 x 4/3 pi domain) for the Re_tau=180 case. However, for higher Reynolds number (Re_tau=590), i got an error larger than your.

It's difficult to give a definitive answer, i would suggest the comparison of nondimensionalized mean and rms velocity profiles with DNS ones.

[Goutam]

A simple formula for the pipe is:

Re_tau = 0.199 * Re^0.875 (Re based on diameter)

Is this relationship correct? Using this, For Re = 10000, Re_tau = 629 (based on diameter).

[Goutam]

Is there anyone who like to share the LES straight circular pipe Fluent "*.cas" file? I am a new user of fluent and trying to simulate the LES side. Also I am using Fluent 6 version for my work. Thanks

[chan1629]

Dear jrrelx,
Now I have the same problem as you. I want to get the velocity profile of fully developed pipe flow (Diameter:104, mean velocity:8.7 m/s, the mass flow: 0.09048). I used the ke model to simulate this model, and I got the maximum velocity on the cross section was only 10.2 m/s, and the experiment was about >10.74. I wonder where i had done wrong.
Thanks.

[RodriguezFatz]

Originally Posted by sbaffini

Finally, when using the unbounded central scheme, there are some issues concerning the discretization for the pressure. For the unbounded scheme in the plane channel i found the PRESTO! to be be the only reliable choice.

Paolo, do you have any recommendation for the pressure interpolation in OpenFOAM for such a case? I can't see "PRESTO" here, but many other possible choices.

[sbaffini]

Dear Philipp,

the PRESTO issue for Fluent is a longstanding one as, roughly speaking, no one knows what it exactly does. I cannot give you a straight answer but, if you want, you can read part of my thesis:

https://www.politesi.polimi.it/bitst...Lampitella.pdf

More specifically, section 5.4 analyzes the role of the pressure gradient in the freactional step method and some non conventional options available in literature are described. Section 6.3.1 then analyzes the outcome for the different options available in Fluent for the LES of the channel flow.

The main idea (according to what i figured out the PRESTO does) is to use a pressure gradient discretization that minimizes the difference with respect to the pressure gradient available on the faces as a result of the pressure poisson equation discretized compactly. This, in turn, minimizes the spurious kinetic energy and/or mass production related to the cell-centered/compact-laplacian approach.

[sbaffini]

Notice that, currently, Fluent guidelines discourage the use of the PRESTO for LES, which is described as overly diffusive. Actually, my results indicate that are the other schemes being only apparently antidiffusive, their main problem being a spurious mass production.

[RodriguezFatz]

Paolo, thank you for the fast reply.
I will read the parts of Your thesis, but I have consecutive questions:
1) When I face checkerboarding of p and U in a pipe or channel LES, would you rather recommend to keep the velocity interpolation "central differences" and change the pressure gradient calculation? Or the other way around?
2) If the first is the case, would you better just switch on some gradient limiter for "p" or change the face interpolation of "p" to some other than linear?

[sbaffini]

Following my previous discussion i would change the pressure interpolation. However, my answer can only be incomplete without knowing additional details on your simulation, like the time advancement, courant number, pressure-velocity coupling, grid steps etc.

Also, a simple limiter might only give you a more pleasant solution (but i have no experience on using pressure limiters) while worstening the overall quality.