[hx293]

Hello everyone,

I just started learning CFD with the channel flow case. I tried different RANS models and LES SGS models on predicting the velocity profile at the channel outlet, and I found most RANS results agreed well with former experiments and DNS results, but LES results did not.

Is there any idea why the LES results deviate the exp. and DNS results so much?

Attached figs contain results and illustrations of the BC settings. The Reynolds number of the problem (defined by channel height and velocity at the channel center) is around 10,000, and the simulated channel length is enough to reach fully developed turbulent flow at channel outlet. The y+ value of the near wall mesh is around 0.2. The delta x+ (streamwise) value of the near wall mesh is around 6, and the delta y+ (pitchwise) value is around 4. The solver I used is Fluent.

Thank you for your attention.

[FMDenaro]

First, one problem is that you are simulating a spatial developing BL and that requires much care in prescribing the LES inlet profile. Then, the velocity profile has a typical effect of a too diffusive impact of the SGS model (or also discretization).
1) please, give details about the inlet velocity and the discretization
2) try to simulate first the periodical channel flow at Re_tau=590 and compare with available DNS

[sbaffini]

You can't really do it that way. A developing BL is quite an order of magnitude more difficult to get right with respect to a channel flow. You can use the latter to find suitable discretization settings while taking the bc out of the picture. Then you can work on a suitable set of bc for your BL setting. Also, the unstructured grid part is certainly not helping. You might find my phd thesis helpful in setting a channel flow with Fluent:

https://www.cfd-online.com/Forums/bl...hesis-les.html

[hx293]

Originally Posted by sbaffini

You can't really do it that way. A developing BL is quite an order of magnitude more difficult to get right with respect to a channel flow. You can use the latter to find suitable discretization settings while taking the bc out of the picture. Then you can work on a suitable set of bc for your BL setting. Also, the unstructured grid part is certainly not helping. You might find my phd thesis helpful in setting a channel flow with Fluent:

https://www.cfd-online.com/Forums/bl...hesis-les.html

Hi Paolo,

Thank you for your comment. I just have few more questions:

1. In this model, why steady RANS method matched the exp./DNS results while unsteady LES did not? Is it caused by steady/unsteady settings, or caused by RANS/LES methods?

2. Why unstructured grid is not recommended compared to structured one? Will increasing the grid density of unstructured mesh be helpful? Or we must use structured mesh in LES?

I am looking forward to your reply.

[hx293]

Originally Posted by FMDenaro

First, one problem is that you are simulating a spatial developing BL and that requires much care in prescribing the LES inlet profile. Then, the velocity profile has a typical effect of a too diffusive impact of the SGS model (or also discretization).
1) please, give details about the inlet velocity and the discretization
2) try to simulate first the periodical channel flow at Re_tau=590 and compare with available DNS

Hi Filippo,

Thank you for your comments.

I am using uniform velocity at the inlet, with the turbulent intensity of 5% induced by the Spectral Synthesizer method. Attached gif illustrates the inlet vorticity fluctuation induced by this method. The near-wall mesh of the case is structured, its sizing has been mentioned before. The mesh at the channel center is unstructured.

I agree with you that the periodical channel flow case is a better idea, and I found it quite popular in some recent JFM papers. However, I am not curious about the transition process, but only interested in the fully developed velocity profile. Is this model accurate enough for this purpose? Maybe with further refinement of the mesh?

I am looking forward to your reply.

[FMDenaro]

The case you want to simulate is not so simple as it would seem...

Starting from a uniform profile, you need to solve the transition that, even if you supplied a superimposed fluctuation, is not physical but numerical.
I see also that many RANS solutions do not match enough the DNS solution.

I have some further question

1) how do you compute the u_tau velocity? (I see you have Re_tau=300, right?). What is the criterion you use for the streamwise lenght?
2) did you use the static or dynamic Smagorinsky model?
3) are you using the central bounded scheme?
4) what about the spanwise lenght of the domain where you set periodic conditions?
5) the first part of the domain has "symmetric" condition. Why?

[hx293]

Originally Posted by FMDenaro

The case you want to simulate is not so simple as it would seem...

Starting from a uniform profile, you need to solve the transition that, even if you supplied a superimposed fluctuation, is not physical but numerical.
I see also that many RANS solutions do not match enough the DNS solution.

I have some further question

1) how do you compute the u_tau velocity? (I see you have Re_tau=300, right?). What is the criterion you use for the streamwise lenght?
2) did you use the static or dynamic Smagorinsky model?
3) are you using the central bounded scheme?
4) what about the spanwise lenght of the domain where you set periodic conditions?
5) the first part of the domain has "symmetric" condition. Why?

Before heading to the details, I would like to highlight my motivation that I am only interested in the velocity profile of the fully-developed turbulent channel flow.

Although turbulent fluctuation exist, the time-averaged velocity profile of the fully-developed channel flow should stay the same through streamwise direction. My hypothesis (might be a stupid one) is that given enough channel length, the non-physical phenomena near the channel inlet (i.e. unappropriated velocity profile as inlet BC, etc.) has no influence on the downstream fully-developed velocity profile. My RANS results actually fits well with the exp./DNS, which shows that the hypothesis is not that bad.

Back to the details:

(1) u_tao = sqrt(tau/density), and tau is calculated by viscosity times velocity gradient; Re_tau ~ 300 is correct. The streamwise length is chose as the minimum length that required to achieve fully-developed flow at outlet, which is determined by trial and error.
(2) I am using static Smagorinsky model.
(3) I am using the central bounded scheme.
(4) The calculation domain size is 100mm*10mm*3mm in streamwise, spanwise(vertical to the channel plane) and pitchwise(vertical to the periodic plane) directions, respectively.
(5) The symmetric BC is setted because I think it is one of the physically-right scenario.

I only had basic CFD courses, but not studied turbulence modeling. Any recommended readings (for beginners) are welcomed.

Thank you for helping.

[FMDenaro]

First, I do not reccomend the static Smagorinsgy model. Try setting the dynamic model.

Then, RANS and LES are very different in the meaning of the variables you solve, the former being statistically steady, the latter being time dependent.
That means that from the LES solutions, you need to apply ensemble averaging to get a meaningful steady profile. The lenght to have a RANS solution well developed is not as same as the lenght required for LES.

I strongly suggest also to check the spanwise energy spectra to see if the LES solution is quite correct.

There are many textbooks that should be read to go in deep in the simulation of turbulence.
I suggest to my students this list:
https://www.researchgate.net/publica..._Part_I_and_II

[FMDenaro]

Just to add that I suggest also to do a run without any SGS model (LES no-model or unresolved DNS) to check the real effect of the model onto the solution.

[sbaffini]

As stated by Filippo, RANS and LES/DNS are two really different matters.

The way you approached the problem in RANS is ok. It can be steady and you don't even need the third spanwise dimension. Also, the grid is of no great concern.

The difference in LES for this case is that you actually want to reproduce all the main mechanisms leading to the transition or, for fully turbulent scenarios, the BL growth.

Basically, this requires accuracy down to a certain flow scale. Fluent by itself, the grid you choose in particular, not to mention the specific scheme and SGS model you are using, are not well suited for this problem. Eventually, for very fine grids, they are going to be ok, but we are probably talking order 10^8 cells for your problem.

While there is probably room for improvement, I have no experience on this (LES of BL in Fluent).

You can try with these modifications:

- no sgs model at all (laminar or static smagorinsky with the constant equal to 0)
- unbounded central scheme (to be activated via TUI if using laminar)
- fully structured grid (should not be difficult in your case)
- second order time advancement with a dt leading to a courant around 0.1

However, I strongly suggest to go back to a simpler case to start LES while also reading some book on it. Otherwise your main risk is wasting a huge amount of time and resources without ever getting any meaningful result.

[flotus1]

Originally Posted by hx293

Before heading to the details, I would like to highlight my motivation that I am only interested in the velocity profile of the fully-developed turbulent channel flow.

Then I would recommend to model a fully developed channel flow instead of a developing channel flow in a long channel and assuming that it is long enough.
This is usually done with periodic boundary conditions between "inlet" and "outlet" and the symmetry boundaries respectively.

[hx293]

Originally Posted by FMDenaro

Just to add that I suggest also to do a run without any SGS model (LES no-model or unresolved DNS) to check the real effect of the model onto the solution.

Now I kind of understand the limitation of my model. I tried your suggestion to run an unresolved DNS case, and the result is very similar to my former LES results. Thus, it must be the numerical model.

I will try to run a simple case to avoid the transition process. Thank you for your help.

[hx293]

Originally Posted by flotus1

Then I would recommend to model a fully developed channel flow instead of a developing channel flow in a long channel and assuming that it is long enough.
This is usually done with periodic boundary conditions between "inlet" and "outlet" and the symmetry boundaries respectively.

Thank you for your comments. Your suggestion sounds clever!

But I am not sure if I could set the inlet flow velocity (in other words, the Reynolds number) as I want. In my RANS model, this can be easily achieved by the inlet condition directly. In your suggested model, how to set this velocity?

[FMDenaro]

Originally Posted by hx293

Now I kind of understand the limitation of my model. I tried your suggestion to run an unresolved DNS case, and the result is very similar to my former LES results. Thus, it must be the numerical model.

I will try to run a simple case to avoid the transition process. Thank you for your help.

This is a typical problem due to the numerical viscosity introduced by the scheme

[flotus1]

Originally Posted by hx293

Thank you for your comments. Your suggestion sounds clever!

But I am not sure if I could set the inlet flow velocity (in other words, the Reynolds number) as I want. In my RANS model, this can be easily achieved by the inlet condition directly. In your suggested model, how to set this velocity?

Well thanks a lot, but this is not really my idea. It is just the commonly accepted method to simulate fully developed channel flows.
Implementations may vary depending on the software you use, but usually a body force is used to drive the flow. You might have to make a few adjustments to the magnitude of the force until you get the desired flow rate.

[FMDenaro]

I agree, setting periodic streamwise and spanwise conditions is a way to study a temporal evolving boundary layer, no velocity inlet/outlet must be prescribed but only cyclic conditions. The driving force is the constant pressure gradient or the mass-prescribed constraint.

The thesis of Paolo describes the setting, if you want to se a comparison with other LES codes, you can have a look here:
https://www.researchgate.net/publica...mulation_codes