[roi247]

Hello everybody!

I'm running LES to simulate a turbulent flow in a rectangular channel. Basically, there is a under estimation (prediction) of velocity magnitude close to the wall compared with some experimental data using Preston tube. Even after a relatively long distance, the velocity is still not stable(The velocity contour keeps changing after a long distance).


MESH
Mesh were just made to guarantee yplus<=1 at the first cell. But I can only make it at the 3/4 distance from the inlet. At the inlet, the yplus is pretty large because the shear velocity and wall stress are large.

FLUENT SETUP
Transient unsteady-2nd-order-bounded
large-eddy-simulation les-subgrid-smagorinsky
materials/fluid water-liquid
Boundary conditions
top surface specified shear stress 0 0 0
velocity-inlet inlet 0.495
Bottom Wall and side walls no-slip boundary condition
Solution methods scheme(simple) pressure(second order) Momentum (Bounded central difference) transient formulation(bounded second order implicit)
Pressure outlet
solve/monitors/residual/convergence-criteria 1e-06 1e-06 1e-06 1e-06
solve/set/time-step 0.003
solve/dual-time-iterate 1500 120

RESULTS
I have the data from an experiment. The comparison of the wall shear is always under estimation. The best one is with error around 7% at the wall shear of 3/4 distance from the inlet. And it keeps decreasing along the channel shown in the figure below.
This is the along channel velocity contour

In the other plot of velocity change along the channel bottom, it indicates the velocity close the wall keeps decreasing.

Question:
1. Why I cannot choose roughness in the LES? So it doesn't matter what the material of the wall is?


(20160309) My case is end up steady(doesn't change with time step), and I'm increasing the length of the channel. Hope the velocity profile would be end up horizontal(fully-developed)

(20160310) The velocity and wall shear near the wall keeps decreasing. I mean the mean velocity at the cross section is stable, but the velocity close to the wall is decreasing. It becomes more serious when I decrease the cell length and increase the channel length. So maybe pressure outlet is not good for this case.


Rui

[pksri]

Hi, I am also working in similar problem but i have a question about calculating of shear stress at wall. Hope you could help me.

I am working on transition region at present I have flow through the rectangular channel and I have saved my cas & dat file for every 100 time steps. Now I am trying to post process my result in Tecplot to get a wall shear stress along the flat plate to locate the transition region. I am not sucessful in this, and could you help me please?

Regards,
Kumar

[roi247]

Hi Pksri,

I'm not familiar with Tecplot. I'll say something about how I did it in CFD-post ( Ansys workbench.)

I drew a line on the channel bottom and draw x-y plot. The line must be exactly on the wall to show the wall stress in the plot.


Regards
Rui

[pksri]

Hi Rui,

Thanks for the reply. But the plot generated wouldn't be limited to that specific time frame instead of the whole time steps?

[roi247]

I can choose time step selector by clicking on the clock figure on the software.

The figure show above is a steady case, otherwise it should be a lot of timesteps.

[pksri]

Yes yes I understand that.. my question is that is there any way that you could find a time average shear flow over a plate. Because at each time step the value would be different.

[LuckyTran]

Originally Posted by pksri

Yes yes I understand that.. my question is that is there any way that you could find a time average shear flow over a plate. Because at each time step the value would be different.

you need to enable data sampling for time statistics. This will create new variables for the time-averaged quantities and you will be able to get time-averaged wall shear from that.

[pksri]

Could you please explain more about it..I am struggling to do one..

[roi247]

oh I understand now. sorry what I'm doing it using excel to average it . Because I only have 15 files(groups of data to average). Actually, I don't need to do that, because I just wanted the value of the fully-developed flow.

[pksri]

Ah that's great.. I have more transient steps :/ Also a small question I ran LE simulation with SGS model , piso solver and spectral synthesiser ( turbulent intensity 3% ) when I opened the wall shear stress it just shows as a laminar flow in a flat plate. I don't have any transition region :/ do you might have any idea about it.

[roi247]

E sorry I don't know how to solve it. Maybe you can try to search "data sampling" and "time statistics" Or ask again in the forum .

http://jullio.pe.kr/fluent6.1/help/html/ug/node471.htm
http://jullio.pe.kr/fluent6.1/help/html/ug/node865.htm

[LuckyTran]

Originally Posted by pksri

Could you please explain more about it..I am struggling to do one..

All you do is click a check box. It's right next to the calculate button in the GUI. Or you can look up the TUI command if you don't have a GUI.

Originally Posted by pksri

Ah that's great.. I have more transient steps :/ Also a small question I ran LE simulation with SGS model , piso solver and spectral synthesiser ( turbulent intensity 3% ) when I opened the wall shear stress it just shows as a laminar flow in a flat plate. I don't have any transition region :/ do you might have any idea about it.

Did you add perturbations to your flow? Go to solve initialize and init instantaneous velocity. Or you can add perturbations manually.

If you don't have enough perturbations your LES will stay laminar or it can even relaminarize. Turbulence is initiated by perturbations that grow, and if you do not provide any initial perturbations the flow can stay laminar.

[pksri]

Hi Lucky Tran,
Thank you for the reply!

I didn't add any perturbations as I used spectral synthesiser with turbulence intensity, I thought that would be sufficient. So this is the reason why I don't see any transition in my result file.

So if I am using perturbations I hope I can see the transition region properly. Thank you so much!

[roi247]

Originally Posted by LuckyTran

All you do is click a check box. It's right next to the calculate button in the GUI. Or you can look up the TUI command if you don't have a GUI.



Did you add perturbations to your flow? Go to solve initialize and init instantaneous velocity. Or you can add perturbations manually.

If you don't have enough perturbations your LES will stay laminar or it can even relaminarize. Turbulence is initiated by perturbations that grow, and if you do not provide any initial perturbations the flow can stay laminar.

Hi Lucky Tran,

Since you're here, May I ask why there is no roughness option in the LES.
In a one phase 3D simulation, if we don't specify what the material is. How can fluent know which material of the walls is. For example, flow through a concrete channel shouldn't have same wall shear as a plastic channel.

[pksri]

Originally Posted by LuckyTran

All you do is click a check box. It's right next to the calculate button in the GUI. Or you can look up the TUI command if you don't have a GUI.



Did you add perturbations to your flow? Go to solve initialize and init instantaneous velocity. Or you can add perturbations manually.

If you don't have enough perturbations your LES will stay laminar or it can even relaminarize. Turbulence is initiated by perturbations that grow, and if you do not provide any initial perturbations the flow can stay laminar.

Dear lucky Tran,

Now i made the case init initialize command in the TUI and changed the model to LES and used vortex method and running a simulation. Still I dont see any transition. Till now the calculation is performed for 0.25s.

please see the attached picture and give me a comment what is wrong.

Note: I didnt initialize like initialize from inlet. I just did init-initialize instantaneous-vel in GUI and started the model.

[LuckyTran]

Originally Posted by roi247

Hi Lucky Tran,

Since you're here, May I ask why there is no roughness option in the LES.
In a one phase 3D simulation, if we don't specify what the material is. How can fluent know which material of the walls is. For example, flow through a concrete channel shouldn't have same wall shear as a plastic channel.

The only difference between a concrete channel and plastic channel is the wall roughness. You never need to specify what the wall material. The fluid does not care what the material of the wall is beyond the boundary condition (which is the no-slip condition and kinematic blocking condition). The wall material option is for modelling the thermal resistance at the wall. The wall material is relevant only when surface tension is important (which is no longer a Navier-Stokes problem) or if you are doing molecular dynamics simulation (no longer a fluid flow problem).

A rough wall model is currently not supported for LES in Fluent. The problem with rough walls in LES or DNS is that you need a time-accurate rough wall model, which is very hard. If it was easy to come up with a rough wall model that was time-accurate, the problem of turbulent wall bounded flows would be a joke.

There are however, reasonably accurate rough wall models for for the mean flow (the modified law of the wall for roughness). But these are valid only on the mean flow and hence you need to be doing some type of RANS to use the rough wall model. If you want to do LES with wall roughness using these types of time-averaged wall models, then you are effectively doing a DES or hybrid LES-RANS and it is actually much better to use one of those DES or Hybrid LES/RANS than to use plain LES.

Originally Posted by pksri

Dear lucky Tran,

Now i made the case init initialize command in the TUI and changed the model to LES and used vortex method and running a simulation. Still I dont see any transition. Till now the calculation is performed for 0.25s.

please see the attached picture and give me a comment what is wrong.

Note: I didnt initialize like initialize from inlet. I just did init-initialize instantaneous-vel in GUI and started the model.

Check your velocity contours to make sure the velocity is reasonable now and after you did the init-instantaneous. Did you add the perturbations after solving it using a RANS model to have a more accurate turbulence?

Is your time-step and courant number small enough so that you don't clip your simulation temporally? LES needs to be time-accurate.

[pksri]

Originally Posted by LuckyTran

Check your velocity contours to make sure the velocity is reasonable now and after you did the init-instantaneous. Did you add the perturbations after solving it using a RANS model to have a more accurate turbulence?

Is your time-step and courant number small enough so that you don't clip your simulation temporally? LES needs to be time-accurate.

Dear Lucky Tran,

I dont see any changes in velocity contour. I have attached 3 velocity contour images ( 2 shows before and after Initialize , 3rd one is at 200 timestep. dt is 1e-4 ). I dont under stand adding perturbation. How to add perturbations? I used the vortex method for turbulence characterstics. Isnt it suffiecient?

my courant number is 0.2. velocity is 10m-s and dx is 5mm ( considering the largest mesh size )

Also do I have any problem with the dimension of my domain. I use .94*.2*.2m with 1.34° incilnation for the bottom wall.

looking forward for your reply.

Kind Regards,
kumar

[roi247]

Originally Posted by LuckyTran

The only difference between a concrete channel and plastic channel is the wall roughness. You never need to specify what the wall material. The fluid does not care what the material of the wall is beyond the boundary condition (which is the no-slip condition and kinematic blocking condition). The wall material option is for modelling the thermal resistance at the wall. The wall material is relevant only when surface tension is important (which is no longer a Navier-Stokes problem) or if you are doing molecular dynamics simulation (no longer a fluid flow problem).

A rough wall model is currently not supported for LES in Fluent. The problem with rough walls in LES or DNS is that you need a time-accurate rough wall model, which is very hard. If it was easy to come up with a rough wall model that was time-accurate, the problem of turbulent wall bounded flows would be a joke.

There are however, reasonably accurate rough wall models for for the mean flow (the modified law of the wall for roughness). But these are valid only on the mean flow and hence you need to be doing some type of RANS to use the rough wall model. If you want to do LES with wall roughness using these types of time-averaged wall models, then you are effectively doing a DES or hybrid LES-RANS and it is actually much better to use one of those DES or Hybrid LES/RANS than to use plain LES.

Hi Lucky Tran,

Thank you for your help, the roughness has confused me for a long time.

I'm simulating a flow in a perspex flume which has a roughness coefficient of 0.009-0.010. Since I don't have enough perturbations. (I have no roughness) Is this the reason I can never make the flow has the same mean shear stress at the location of fully-developed flow as the experiment? The experiment gives a value of 0.64 [pa] at a location 11.97m to the inlet. They believe it is fully-developed at that location. You can tell in the figure below, at -0.33 m, I get the value exactly the same with the experiment. However it is not able to maintain that value. I mean it keeps decreasing even after a 6H(6 depth) distance. And the value will be far from the experimental value.
The velocity profile of the boundary layer becomes somehow like a laminar flow at a relatively long distance



Since what I'm doing is turbulent flow which changes with time and space, I shouldn't use DES and hybrid LES/RANS? So what should I do? Are there some portable settings can generate some perturbations which has the same effect as the roughness.

[LuckyTran]

DES and hybrid RANS/LES still behave mostly likely LES. You're only applying RANS in the viscous regions (where turbulence plays a less important role).

I think your roughnesses are small. But you can compare it to the here:
https://en.wikipedia.org/wiki/Law_of_the_wall

If your roughness is smaller than the viscous sublayer then it interacts with the flow mainly by increasing the wall shear stress and does not cause any perturbations.

The lack of any roughness would suggest that your simulation should underpredict the wall shear stress.

I just realized you have a top surface with no wall shear. How do you have a rectangular channel? You should have an inlet outlet and four walls if you are doing rectangular channel LES. Is this an open channel?

In order for this to become fully developed, the boundary layer would have to grow all the way to the other wall. Your simulation shows this is far from the case.

Did you specify any turbulence at your inlet? If not, then you have a laminar inflow and this is a laminar boundary layer growth which is better done using a a steady laminar flow solver than LES.

[roi247]

Originally Posted by LuckyTran

DES and hybrid RANS/LES still behave mostly likely LES. You're only applying RANS in the viscous regions (where turbulence plays a less important role).

I think your roughnesses are small. But you can compare it to the here:
https://en.wikipedia.org/wiki/Law_of_the_wall

If your roughness is smaller than the viscous sublayer then it interacts with the flow mainly by increasing the wall shear stress and does not cause any perturbations.

The lack of any roughness would suggest that your simulation should underpredict the wall shear stress.

I just realized you have a top surface with no wall shear. How do you have a rectangular channel? You should have an inlet outlet and four walls if you are doing rectangular channel LES. Is this an open channel?

In order for this to become fully developed, the boundary layer would have to grow all the way to the other wall. Your simulation shows this is far from the case.

Did you specify any turbulence at your inlet? If not, then you have a laminar inflow and this is a laminar boundary layer growth which is better done using a a steady laminar flow solver than LES.

Hello LuckyTran
My aim is to get the wall shear on the wall for a turbulent flow.

It's a one phase rectangular channel case. The top wall is zero shear stress. The data here are cited from a paper
The other three walls are no-slip wall. inlet 0.495m/s (Maybe using udf, 1/7 law), pressure outlet. 0.381m wide,0.0975m deep and 6H length. You mean I should have air??

http://www.cfd-online.com/Tools/yplus.php Using the estimator here. y=3.76e-5 which is smaller than roughness 0.009


I did't specify any turbulence on the wall. Ah Maybe That's the reason why I got the laminar velocity profile at the end of the channel. Where to specify that?




Which algorithm do you suggest me to use? How to set the parameters there ? leave as default?

Thank you so much!