CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Problem with Turbulence Kinetic Energy (http://www.cfd-online.com/Forums/fluent/122013-problem-turbulence-kinetic-energy.html)

 Davide_sd August 10, 2013 05:12

Problem with Turbulence Kinetic Energy

2 Attachment(s)
Hi all,

i've setup a very simple simulation: a flat terrain, with a given inlet velocity and turbulence kinetic energy profile (find it on a paper). To create these profiles, i've setup a UDF.

I was expecting the velocity profile to mantein along the domain length, as it was written in the paper. Instead i've found these velocity profiles (picture in the attachment: line-0 = inlet; line-1650 = outlet, ie 1.65m; line-825 = mid section, ie 0.825m).

If i remove the turbulence kinetic energy profile, and set it to value 1 m^2/s^2, the velocity profiles are way better...

Question is: why the turbulence kinetic energy profile is giving me those strange results?

 flotus1 August 10, 2013 06:33

Which turbulence model did you use in your simulation?
Which kind of wall function?

 Davide_sd August 10, 2013 06:44

k-epsilon with enhanced wall treatment, because y+ < 1 (in this case it starts at 0.9 at inlet, and drop to 0.4 at outlet).

 flotus1 August 10, 2013 12:02

A quick estimate of the Reynolds number yields ~1600 (assuming the kinematic viscosity of air).
Are you sure that this is correct?

If so, the standard k-epsilon model is not the best choice because of the relatively low Reynolds number.
Did you try other turbulence models?

 Davide_sd August 10, 2013 13:19

all the data used in the simulation are taken from the paper, and i'm pretty sure to have them extracted correctly.

i know k-epsilon is not the best choice for low Reynolds number. Still i'm using it because it gives me the best result.

The paper i'm following is: "Near wall characterization of the flow over a two-dimensional steep smooth hill" by J. B. R. Loureiro, F. T. Pinho, A. P. Silva Freire.
It discuss about the experimental data of a flow over a hill.

I have setup the hill simulation, with the same inlet profiles (extracted from the paper). The results of the hill simulation were not satisfactory, as you can see from the following pictures (i can't use the attachment because the quality of the pic would be too low...):
Velocity Profiles; Turbulent Kinetic Energy Profiles; Domain of the simulation; y+ plot
Where: H=60mm (height of the hill); u_delta=0.0482 m/s (external velocity/free stream velocity).

As you can see from the velocity profiles image, even at x/H=-5 (at the base of the uphill) there are significant variation from the simulation data and the experimental data. Besides, you can see the k-epsilon method with Enhanced Wall Treatment is working better in the recirculation region.
I've decided to use this method because, given the low free stream velocity (just 0.0482 m/s), it is impossible to have y+>30.

So i've setup the flat terrain simulation, with the same inlet profiles, to investigate what are the reasons of this behavior.

It seems like the flow is not in fully developed state. Do you have any ideas about what can i do to improve the result?

 flotus1 August 10, 2013 15:19

What is your boundary condition for the dissipation of the tke at the inlet?
This could cause the discrepancy between the simulation and the experiment.

 Davide_sd August 10, 2013 15:47

for the turbulent dissipation rate, i'm using the default value of 1m^2/s^3; the paper doesn't provide a dissipation profile.

What value should i try?

 flotus1 August 10, 2013 16:50

This seems to be too much, which would also explain why the tke in your simulations decays too fast.
Since the flow is considered fully developed, you could run a simulation with a periodic channel and take the dissipation profile from this one.
Or you simply decrease it a few times by an order of magnitide until your results look better.

 Davide_sd August 10, 2013 18:39

Quote:
 Originally Posted by flotus1 (Post 444919) Since the flow is considered fully developed, you could run a simulation with a periodic channel and take the dissipation profile from this one.
Can you explain it better, please?

Quote:
 Originally Posted by flotus1 (Post 444919) Or you simply decrease it a few times by an order of magnitide until your results look better.
I've tryed to decrease the dissipation (as low as 1e-10) and i've noticed:
• k-epsilon with enhanced wall treatment: no changes at all;
• k-epsilon with standard wall function: some minor changes, still big differences in respect to the inlet profile.
• k-omega/k-omega SST: the outlet profile tend to approach the mid section profile, still with big differences in respect to inlet profile.

I was reading Fluent user guide, where i noticed the following:
"The relationship between the turbulent kinetic energy, k, and turbulence intensity, I, is: k = 3/2 * (u_avg * I)^2
where u_avg: mean flow velocity.
In the paper there was a chart of the longitudinal Reynolds stress profile, normalized in respect to u_delta^2 (u_delta: free stream velocity).
To calculate the turbulent kinetic energy i have used: k = 3/2 * (u'^2/u_delta^2) * u_delta^2. The error i've committed, could it be neglectable?

 flotus1 August 11, 2013 04:01

Let me start from the beginning.
The turbulent kinetic energy k is the trace of the Reynolds stress tensor

.

So if the velocity profiles are normalized by , you can recover the tke via

.

Now the way I see it, when you use

you assume that all normal Reynolds stresses are equal (), which is not the case for near wall turbulence.
So yes, with this assumption you introduce an error which is not negligible.
If the other components of the Reynolds stress tensor are given, you could use them to reconstruct the "correct" turbulent kinetic energy from the second equation.
Nevertheless, if you know the individual components of the Reynolds stress tensor from the experiment, you should consider using a Reynolds stress turbulence model.

Quote:
 Can you explain it better, please?
I meant that you can set up a separate simulation of a straight "channel" with the same dimensions and boundary conditions as your actual case.
In streamwise direction between inlet and outlet, you set up a periodic boundary condition and impose a mass flow rate (with the mass flow option of the periodic boundary) that recovers the correct average velocity.
This way, a profile of the dissipation of the tke develops which is in balance with the tke. You can impose it at the inlet of the actual simulation.

 Davide_sd August 11, 2013 15:05

1 Attachment(s)
Alex, thank you for your response!

I have to take a look at Reynold Stress Model!

In the meantime, i have extracted all the reynolds profiles from the paper.
Just to be sure, i want to ask you this: in the attachment you can see these profiles (the circles) and the interpolations of my UDF (the green lines). My simulation is a 2D case; to calculate the turbulent kinetic energy i have used:

Because the paper do not report all the values, i've done two assumptions:
1. at altitude = 0m, all the profiles has value = zero;
2. at altitude > 0.15m, the profiles tend to a vertical asymptote.
Are these two assumptions "good"?

As you can see from the plot, the paper reports the Reynolds shear stress profile -u'v'; fluent requires u'v'. Should i use the opposite sign profile?

 flotus1 August 11, 2013 15:46

Quote:
 to calculate the turbulent kinetic energy i have used:

Although your simulation is run on a 2-dimensional domain, the physics are still 3-dimensional. While the time-averaged velocity in w-direction is zero (thats why a 2-dimensional simulation with a RANS turbulence model is justified) there are fluctuations of the velocity in w-direction.
Accordingly, the tke should contain all three components including
.
Edit: The sentence here made no sense at all...

Quote:
 Because the paper do not report all the values, i've done two assumptions: at altitude = 0m, all the profiles has value = zero; at altitude > 0.15m, the profiles tend to a vertical asymptote.

Both assumptions are perfectly justified.

Quote:
 As you can see from the plot, the paper reports the Reynolds shear stress profile -u'v'; fluent requires u'v'. Should i use the opposite sign profile?
No. People usually report just to have less minus signs in the table, to have the plots all in the same sector of the coordinate system and to cause additional confusion:rolleyes:
There is no physical difference between and .

 flotus1 August 12, 2013 11:12

A correction to my last post. I put it in a new post so I hope you see it.

I claimed that the third component of the normal Reynolds stresses was comparatively small... Well that was complete nonsense and my only excuse is that it was late on a sunday evening.
In fact, it is of similar magnitude than the second component as we can see for example from the reproduction of DNS results in Popes book (pages 13 and 14 in this document):

http://pope.mae.cornell.edu/Turbulen...er7Figures.pdf

If you have no data for the third component, you could estimate its magnitude from a similar figure or from a periodic channel run with a Reynolds stress turbulence model.

 Davide_sd August 16, 2013 04:53

Seems like i'm having trouble to setup the periodic conditions.
I've been following fluent guide: mesh/modify-zones/make-periodic

Code:

mesh/modify-zones/make-periodic               Periodic zone [()] inlet Shadow zone [()] outlet Rotational periodic? (if no, translational) [yes] no Create periodic zones? [yes] yes Auto detect translation vector? [yes] yes
When i do this, the outlet condition disappear, and the inlet becomes periodic; this way i've lost all the inlet profiles...

 flotus1 August 16, 2013 05:39

That is what should happen. Dont worry, you are on the right path...

With a periodic boundary condition between inlet and outlet, you cannot specify any profiles for velocity or tke in the same way you did it with the inlet boundary condition.
The basic idea behind the periodic boundary conditions is to impose a mass flow rate that corresponds to the average velocity of your actual simulation.
The profiles for velocity and tke (and the epsilon profile we were searching for) develop as a result of the simulation.

Of course the profiles for velocity and tke wont match the profiles from the paper exactly.
But it is the best estimate we have to get the profile for the dissipation of the tke (and way better than assuming a value of 1;))

 Davide_sd August 20, 2013 12:19

I have done some tests:
k-epsilon (standard wall function, enhanced wall treatment), k-omega, SST aren't able to converge.
Reynolds Stress with enhanced wall treatment is not able to converge.
Reynolds Stress with standard wall function converge.

This are the results.

A couple of questions:
1 - why the value of k, u'u', v'v', w'w', u'v', epsilon at z=0 is different from zero?
2 - What can be said about these profiles, in respect to the experimental data?

 Davide_sd August 21, 2013 16:38

I have to make a correction to my previus post:
The result of the simulation with periodic boundary condition is shown in this image: Link 1
This results where obtained with Reynolds Stress Model with Standard wall function (I've tryed to use Enhanced wall treatment, but the simulation does not converge).

I've modified the profiles of that simulation in this way: Link 2; i've used these profiles in the same flat terrain simulation, with classic boundary condition (inlet := velocity inlet, outlet := pressure-outlet). Results:
1. Reynolds Stress Model + Standard Wall function (same as the previus simulation): not converging.
2. Reynolds Stress Model + Enhanced Wall treatment: converge. The flow is almost fully developed: the outlet velocity profiles is pretty similar to inlet velocity profile... There is some notable changes in the profiles of k, epsilon, u'u', v'v', w'w', u'v'...
3. k-epsilon + Enhanced Wall treatment: converge; the outlet velocity profiles is slightly different from inlet velocity profile...
Now i need to figure it out a way to "create" appropriate profiles of w'w' and epsilon, in order to get a fully developed simulation with the experimental data inlet velocity profile.

 flotus1 August 21, 2013 18:10

I hardly believe that you cannot get a converged solution with periodic boundary conditions for the flow over a flat plate.
These cases have to converge to floating point accuracy. It may take lots of iterations though.

Since you get streamwise velocity profiles of a laminar flow, the profiles for the turbulent quantities are useless too.
This may happen if you initialize the periodic case with zero k, epsilon and velocity values an when the Reynolds number is low. Or when the solution is not really converged.

If you tell me the Reynolds number of your case (based on the extent in wall-normal direction and the bulk velocity) I can check what is needed to obtain a suitable solution.

 Davide_sd August 22, 2013 15:38

Bulk velocity = 0.045920161602589 [m/s]

according to the paper:
Boundary layer thickness d = 100 [mm]
External velocity ud = 0.0482 [m/s]
Reynolds number Rd = 4,772
Friction velocity u* = 0.0028 [m/s]

Simulation with periodic boundary condition: link 1
Simulation with profiles obtained from the previus: link 2

 flotus1 August 23, 2013 14:03

3 Attachment(s)
So...
Here are the settings that definitely allow for a converged solution
• solver: pressure based, steady, 2d planar, double precision
• models: all off except the turbulence models
• material: density: 1000 kg/m³, viscosity 1.001e-3 Pa s
• mass flow rate at the periodic boundary: 11.48 kg/s
• initial conditions: x-velocity 0.04592 m/s, k and epsilon: 0.0001
• solution methods: second order upwind for momentum and turbulent quantities; for the RSM model, start with first order upwind
• under-relaxation factors: default for k-epsilon, reduce body forces and turbulent quantities for the RSM model
The computational domain is a rectangular box with 0.25 m height (wall-normal direction) and 0.1 m length (streamwise direction).
The mesh consists of 50x5 quad elements with y+ around 0.7.

Took around 10k iterations for the k-epsilon model to converge and 100k for the RSM model... there might be better setting to improve on this but the calculation times are low because of the small mesh.

The results:
Attachment 24786Attachment 24785Attachment 24784

All times are GMT -4. The time now is 12:47.