epsilon and omega free stream BC's

immortality · May 23, 2013, 16:45

in this page:
http://www.cfd-online.com/Wiki/Turbu...ary_conditions
there are different formulas for epsilon and omega,I want to test with both kOmegaSST and k-epsilon-realizable(does anyone knows how to set it in OF?)
how can find out which is appropriate for OF with your experience?

for epsilon we have:
$\epsilon = C_\mu \, \frac{k^\frac{3}{2}}{l}$
or
$\epsilon = C_\mu^\frac{3}{4} \, \frac{k^\frac{3}{2}}{l}$
or
$\epsilon = C_\mu \, \frac{\rho \, k^2}{\mu} \, (\frac{\mu_t}{\mu})^{-1}$

and for omega we have:
$\omega = \frac{\sqrt{k}}{l}$
or
$\omega = C_\mu^{-\frac{1}{4}} \, \frac{\sqrt{k}}{l}$
or
$\omega = \frac{\rho \, k}{\mu} \, (\frac{\mu_t}{\mu})^{-1}$

immortality · May 25, 2013, 16:12

Hi again
I saw in page 25 of this thesis that he has used : $\frac{3}{2} \, (l \, I \, U)^{2}$ (I managed this LaTeX formula at last!)

the thesis:
Simulation and validation of
compressible flow in nozzle geometries
and validation of OpenFOAM for this application

is this work and change in formula by adding l is acceptable?
http://s2.picofile.com/file/77781039...rbeit.pdf.html

wyldckat · May 25, 2013, 17:17

Hi Ehsan,

Quick note - here's another link to said thesis: http://www.rw.ethz.ch/alumni/thesis/...sterarbeit.pdf

From what I can figure out, the author of the thesis went along with the spirit of this whole turbulence stuff.
If you look at the first sections of the wiki page you've mentioned earlier, you'll see in "Modified turbulent viscosity" that the "turbulent length scale" is used for the "modified turbulent viscosity". This is possibly what influenced the author's decision.

As for the wiki, it does have some more helpful hints, namely the one about "Eddy viscosity ratio": http://www.cfd-online.com/Wiki/Eddy_viscosity_ratio
In essence, if you are able to calculate the "turbulent length scale", it's easier to calculate through it, instead of through the "Eddy viscosity ratio".

In case you haven't seen how to calculate the relevant parameters, here's a quote:

Quote:

is the turbulence intensity and

is the turbulent length scale.

As for which calculation to use: my usual rule of thumb is to use the equations I can calculate

Best regards,
Bruno

Eloise · September 6, 2013, 09:49

Hi Ehsan,
I'm also interested in some free-stream turbulence problems. I run a simulation of an object in uniform flow and I would like to perform a sensitivity study on the inlet turbulence intensity level. I've tested several TI levels (3% to 7%), but in all cases the TI drops to about 1% a few cells after the inlet. So whatever TI level I put at the inlet, my object is always in a 1% TI level.
Have you experienced something similar with your simulations? If not, what is the way to maintain TI through the domain?
About my case: the velocity profile is steady and uniform, the mesh is uniform, I use k-omega SST turbulence model.
Best regards,
Eloïse

wyldckat · September 7, 2013, 08:47

Hi Eloïse,

A few questions regarding your case:

Is it 2D or 3D?
Have you first tested to see if it runs well in laminar flow?
- Found this after a quick search: http://www.mathematik.tu-dortmund.de...aTurek2011.pdf
Is it a steady-state or transient simulation?
The turbulence intensity and so on, is it similar throughout the whole domain or is it only near the object that it keeps the low turbulence values?

Best regards,
Bruno

immortality · September 7, 2013, 09:00

Quote:

Hi Ehsan,
I'm also interested in some free-stream turbulence problems. I run a simulation of an object in uniform flow and I would like to perform a sensitivity study on the inlet turbulence intensity level. I've tested several TI levels (3% to 7%), but in all cases the TI drops to about 1% a few cells after the inlet. So whatever TI level I put at the inlet, my object is always in a 1% TI level.
Have you experienced something similar with your simulations? If not, what is the way to maintain TI through the domain?
About my case: the velocity profile is steady and uniform, the mesh is uniform, I use k-omega SST turbulence model.
Best regards,
Eloïse

Hi Eloise
sorry for delay,how did you notice that TI in internal cells becomes low?

Eloise · September 9, 2013, 03:54

Quote:

Originally Posted by wyldckat

Is it 2D or 3D?
Have you first tested to see if it runs well in laminar flow?
- Found this after a quick search: http://www.mathematik.tu-dortmund.de...aTurek2011.pdf
Is it a steady-state or transient simulation?
The turbulence intensity and so on, is it similar throughout the whole domain or is it only near the object that it keeps the low turbulence values?

Hi Bruno,

1. It is a 3D case
2. I ran the case in laminar and haven't had any specific problem. Do you think of something specific which should be checked in the laminar case? I'll have a look at the paper, thanks for the link.
3. It is a steady-state simulation
4. The TI decreases in the very first cells after the inlet. Around the object, the TI increases again. (see attached image, which is a cut of the domain) Ehsan: that's how I detected the issue.

Regards,
Eloïse

immortality · September 9, 2013, 06:30

How did you define turbulence intensity field?is there any postProcessing utility for that?

Eloise · September 9, 2013, 07:53

Quote:

Originally Posted by immortality

How did you define turbulence intensity field?is there any postProcessing utility for that?

This page shows you how to get it from the k field. You can then use the "calculator" in paraView to define a new variable in your field.

Eloïse

immortality · September 9, 2013, 08:33

how you have defined TI in inlet?
you should set it to a constant so that can define k in inlet not inverse.

Eloise · September 9, 2013, 09:47

Quote:

Originally Posted by immortality

how you have defined TI in inlet?
you should set it to a constant so that can define k in inlet not inverse.

I compute the k and omega values corresponding to the desired TI level and use the "fixedValue" for k and omega at the inlet. Do you think the "turbulentIntensityKineticEnergyInlet" for k and "turbulentMixingLengthFrequencyInlet" for omega makes any difference? (as described here)

Eloïse

immortality · September 9, 2013, 12:28

is velocity constant in inlet?if it varies during run and you have set a fixed k and omega it might makes some error,I don't know how you set your BC's,could you attach them?

wyldckat · September 9, 2013, 15:32

Greetings to all!

@Eloïse: Well, the only way to maintain the turbulence intensity is if you introduce small obstacles, such as wires or something like that.

Because there are a few details in play here and all of them are related to the solver doing what it was told to do. More specifically:

There's a lot of empty space between the inlet and the obstacle. It's natural that any and all vortices will fade away, given enough space.
- Unless you inject with a very high speed and high turbulence intensity.
The "fvSchemes" might be using too much 1st order div schemes. Or in other words, if all div equations are solved with 1st order, you'll see a very quick smoothing of the results. This is why it usually converges and converges fast!
The RAS turbulence models are only representative of turbulence, they usually don't simulate the micro-vortices themselves. For that, you would need a much finer mesh + LES or DNS.

Which reminds me... have you ever seen those old fluid dynamics/mechanics videos showing how turbulence work and so on? I can't remember where I kept the link for them...
Anyway, one of them shows the effect of a wire inducing turbulence.

Best regards,
Bruno

Eloise · September 10, 2013, 04:38

Quote:

Originally Posted by immortality

is velocity constant in inlet?if it varies during run and you have set a fixed k and omega it might makes some error,I don't know how you set your BC's,could you attach them?

Nothing fancy in my BC. Constant velocity, k and omega, and nothing varies in time. I guess it is the same as in the motorbike tutorial.

@Bruno: Thanks for the advices on fvSchemes. I'll have a look at that too. I guessed that if there is nothing to create velocity gradients and maintain turbulence, then the turbulence would fade out. Or at least that's how I understood my problem. I asked about it here because I was wondering if others observed the same and if something could be done about it

May 23, 2013, 16:45	epsilon and omega free stream BC's	#1
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 27	in this page: http://www.cfd-online.com/Wiki/Turbu...ary_conditions there are different formulas for epsilon and omega,I want to test with both kOmegaSST and k-epsilon-realizable(does anyone knows how to set it in OF?) how can find out which is appropriate for OF with your experience? for epsilon we have: $\epsilon = C_\mu \, \frac{k^\frac{3}{2}}{l}$ or $\epsilon = C_\mu^\frac{3}{4} \, \frac{k^\frac{3}{2}}{l}$ or $\epsilon = C_\mu \, \frac{\rho \, k^2}{\mu} \, (\frac{\mu_t}{\mu})^{-1}$ and for omega we have: $\omega = \frac{\sqrt{k}}{l}$ or $\omega = C_\mu^{-\frac{1}{4}} \, \frac{\sqrt{k}}{l}$ or $\omega = \frac{\rho \, k}{\mu} \, (\frac{\mu_t}{\mu})^{-1}$ __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. Last edited by immortality; May 25, 2013 at 16:01.

May 25, 2013, 16:12		#2
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 27	Hi again I saw in page 25 of this thesis that he has used : $\frac{3}{2} \, (l \, I \, U)^{2}$ (I managed this LaTeX formula at last!) the thesis: Simulation and validation of compressible flow in nozzle geometries and validation of OpenFOAM for this application is this work and change in formula by adding l is acceptable? http://s2.picofile.com/file/77781039...rbeit.pdf.html __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

September 7, 2013, 08:47		#5
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,982 Blog Entries: 45 Rep Power: 128	Hi Eloïse, A few questions regarding your case: Is it 2D or 3D? Have you first tested to see if it runs well in laminar flow? Found this after a quick search: http://www.mathematik.tu-dortmund.de...aTurek2011.pdf Is it a steady-state or transient simulation? The turbulence intensity and so on, is it similar throughout the whole domain or is it only near the object that it keeps the low turbulence values? Best regards, Bruno immortality likes this. __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

September 9, 2013, 06:30		#8
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 27	How did you define turbulence intensity field?is there any postProcessing utility for that? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

September 9, 2013, 08:33		#10
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 27	how you have defined TI in inlet? you should set it to a constant so that can define k in inlet not inverse. __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

September 6, 2013, 09:49		#4
Eloise Senior Member Eloïse Join Date: Jul 2012 Location: Trondheim, Norway Posts: 113 Rep Power: 14	Hi Ehsan, I'm also interested in some free-stream turbulence problems. I run a simulation of an object in uniform flow and I would like to perform a sensitivity study on the inlet turbulence intensity level. I've tested several TI levels (3% to 7%), but in all cases the TI drops to about 1% a few cells after the inlet. So whatever TI level I put at the inlet, my object is always in a 1% TI level. Have you experienced something similar with your simulations? If not, what is the way to maintain TI through the domain? About my case: the velocity profile is steady and uniform, the mesh is uniform, I use k-omega SST turbulence model. Best regards, Eloïse

September 9, 2013, 12:28		#12
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 27	is velocity constant in inlet?if it varies during run and you have set a fixed k and omega it might makes some error,I don't know how you set your BC's,could you attach them? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

September 9, 2013, 15:32		#13
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,982 Blog Entries: 45 Rep Power: 128	Greetings to all! @Eloïse: Well, the only way to maintain the turbulence intensity is if you introduce small obstacles, such as wires or something like that. Because there are a few details in play here and all of them are related to the solver doing what it was told to do. More specifically: There's a lot of empty space between the inlet and the obstacle. It's natural that any and all vortices will fade away, given enough space. Unless you inject with a very high speed and high turbulence intensity. The "fvSchemes" might be using too much 1st order div schemes. Or in other words, if all div equations are solved with 1st order, you'll see a very quick smoothing of the results. This is why it usually converges and converges fast! The RAS turbulence models are only representative of turbulence, they usually don't simulate the micro-vortices themselves. For that, you would need a much finer mesh + LES or DNS. Which reminds me... have you ever seen those old fluid dynamics/mechanics videos showing how turbulence work and so on? I can't remember where I kept the link for them... Anyway, one of them shows the effect of a wire inducing turbulence. Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
calculation of k, epsilon and omega	kroetenechse	OpenFOAM Pre-Processing	31	March 5, 2021 11:32
Bounding epsilon or bounding omega	Stylianos	OpenFOAM	8	February 23, 2018 14:41
Problem with K omega boundary conditions	malaboss	OpenFOAM Pre-Processing	6	April 20, 2015 00:25
problem from k epsilon to k omega	NJG	OpenFOAM Running, Solving & CFD	0	April 15, 2013 09:24
why omega instead of epsilon in turbulence modeling	pgoyal10	Main CFD Forum	1	May 5, 2012 12:02