CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   RANS modelling and URANS methods in unsteady flow simulations (http://www.cfd-online.com/Forums/openfoam-solving/118990-rans-modelling-urans-methods-unsteady-flow-simulations.html)

immortality June 7, 2013 14:50

RANS modelling and URANS methods in unsteady flow simulations
 
Hi
I have read in some texts and papers that RANS turbulent simulation is not appropriate for unsteady cases and for example in https://www.google.com/url?sa=t&rct=...47534661,d.bGE
this subject in page 24 has mentioned and has proposed to use a URANS method.
so I have two clear question:
1)how much may be the error in using RANS models in unstedy flow simulations?(so we should give up it totally?)
2)is there a(or some) URANS method in OpenFOAM?
thanks for consideration.

wyldckat June 9, 2013 13:28

Hi Ehsan,

AFAIK, OpenFOAM only has these: http://www.openfoam.com/features/turbulence.php
Quote:

OpenFOAM offers a large range of methods and models to simulate turbulence. The methods include:
  • Reynolds-average simulation (RAS), also known as Reynolds-averaged Navier-Stokes (RANS): The governing equations are solved in ensemble-averaged form, including appropriate models for the effect of turbulence. See the list of incompressible and compressible RAS models for more information.
  • Large eddy simulation (LES): Large turbulent structures in the flow are resolved by the governing equations, while the effect of the sub-grid scales (SGS) are modelled. The scale separation is obtained by applying a filter to the governing equations which also influences the form of the SGS models. The list of LES models contains information about models, LES filters and filter width functions.
  • Detached eddy simulation (DES): Hybrid method that treats near-wall regions with a RAS approach and the bulk flow with an LES approach. DES models are found in the list of LES models.
  • Direct numerical simulation (DNS): Resolves all scales of turbulence by solving the Navier-Stokes equations numerically without any turbulence modelling. DNS simulations can be performed in OpenFOAM using the dnsFoam solver.

From what I can see, the closest you've got to something like "URANS" is "DES".

As for using RANS in unsteady cases: it depends on the nature of the simulation. As I've said in a previous email or thread, possibly you'll need to switch to LES or DES, in order to properly simulate your specific cases. At the very least, for comparing if the solutions are approximate or not.
But the problem with LES is that it's far more heavy computationally, although DES might ease on the computational power needed...

On the topics of DES, all I know are on these two threads:
Best regards,
Bruno

edit: continue reading down to and including post #13 for an updated answer.

immortality June 9, 2013 13:45

Hi Bruno
are there any test case to see whats the settings for LES or DES?

wyldckat June 9, 2013 13:56

Quote:

Originally Posted by immortality (Post 432953)
are there any test case to see whats the settings for LES or DES?

On the first link I pointed out on the paragraph "On the topics of DES", has a case that uses DES.
I have not tried to compare with LES, because that case never entered into the LES region, because there was no obstacle inside it or anything that unleashed complex turbulence :(


In reference to your thesis: since it's a master thesis, you can always indicate, in the section "future work", that there should be a comparison with LES, in order to ascertain the validity of the simulations.
Keep in mind that 5-10 years ago, LES could only be properly performed using supercomputers! Nowadays, a home made cluster or a top grade workstation can handle some of these kinds of LES simulations, but it could still take a week or so to do a single simulation, depending on the mesh resolution!

immortality June 9, 2013 14:09

then in DES it sometimes turns LES(when flow be very turbulent,yes?)
Oh! my case is complicated and slow enough.maybe I test a DES not LES with these circumstances you prescribed!
thanks so much.

wyldckat June 9, 2013 14:11

Quote:

Originally Posted by immortality (Post 432957)
then in DES it sometimes turns LES(when flow be very turbulent,yes?)

From what I could figure out: yes, it switches from RAS to LES in the regions it thinks it should use LES. And from OpenFOAM's website, RAS (RANS) is always used near the walls.

immortality June 9, 2013 17:37

well,i try a DES method.
But i don't know exactly which method of LES is better for a compressible unsteady case that i have.
Any suggestion and explanation is thanked.

HaveSomeQuestions July 27, 2013 18:41

URANS question
 
Hi,

I also have a URANS question. It seems like when I use URANS (with all 2nd order upwind solvers), the oscillations decay away. This is even though the flow configuration (flow around a blunt body) should have unsteadiness. Do you have any advice on why this would be happening? My inflow conditions are all steady. Do I have to use forced inlet conditions to sustain the oscillations?

Thanks!

immortality July 28, 2013 07:20

Hi
how you use URANS?which model in OF is of type of URANS?
what do you mean by forced inlet condition?

HaveSomeQuestions July 28, 2013 12:36

I'm using RKE in Fluent. By "forced", I mean "unsteady."

Thanks.

wyldckat August 17, 2013 14:12

Greetings to all!

I'm a bit late to the conversation, but here goes anyway...

@HaveSomeQuestions:
Quote:

Originally Posted by HaveSomeQuestions (Post 442386)
I also have a URANS question. It seems like when I use URANS (with all 2nd order upwind solvers), the oscillations decay away. This is even though the flow configuration (flow around a blunt body) should have unsteadiness.

Looks to me that you didn't read the OpenFOAM User Guide... namely the section 4.4: http://www.openfoam.org/docs/user/fvSchemes.php
From there:
Quote:

Originally Posted by http://www.openfoam.org/docs/user/fvSchemes.php
upwind First order, bounded

Therefore, it's only natural that with a first order divergence scheme, that you get such nice results ;)

Quote:

Originally Posted by HaveSomeQuestions (Post 442440)
I'm using RKE in Fluent.

Then I think that's not exactly URANS... technically that should be the "Realizable k-Epsilon" turbulence model... but I could be wrong.

Best regards,
Bruno

immortality August 17, 2013 15:24

Quote:

Then I think that's not exactly URANS... technically that should be the "Realizable k-Epsilon" turbulence model... but I could be wrong.
there is not any URANS in OF,is?

wyldckat August 17, 2013 15:53

Hi Ehsan,

Since you asked once again... I did some more searching and researching... and apparently I can now stand corrected, I suppose - here's a quote from an old post (from this thread: http://www.cfd-online.com/Forums/ope...algorithm.html):
Quote:

Originally Posted by vkrastev (Post 293256)
About my second question, at this moment I'm running an exeternal aerodynamics case in URANS mode (Realizable k-epsilon turbulence model, mesh of about 3 milions cells) using the pimpleFoam solver: the case is running with nOuterCorrectors set to 2 (thus, only one additional integration over the time step), number of PISO correctors also equal to 2 and with a constant time step value wich corresponds to a max Co of about 3.4.

Therefore, looks like HaveSomeQuestions has a very good reason to say that RKE is URANS.

Also, from my research, here's what I found that might come in handy:

Last but not least: I found at least around 3 or 4 threads here at CFD-Online of people who apparently didn't search the forum for more information... and ironically, they got no answer in return.

Best regards,
Bruno

immortality August 17, 2013 16:16

thanks Bruno for searching despite of your tiredness,
only please correct the first link"on the pimpleFoam".
and is Jose your brother? :)
I'll edit this post after reading links.

wyldckat August 17, 2013 16:40

Quote:

Originally Posted by immortality (Post 446349)
only please correct the first link"on the pimpleFoam".

Thanks! I've fixed it!

Quote:

Originally Posted by immortality (Post 446349)
and is Jose your brother? :)

:confused: No. "Santos" is a popular family name here in Portugal.
Better yet, there should be more than 10 "Bruno Santos" in just Portugal, not even counting Brazil and other countries. Which is why people here in Portugal have 4 or more names, not just first and last names.

immortality August 17, 2013 17:37

sorry,I was thinking that user is in your family since a long time :)

RodriguezFatz October 7, 2013 07:42

Don't you call "URANS" every RANS simulation that is unsteady? E.g. by unsteady inlet or globally unstable flow, such as bluff-body flows? So basically you can use every RANS model for URANS by switching to any unsteady solver (Piso, pimple, ...).

immortality October 9, 2013 06:18

Hi Philip
do you mean if I use any of turbulent models in unsteady solvers,the RANS model will become URANS automatically?
is there any other comment?
thanks.

skyinventorbt October 9, 2013 06:54

Quote:

Originally Posted by immortality (Post 455900)
Hi Philip
do you mean if I use any of turbulent models in unsteady solvers,the RANS model will become URANS automatically?
is there any other comment?
thanks.

Dear Ehsan,
When you specify ddtSchemes (i.e. not steady state), the simulation becomes unsteady, i.e. you are using URANS.

I do not know how far URANS is physically meaningful.

Any comments ?
--
KANNAN

RodriguezFatz October 9, 2013 07:06

Ehsan, yes, that is right.
I found from Jochen Fröhlich, Progress in Aerospace Sciences 44 (2008) 349-377, Hybrid LES/RANS methods for the simulation of turbulent flows:
"...It has become common to name RANS modeling as URANS whenever the computed solution is time-dependent."

Kannan, I don't see why this wouldn't be physically meaningful. RANS model derivation does not say anything about the meaning of the <...> operator. This can be temporal mean, phase average,... Just some basic features must be supported by <...> such as linearity and so on. Now, the turbulence model doesn't know about this.
Only the turbulent fluctuations of certain time-scales are damped out by the model. If the inlet is unsteady, with a time-scale slower than the turbulence, you will get a time-dependent solution. On the other hand, for bluff body flows, you will get such things as vortex streets, which are physically meaningfull as well.


All times are GMT -4. The time now is 16:49.