CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   low Reynolds Model for pipe flow (http://www.cfd-online.com/Forums/openfoam/90132-low-reynolds-model-pipe-flow.html)

RugbyGandalf July 1, 2011 04:57

low Reynolds Model for pipe flow
 
Dear Community,

i would like to simulate a pipe flow with has a low Reynolds - Number.

Does someone know, what low-Re-turbulence-model is best for?
I already tried using LaunderSharma KE - it works with only 2% difference from u_max in comparison with Hagen-Poiseuille - but i do not know, if LaunderSharmaKE was developed for such applications.

So does someone know about this?
I am using the simpleFoam solver!

Greetings

Martin

bastil July 1, 2011 06:40

Quote:

Originally Posted by RugbyGandalf (Post 314363)
Dear Community,

i would like to simulate a pipe flow with has a low Reynolds - Number.

Does someone know, what low-Re-turbulence-model is best for?


Martin,

it is a pitfall: A Low-Reynolds turbulence model is NOT designed for low reynolds numbers. It is designed for resolving the near wall layer without wall functions. Therefore, you need to create your mesh different if you use a low-Re model compared to a Hi-Re model. I suspect for a pipe flow with modest separations a Hi-Re model should be sufficient. However, you have to make sure your mesh fits for a Hi-Re model.

Regards Bastian

Eren10 July 1, 2011 08:51

Is there a tutorial of LaunderSharma, I want to copy their files, however, the files of LaunderSharma should be almost the same as the k epsilon.

RugbyGandalf July 1, 2011 08:54

2 Attachment(s)
I need to resolve the near wall layers without wallfunctions!
The Reynolds-Numbers vary between 150 up to 320...

I do not think, that a high Re - Model is able to solve the flow right!
My pipe has a diameter of 0.004 m - in fact it consists only of near wall layers ;)

i also added a picture showing my grid and one which shows the velocity field, that kOmegaSST Model offers in comparison to Hagen-Poiseuille-profile!

Martin

bastil July 1, 2011 10:20

Quote:

Originally Posted by RugbyGandalf (Post 314398)
I need to resolve the near wall layers without wallfunctions!

Why?


Quote:

Originally Posted by RugbyGandalf (Post 314398)
The Reynolds-Numbers vary between 150 up to 320...

Well in that case I think your case is laminar and you need to run it laminar, e.g. without turbulence models... Otherwise you imprint turbulence where none exists.

If you still want to run a low Reynolds model (even though it is not necessary) you need to have a much lower thickness of the first cell next to the wall. The appropriate value of this can be estimated with the y+ value.

Regards Bastian.

liguifan July 1, 2011 10:32

Hi Martin,

You mesh look quite nice.

Just want to ask that did you use transfinite progression stuff to make the layers at boundary more denser than those away from boundary?

Thanks a lot.

rob3rt 0ng July 2, 2011 05:24

Hi Eren,

You can lookup nacaAirFoil tutorial but it's for compressible case though. Otherwise, you always can look for launderSharma codes from Doxygen.

Regards,
Robert

Martin Hegedus July 2, 2011 11:35

Quote:

Originally Posted by RugbyGandalf (Post 314363)
Dear Community,

i would like to simulate a pipe flow with has a low Reynolds - Number.

Does someone know, what low-Re-turbulence-model is best for?
I already tried using LaunderSharma KE - it works with only 2% difference from u_max in comparison with Hagen-Poiseuille - but i do not know, if LaunderSharmaKE was developed for such applications.

So does someone know about this?
I am using the simpleFoam solver!

Greetings

Martin

Interesting, I never gave much thought to a turbulence model in a pipe before, until now. I'm just hypothesizing, but I assume the eddy viscosity might keep building inside the pipe. Of course close to the walls the eddy viscosity is forced to go to zero. A low turbulence model might just delay the build-up. Eventually an equilibrium will be reached between the construction and destruction terms. Because of the eddy viscosity distribution, your velocity will be flatish on top (i.e. the high eddy viscosity in the middle makes the center flow rigid) and steep on the side (since eddy viscosity goes to zero at side).

Laminar is probably the way to go.

Just my thoughts, and if anyone disagrees with my conjecture, please include your thoughts.

RugbyGandalf July 4, 2011 11:19

Dear Bastian,

what y+ value do i need? My calculations actually run with y+ avg of 0.8...
is this to high?

@ Martin:
maybe laminar seems to be the best way... it was a test with low-Re... In fact, LaunderSharmaKE gives out great results. I will also calculate all my cases with laminar flow and compare them with LaunderSharmaKE.

For information: LaunderSharmaKE was originally designed to solve the flow and heat / mass transfer near a rotating disk.

@ liguifan: i used meshGrading with blockMesh to make the cells finer at the wall.

RugbyGandalf July 4, 2011 11:28

2 Attachment(s)
I also have another question:

i am calculating the flow through bend pipes, to get to know about the wall shear stress:

Does someone have an idea, how i could get wall shear stress in cylinder coordinates from a result, that gives out Cartesian ones?
The aim is, to get a chart, which shows the wall stress in dependence from pipe-lenght...

maybe the pictures will make it clearer! The chart is only an example!

Thank you very much for your answers!

Martin


All times are GMT -4. The time now is 22:51.