CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

LES turbulent pipe flow

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree8Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   August 24, 2006, 12:45
Default Dear all, I would like to m
  #1
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
Dear all,

I would like to make a LES calculation of a turbulent pipe flow.
I made a 3D grid and I would like to initialize the field with some turbulence.

Can I use boxTurb somehow? Is there any tool to add white noise to a uniform flowfield?
panara is offline   Reply With Quote

Old   August 24, 2006, 13:36
Default Try this http://www.cfd-on
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Try this

perturbCylinder.tgz

You have to edit the code and set the cylinder diameter and Re_tau. It only works for flow in the x direction. It will set up wavy sinusoidal precursor perturbations that should develop into fully blown turbulence after a few dozen flow-through times.
solefire and songwukong like this.
eugene is offline   Reply With Quote

Old   August 25, 2006, 02:13
Default Thanks very much Eugene, do y
  #3
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
Thanks very much Eugene,
do you have a reference on the formula you used in perturbCylinder, I would like to understand what I am doing...

Daniele
panara is offline   Reply With Quote

Old   August 25, 2006, 04:27
Default Hi Daniele, I would like to
  #4
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Hi Daniele,

I would like to know, what kind of inlet you use; especially, how do create turbulence at the inlet?

Greetings!
Fabian
braennstroem is offline   Reply With Quote

Old   August 25, 2006, 04:36
Default Hi Fabian, I am using cylcic
  #5
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
Hi Fabian,
I am using cylcic boundary condition at the inlet and outlet of the pipe plus a source term in the momentum equation to sustain the flow.

I have used this configuration already with another code and in a channel configuration initializing the flowfield with white noise.
It worked for the channel, but I am having problems with openFoam and the pipe configuration (I just started to try.. )

I saw that in OpenFoam exists also a turbulent inlet... but I didn't try it..

Anyway could anybody give some reference on the compressible LES turbulence models implemented in OpenFoam?

Thanks
panara is offline   Reply With Quote

Old   August 25, 2006, 05:32
Default Schoppa & Hussain, "Coherent s
  #6
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Schoppa & Hussain, "Coherent structure dynamics in near-wall turbulence", Fluid Dynamics Research, Vol 26, p 119-139, 2000.

Although they don't explain everything in detail either. Not too difficult to figure out though.
mgg likes this.
eugene is offline   Reply With Quote

Old   August 27, 2006, 15:45
Default Dear all, I have a question
  #7
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
Dear all,
I have a question about boundary conditions in LES:

is it possible to use cyclic boundary conditions for velocity and pressure and non cyclic boundary conditions for temperature? if yes how can I set them?

I would like to simulate a turbulent pipe flow with heat transfer from the wall. Using the cyclic condition on P and U I ensure that the flow remains turbulent and using a source term in the momentum equation I sustain the flow.
(I have already tryed this configuration and works very well)

The Temperature instead cannot be cyclic, the temperature profile at the inlet has to be different from the one at the outlet..

Does anybody have an idea on how to do that in LES?

Regards
Daniele
panara is offline   Reply With Quote

Old   August 28, 2006, 01:53
Default Hi Daniele, thanks! Does an
  #8
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Hi Daniele,

thanks! Does anybody know, if the turbulent inlet is useful for LES?

Greetings!
Fabian
braennstroem is offline   Reply With Quote

Old   August 28, 2006, 02:25
Default turbulentInlet is useful but n
  #9
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,761
Rep Power: 21
hjasak will become famous soon enough
turbulentInlet is useful but not great: it will create uncorellated noise which is better than nothing (well, not much) :-)

The issue is that turbulence has structure that needs to be captured: vortices, correlations, energy casecade and none of this is captured by the white noise in turbulence inlet b.c. In practice, your implied length-scale at the inlet is very small and this kill the turbulence.

For a serious LES simulation you need to do better, but this may give you a good start. Examples would be a fully developed duct flow as a source of inlet data, a sampling plane somewhere else in the domain or a side-by-side POD simulation providing you correlated inlet snapshots.

Hrv
rajibroy likes this.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 28, 2006, 03:04
Default I was infact thinking to make
  #10
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
I was infact thinking to make a periodic pipe and use the inlet/outlet data as an input for another non periodic pipe simulation with zeroGradient at the outlet (that should affect not too much the simulation )...

but how can I implement that in openFoam?
I can make a two region computation like I did in conjugateFoam and set the inlet of the second non periodic mesh as the inlet/outlet of the first mesh with cyclic conditions... but can I just use

U2.boundaryField()[inlet]=U1.boundaryField()[cyclic]

??

I mean, I guess that the cyclic patch are seen in a different way..

any suggestion before I start to look more in details the code?

What do you mean with side-by-side POD?

Another question, can I define in OpenFoam a cyclic patch in the middle of the domain?
I mean: can I define a cyclic BC between the pipe inlet and an internal section of the pipe, plus the condition of zero gradient for U at the pipe exit?

sorry for the long mail,

Daniele
panara is offline   Reply With Quote

Old   August 31, 2006, 06:28
Default Dear all, could anybody giv
  #11
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
Dear all,

could anybody give any reference on the LES SGS models implemented in OpenFoam?

which one is best suited for a wall-resolved LES computation ( no wall functions ) ?

Daniele
panara is offline   Reply With Quote

Old   September 1, 2006, 04:43
Default Heya, Look for the paper:
  #12
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,761
Rep Power: 21
hjasak will become famous soon enough
Heya,

Look for the paper:

C.Fureby, G.Tabor, H.Weller & A.D.Gosman
"A Comparative Study of Sub Grid Scale Models in Homogeneous Isotropic Turbulence", Phys.Fluids., 9#5, pp1416 - 1429 [1997]

It's got details of most models implemented in OpenFOAM. I know it's a bit old, sorry. There will also be a PhD Thesis on LES from Eugene de Villiers of Imperial College coming soon, but I don't think we can have it just yet. You will find a lot of stuff on wall handling as well - all the work has been done with OpenFOAM.

Hrv
solefire likes this.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   November 22, 2006, 08:39
Default Hi everyone I used oodles
  #13
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hi everyone

I used oodles for turbulent pipe flow modeling
but the results are not as I expected from LES.

I do this with mesh&parameter changing in pitzDaily.

Please help me.

regards
marhamat
marhamat is offline   Reply With Quote

Old   November 23, 2006, 19:03
Default Hi everyone I add that: Re
  #14
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hi everyone

I add that:
Re=4000,input velocity is uniform=2m/s
Meshes are fine enough & Co<0.52
Can i expect good advantages from results?
Nobody have any idea?

Regards
marhamat
marhamat is offline   Reply With Quote

Old   December 25, 2006, 03:47
Default Hi everyone I wan't to implem
  #15
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hi everyone
I wan't to implement the package that Eugene attached in this page for turbulent pipe flow initialazation .
I'm beginner in openfoam using&programming.

HOw i can use this code?
How i run this package for my case?
What is the effect of this code in OpenFOAM cases(for example:oodles)
Which files changes after running the code?

Please explaine me the details.
any help are useful for me

Best regards
Marhamat
marhamat is offline   Reply With Quote

Old   December 25, 2006, 03:56
Default Hi everyone I wan't to implem
  #16
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hi everyone
I wan't to implement the package that Eugene attached in this page for turbulent pipe flow initialazation .
I'm beginner in openfoam using&programming.

HOw i can use this code?
How i run this package for my case?
What is the effect of this code in OpenFOAM cases(for example:oodles)
Which files changes after running the code?

Please explaine me the details.
any help are useful for me

Best regards
Marhamat
marhamat is offline   Reply With Quote

Old   February 6, 2007, 08:50
Default Hi everyone As i explained be
  #17
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hi everyone
As i explained before i used oodles for turbulent pipe flow modeling.
So i imposed universal results as a inlet velocity.
I used inlet as a inlet boundry condition & wallfor wall boundry condition&
inletOutlet for outlet boundry condition.
You see the result in some sections.

Q1)Is this results are reasonable?
Results in different section are different.
Q2)Do this mean that the solution didn't converged Or flow isn't developed?
I imposed developed velocity profile in inlet and we know in inlet the pressure gradient is zero.In my idea these are paradox, So for pressur gradient effect decreasing on flow i increased the pipe length from L=5d to L=30d.
But result aren't acceptable .

Q3)Are you have any idea?

Regards
Marhamat
marhamat is offline   Reply With Quote

Old   February 6, 2007, 09:17
Default Hi everyone As i explained be
  #18
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hi everyone
As i explained before i used oodles for turbulent pipe flow modeling.
So i imposed universal results as a inlet velocity.
I used inlet as a inlet boundry condition & wallfor wall boundry condition&
inletOutlet for outlet boundry condition.
You see the result in some sections.

Q1)Is this results are reasonable?
Results in different section are different.
Q2)Do this mean that the solution didn't converged Or flow isn't developed?
I imposed developed velocity profile in inlet and we know in inlet the pressure gradient is zero.In my idea these are paradox, So for pressur gradient effect decreasing on flow i increased the pipe length from L=5d to L=30d.
But result aren't acceptable .In pipe length direction the velociy profile near to lamiar velocity profile.

Q3)Are you have any idea?

Regards
Marhamat
marhamat is offline   Reply With Quote

Old   February 6, 2007, 09:36
Default Sorry for duplicate sending an
  #19
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Sorry for duplicate sending and for Q1
Marhamat
marhamat is offline   Reply With Quote

Old   February 6, 2007, 10:27
Default Hi Marhamat! I've been trying
  #20
Member
 
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 8
ville is on a distinguished road
Hi Marhamat!
I've been trying to carry out a simulation
of turbulent pipe flow with Xoodles with parabolic
initial flow field that I've perturbed with
a) Gaussian noise with different amplitudes
b) sinusoidal perturbations in radial coordinate
(i.e. streamwise component = parabola + u(r), where u(r)=a*sin(k*r)) .
The pipe length was 6d and I ran it on cyclic bc's
parallel (btw the cyclic patches needed to be on the same processor).
So far I haven't been able to make this perturbed system break into turbulence but the latest results imply that it would take something like 150d flow throughs for this to happen since there
are visible fluctuations in k at the wall at
around 40d flow through times. This I was
able to see when I decreased the flux limiter parameter psi from value 1 to 0.

I've also tried turbulent inlet bc but this
is not breaking into turbulence because the
perturbations die out too fast.

The options for 'getting turbulent conditions
quickly' seem to be proper flow field
initialization with a streak or then
finding a good boundary condition that
has some kind of correlations.

The latest idea I've come up with is to
modify the turbulentInlet conditions
to generate time correlations (no spatial)
to the streamwise
boundary velocity using the Ornstein-Uhlenbeck process (see http://qwiki.caltech.edu/wiki/
Simulating_an_Ornstein-Uhlenbeck_Process)
though I haven't tried it so far and I do not
know will this remove the problems;
depends probably on the solver but anyways
it would be a step forward to create some correlations. Btw, does anybody have experience
of doing this type of work?

-Ville
ville is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
MapFields turbulent pipe flow anita OpenFOAM Pre-Processing 5 July 3, 2008 23:29
pipe turbulent flow Hao FLUENT 4 April 29, 2008 22:30
turbulent pipe flow John FLUENT 2 August 2, 2005 13:00
fully developed turbulent flow in a pipe Dipak Phoenics 3 July 20, 2000 05:53
Measurements on turbulent pipe flow Bo B. B. Jensen Main CFD Forum 4 June 30, 1999 05:34


All times are GMT -4. The time now is 16:41.