Dear all, I would like to m
 

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?

Try this http://www.cfd-on
 

Try this

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif 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.

Thanks very much Eugene, do y
 

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

Hi Daniele, I would like to
 

Hi Daniele,

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

Greetings!
Fabian

Hi Fabian, I am using cylcic
 

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

Schoppa & Hussain, "Coherent s
 

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.

Dear all, I have a question
 

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

Hi Daniele, thanks! Does an
 

Hi Daniele,

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

Greetings!
Fabian

turbulentInlet is useful but n
 

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

I was infact thinking to make
 

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

Dear all, could anybody giv
 

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

Heya, Look for the paper:
 

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

Hi everyone I used oodles
 

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

Hi everyone I add that: Re
 

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

Hi everyone I wan't to implem
 

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

Hi everyone I wan't to implem
 

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

Hi everyone As i explained be
 

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.
http://www.cfd-online.com/OpenFOAM_D...your_image.gif
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

Hi everyone As i explained be
 

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.
http://www.cfd-online.com/OpenFOAM_D...ges/1/3782.jpg
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

Sorry for duplicate sending an
 

Sorry for duplicate sending and for Q1
Marhamat

Hi Marhamat! I've been trying
 

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