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

Ive done quite a lot with a Ph
 

Ive done quite a lot with a PhD student; using wavelet and fourier series with UO processes to synthesise inlet conditions; and to use the internal mapping techniques (already implemented in OpenFOAM) to do the same sort of thing. If you email me at

g.r.tabor@ex.ac.uk

I'll send you a couple of papers on our work.

Gavin

Hi Ville Thanks alot Mar
 

Hi Ville

Thanks alot

Marhamat

Hello evrybody Did anybody
 

Hello evrybody

Did anybody simulate turbulent pipe flow or turbulent channel flow in OF using with LES?
I made some effort in this field .But the results aren't correct.
Please explan me your exprience in this field

Best Regards
Marhamat

Hi, I did some experimenting
 

Hi,
I did some experimenting lately and my experience is that making a pipe flow simulation (getting a turbulent flow situation) depends on whether you want to drive the system into turbulent starting
from the boundary layer at the walls takes long
time (which is the physics). If you just want to produce turbulence i.e. for e.g. collecting data for making a boundary
condition then you can try to initialize the velocity field with some function that will develop into turbulent after a while i.e. pretty
soon. If you want to do the former one there
is no way to avoid long simulation times but
if you want to go a quicker way you can try for instance a cyclic square channel with length=6*diameter
and initialize the field properly. You can
try for instance setting the field according to some function in a region in the middle and 0 elsewhere. You can mail me
if you need extra instructions (I'm interested
in the topic as well!)

Regards,
Ville

Dear all and in particular Eug
 

Dear all and in particular Eugene,

I have used perturbCyl with success in OF1.2.
Now I am trying to use it with OF1.3 and I cannot compile it..

Does anyone have a version of perturbCyl for OF1.3?

Thanks

Daniele

Here is a more generalised imp
 

Here is a more generalised implementation for perturbing any ducted flows. I haven't tried it on cylinders though so please let me know if it works ok.

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

You will need entries for dimentsionedVector Ubar and dimensionedScalar Retau in the transportProperties dictionary. The exact value of Retau (shear velocity based Re) is not critical though.

generating 3D mesh for a pipe
 

generating 3D mesh for a pipe LES.

how can we generate a good quality mesh for 3D LES of a pipe flow. I'm familiar with blockMesh. Thanks.

Best regards,
Maka

There's a script released by R
 

There's a script released by Rasmus here:

http://www.cfd-online.com/OpenFOAM_D...es/1/3249.html

Regards,
Alberto

Thanks Alberto. Best Regard
 

Thanks Alberto.

Best Regards,
Maka

Hi all, questions about the u
 

Hi all,
questions about the upper perturbU from Eugene.
what is the wallDistReflexion to define yDir?
it means the wall normal direction (because X is streamwise direction), with the (.n()) ?
cause I also want to use it for a pipe and , I would like to ckeck if we can use this tool for that.

an other question more general, which kind of numerics we can use not to dissip these fluctuations...I afraid that upwind scheme won't work there so ... centred one in OF?

thanks
Cedric

You want to use CD for convect
 

You want to use CD for convection of U (linear).

reflexVec.n() returns the direction from the cell centre to the closest wall.

I rewrote perturbU to be more general, but it is bugged atm so I wont post it.

Hi Eugene, Yes, I plan to sup
 

Hi Eugene,
Yes, I plan to superimpose on my inlet profile a noise to my laminar inlet.
I notice that the initial law in your PerturbU is for channel (Schoppa & Hussain) so I want to test it to my axisymetric geometry.
If it doesn't work, I found other noise like in (Balarac Metais Phy. of Fluids 2005) which seems to be interresting and it was written for a turbulent jet flow.
well, Thanks for the .n(), it will be usefull and I will try to understand your code well now and re-write it for my case.
Thanks for replying,

Cedric

Hi all, I am doing calculatio
 

Hi all,
I am doing calculation with periodic channel which is working well.
Now, I try to do the same thing with a periodic pipe. I use a mesh from Gambit and createPatch to make cyclic boundary condition.
In my calculations, the Courant number and the velocity are still increasing.
I changed my viscosity to reduce the Re but, it is still increasing.
I also change the numerical schemes (to more diffusive) but ... still not working.
My initial field is a turbulent profile, I checked it with paraFoam.
Maybe, the cyclic Patch is the problem but, I'm not sure.
Well, now, I have no more idea. Maybe someone did this calculation before ....Thanks for helping

Regards,
Cedric

Hi Cedric, Maybe I am answ
 

Hi Cedric,

Maybe I am answering too late but anyway...
Which solver are you using?
My suggestion would be, if you have not done it yet,
to run the case with a laminar flow just to make sure the BCs are ok. Then you could shift to a RANS turbulent model to see the impact of the Re.

Hope it helps

Pierre

Hello all would you please
 

Hello all

would you please any one let me know how can i push flow into the pipe in openfoam?
I have created the geometry of the pipe and also the mesh.
I need to see the velocity profile which comes from the moving flow into the pipe.
I am new user of openfoam and i dont know how can i put the amounts for the u velocity and see the motion of the fluid inside the pipe.

I would appreciate any comments.

sorry if it is not an advance question.

Cheers
Armin

Is it normal that perturbU lea
 

Is it normal that perturbU leaves the y component of the laminar flow unaffected ?

Hi John, In perturbU, the y
 

Hi John,

In perturbU, the y component is the wallReflection vectors.
if you look at the code from Eugene or the main article of this method (Schoppa & Hussain, "Coherent structure dynamics in near-wall turbulence", Fluid Dynamics Research, Vol 26, p 119-139, 2000), we only add streaks in two direction; the streamwise and the spanwise perturbation.

Regards,

Cedric

Hi, I've got questions abou
 

Hi,

I've got questions about perturbU parameter to initialise a periodic LES pipe flow.
I'd like to know if someone try to do that. I did a first try with a 10% variation, and perturbations die out, then I encrease to 20% with the same result.
I didn't play with the wave number value yet but if someone succed I'll be greatfull to get his parameters' value.

I know that an other method is to mapFields a previous result but, there is no turbulent pipe flow result avaiable (I think). So, I started from the channel395 (channelOodles tutorial) without any success.
I guess, map field works with i,j,k intercoordinate. My mesh look like Rasmus code one (buterfly mesh) which may not work with mapField (only one fourth of the geometry).
Here again, if someone have tricks, they will be usefull for people, .... and me :o)

Regards,

Cedric

Good morning OpenFOAMers, I
 

Good morning OpenFOAMers,

I over pass the previous problem. Here is the method :
I haven't tryed to use mapfield anymore and I started from a perturbed parabolic profile (perturbU) :o) so, it's longer but, it's working fine.(See pictures, streaks visualized by vorticity)

http://www.cfd-online.com/OpenFOAM_D...ges/1/7553.jpg

If you start directly with a fine mesh, the flow will become laminar and the fluctuations will disappear.
So I started from a coarse mesh, made it turbulent and mapped it into a fine one.

Now, I plan to postprocess the result and I'd like to know if there is a "postChannel" for periodic LES pipe ? or if a postChannel with one periodic direction will be enough ?
If some one has experience of this topic, I'm interesting to that.

Regard,

enjoy this sunny week-end,

Cedric

Hii Ville,

Can you please let me know how did you provide the initial perturbations, like gaussian noise etc? I am looking for such methods as I need to use them for doing LES of rearward facing step.

Thanks,
Tarak