|
[Sponsors] |
August 24, 2006, 12:45 |
Dear all,
I would like to m
|
#1 |
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 17 |
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? |
|
August 24, 2006, 13:36 |
Try this
http://www.cfd-on
|
#2 |
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 |
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. |
|
August 25, 2006, 02:13 |
Thanks very much Eugene,
do y
|
#3 |
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 17 |
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 |
|
August 25, 2006, 04:27 |
Hi Daniele,
I would like to
|
#4 |
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 19 |
Hi Daniele,
I would like to know, what kind of inlet you use; especially, how do create turbulence at the inlet? Greetings! Fabian |
|
August 25, 2006, 04:36 |
Hi Fabian,
I am using cylcic
|
#5 |
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 17 |
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 |
|
August 25, 2006, 05:32 |
Schoppa & Hussain, "Coherent s
|
#6 |
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 |
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. |
|
August 27, 2006, 15:45 |
Dear all,
I have a question
|
#7 |
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 17 |
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 |
|
August 28, 2006, 01:53 |
Hi Daniele,
thanks! Does an
|
#8 |
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 19 |
Hi Daniele,
thanks! Does anybody know, if the turbulent inlet is useful for LES? Greetings! Fabian |
|
August 28, 2006, 02:25 |
turbulentInlet is useful but n
|
#9 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,906
Rep Power: 33 |
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
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
August 28, 2006, 03:04 |
I was infact thinking to make
|
#10 |
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 17 |
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 |
|
August 31, 2006, 06:28 |
Dear all,
could anybody giv
|
#11 |
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 17 |
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 |
|
September 1, 2006, 04:43 |
Heya,
Look for the paper:
|
#12 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,906
Rep Power: 33 |
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
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
November 22, 2006, 07:39 |
Hi everyone
I used oodles
|
#13 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
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¶meter changing in pitzDaily. Please help me. regards marhamat |
|
November 23, 2006, 18:03 |
Hi everyone
I add that:
Re
|
#14 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
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 |
|
December 25, 2006, 02:47 |
Hi everyone
I wan't to implem
|
#15 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
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 |
|
December 25, 2006, 02:56 |
Hi everyone
I wan't to implem
|
#16 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
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 |
|
February 6, 2007, 07:50 |
Hi everyone
As i explained be
|
#17 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
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 |
|
February 6, 2007, 08:17 |
Hi everyone
As i explained be
|
#18 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
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 |
|
February 6, 2007, 08:36 |
Sorry for duplicate sending an
|
#19 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
Sorry for duplicate sending and for Q1
Marhamat |
|
February 6, 2007, 09:27 |
Hi Marhamat!
I've been trying
|
#20 |
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 17 |
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 |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
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 |