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   February 6, 2007, 10:49
Default Ive done quite a lot with a Ph
  #21
Senior Member
 
Gavin Tabor
Join Date: Mar 2009
Posts: 181
Rep Power: 8
grtabor is on a distinguished road
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
grtabor is offline   Reply With Quote

Old   February 7, 2007, 07:59
Default Hi Ville Thanks alot Mar
  #22
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hi Ville

Thanks alot

Marhamat
marhamat is offline   Reply With Quote

Old   February 25, 2007, 07:41
Default Hello evrybody Did anybody
  #23
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
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
marhamat is offline   Reply With Quote

Old   February 26, 2007, 07:50
Default Hi, I did some experimenting
  #24
Member
 
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 8
ville is on a distinguished road
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
ville is offline   Reply With Quote

Old   March 1, 2007, 14:39
Default Dear all and in particular Eug
  #25
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
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
panara is offline   Reply With Quote

Old   March 2, 2007, 06:29
Default Here is a more generalised imp
  #26
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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.

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.
eugene is offline   Reply With Quote

Old   April 2, 2007, 13:16
Default generating 3D mesh for a pipe
  #27
Senior Member
 
Maka Mohu
Join Date: Mar 2009
Posts: 305
Rep Power: 9
maka is on a distinguished road
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
maka is offline   Reply With Quote

Old   April 2, 2007, 14:37
Default There's a script released by R
  #28
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
There's a script released by Rasmus here:

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

Regards,
Alberto
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   April 3, 2007, 10:13
Default Thanks Alberto. Best Regard
  #29
Senior Member
 
Maka Mohu
Join Date: Mar 2009
Posts: 305
Rep Power: 9
maka is on a distinguished road
Thanks Alberto.

Best Regards,
Maka
maka is offline   Reply With Quote

Old   July 5, 2007, 05:17
Default Hi all, questions about the u
  #30
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
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
cedric_duprat is offline   Reply With Quote

Old   July 9, 2007, 08:18
Default You want to use CD for convect
  #31
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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.
eugene is offline   Reply With Quote

Old   July 9, 2007, 09:50
Default Hi Eugene, Yes, I plan to sup
  #32
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
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
cedric_duprat is offline   Reply With Quote

Old   October 4, 2007, 09:15
Default Hi all, I am doing calculatio
  #33
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
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
cedric_duprat is offline   Reply With Quote

Old   October 9, 2007, 23:31
Default Hi Cedric, Maybe I am answ
  #34
pvc
Guest
 
Posts: n/a
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
  Reply With Quote

Old   November 26, 2007, 00:50
Default Hello all would you please
  #35
New Member
 
Armin Hosseinian
Join Date: Mar 2009
Location: Perth, Western Australia, Australia
Posts: 17
Rep Power: 8
armin_h is on a distinguished road
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
armin_h is offline   Reply With Quote

Old   January 8, 2008, 05:07
Default Is it normal that perturbU lea
  #36
Senior Member
 
John Deas
Join Date: Mar 2009
Posts: 160
Rep Power: 8
johndeas is on a distinguished road
Is it normal that perturbU leaves the y component of the laminar flow unaffected ?
johndeas is offline   Reply With Quote

Old   January 8, 2008, 05:20
Default Hi John, In perturbU, the y
  #37
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
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
cedric_duprat is offline   Reply With Quote

Old   February 25, 2008, 11:06
Default Hi, I've got questions abou
  #38
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
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
cedric_duprat is offline   Reply With Quote

Old   May 4, 2008, 06:40
Default Good morning OpenFOAMers, I
  #39
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
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)



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
songwukong and mgg like this.
cedric_duprat is offline   Reply With Quote

Old   June 23, 2011, 18:45
Default
  #40
Senior Member
 
Tarak
Join Date: Aug 2010
Location: State College, PA
Posts: 105
Rep Power: 7
Tarak is on a distinguished road
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
Tarak 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 07:06.