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

question regarding LES of pipe flow - pimpleFoam

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

Like Tree9Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 18, 2014, 04:17
Default
  #21
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27
RodriguezFatz will become famous soon enough
But does it work now, with a correct mesh?

Btw: You need to change p solver to GAMG as I wrote above...
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   November 19, 2014, 01:43
Default
  #22
Member
 
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 12
Dan1788 is on a distinguished road
It still does not work, even with the correct mesh. Thanks for your suggestions nonetheless

Yes I do wall resolved LES. I am not sure about the boundary condition for k at the wall. Conceptually you are right that for a WR LES it needs to be 0. As for the nuSgs I suppose OF requires a nuSGS file in the 0 folder and I dont think the boundary conditions are used.

I am going to try perturbing the flow with turbulence to see how that works out. Have you ever tried that option?

btw, could you upload your pipe case for reference?
Dan1788 is offline   Reply With Quote

Old   November 19, 2014, 04:18
Default
  #23
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27
RodriguezFatz will become famous soon enough
Yes,

here it is.
LES_pipe.tar.gz

Can you upload your mesh somewhere?
One thing: In your first pictures you show a turbulent profile (from one-eq. model), in your last pictures this looks like a laminar profile. Maybe the first was right, but you expect too much turbulence...
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   November 19, 2014, 04:25
Default
  #24
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27
RodriguezFatz will become famous soon enough
Quote:
Originally Posted by Dan1788 View Post
As for the nuSgs I suppose OF requires a nuSGS file in the 0 folder and I dont think the boundary conditions are used.
Yes, I think thats right.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   November 20, 2014, 18:49
Default
  #25
Member
 
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 12
Dan1788 is on a distinguished road
Quote:
Can you upload your mesh somewhere?
One thing: In your first pictures you show a turbulent profile (from one-eq. model), in your last pictures this looks like a laminar profile. Maybe the first was right, but you expect too much turbulence...
Sure, since the mesh is big if you can give me your email or dropbox ID I can send it to you. As for the pictures I think both are laminar flow just that earlier I used paraview and then Tecplot to show the contours. I think there should be an eddy like structure, similar to how your contours look (but corrrect me if I am wrong). Thanks for sharing your case though
Dan1788 is offline   Reply With Quote

Old   November 27, 2014, 04:31
Default
  #26
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27
RodriguezFatz will become famous soon enough
Daniel, I put the case on our server and let it run. I couldn't find any obvious mistake. You still need to wait a bit.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   November 27, 2014, 16:10
Default
  #27
Member
 
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 12
Dan1788 is on a distinguished road
Appreciate your help Philipp :-)

let me know if you happen to find anything.
Dan1788 is offline   Reply With Quote

Old   November 28, 2014, 07:12
Default
  #28
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27
RodriguezFatz will become famous soon enough
Daniel, after struggling that much without any outcome I try something different: I changed the boundary conditions from cyclic to mapped. I also made a thread about cyclic pipes for a different bur similar problem:
http://www.cfd-online.com/Forums/ope...-unstable.html
So, maybe that will work. I can tell you after the weekend
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   December 2, 2014, 03:35
Default
  #29
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27
RodriguezFatz will become famous soon enough
Ok, It doesn't work either. I give up... maybe someone else can help.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   December 3, 2014, 00:26
Default
  #30
Member
 
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 12
Dan1788 is on a distinguished road
Hey,

I think because my reynolds number is less just by solving the equations without initializing turbulence wont help. But thanks for your help anyways. I am now trying to solve the problem by giving turbulence using boxTurb. Let me see how that goes.

Will let you know if I manage to get some good results
Dan1788 is offline   Reply With Quote

Old   January 3, 2015, 14:26
Default
  #31
Member
 
Likun
Join Date: Feb 2013
Posts: 52
Rep Power: 13
Likun is on a distinguished road
Send a message via Skype™ to Likun
Hi Daniel,

Have you solved your problem? I am trying to do LES for a pipe flow, but similar to the results that you shown in your first post of this thread, I don's see any turbulent structure after a very long time. Can you give some hints on the reason and solution for this problem?

Best,
Likun
Likun is offline   Reply With Quote

Old   January 5, 2015, 10:15
Default
  #32
Member
 
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 12
Dan1788 is on a distinguished road
Quote:
Originally Posted by Likun View Post
Hi Daniel,

Have you solved your problem? I am trying to do LES for a pipe flow, but similar to the results that you shown in your first post of this thread, I don's see any turbulent structure after a very long time. Can you give some hints on the reason and solution for this problem?

Best,
Likun
Hi Likun,

I found the solution of this problem by using boxTurb utility in a square duct of the same length as the pipe to generate turbulence. Then mapping the turbulence from the duct to the pipe using the mapFields utility. This will be the initial condition which if you let run would give you turbulent structures in the flowfield.

Let me know if you need any other clarification.
Dan1788 is offline   Reply With Quote

Old   January 6, 2015, 04:30
Default
  #33
Member
 
Likun
Join Date: Feb 2013
Posts: 52
Rep Power: 13
Likun is on a distinguished road
Send a message via Skype™ to Likun
Quote:
Originally Posted by Dan1788 View Post

I found the solution of this problem by using boxTurb utility in a square duct of the same length as the pipe to generate turbulence. Then mapping the turbulence from the duct to the pipe using the mapFields utility. This will be the initial condition which if you let run would give you turbulent structures in the flowfield.

Let me know if you need any other clarification.

Hi Daniel,

Thank you for your reply. I did what you suggested, and now my pipe is turbulent. However, I still have one doubt about the level of perturbation using boxTurb. I first generated a relatively small fluctuation with boxTurb, but then the turbulence was killed after some iterations. However, with a larger perturbation at the beginning (same order of the main velocity component), the turbulence survived. My question is that, does the extent of perturbation at the beginning influences the final results? Do you (or anybody) have any idea on what should be a proper level of perturbation?

Thanks in advance!

Best,
Likun
Likun is offline   Reply With Quote

Old   January 11, 2015, 02:12
Default
  #34
Member
 
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 12
Dan1788 is on a distinguished road
Quote:
Originally Posted by Likun View Post
Hi Daniel,

Thank you for your reply. I did what you suggested, and now my pipe is turbulent. However, I still have one doubt about the level of perturbation using boxTurb. I first generated a relatively small fluctuation with boxTurb, but then the turbulence was killed after some iterations. However, with a larger perturbation at the beginning (same order of the main velocity component), the turbulence survived. My question is that, does the extent of perturbation at the beginning influences the final results? Do you (or anybody) have any idea on what should be a proper level of perturbation?

Thanks in advance!

Best,
Likun
Hi Likun,

I am not entirely sure how the extent of perturbation affects the results because I havent really done a parametric study. Usually I have always taken the perturbation to be approximately 10% of the bulk velocity which is known. Hope that helps!
Dan1788 is offline   Reply With Quote

Old   January 12, 2015, 15:51
Default
  #35
Member
 
Likun
Join Date: Feb 2013
Posts: 52
Rep Power: 13
Likun is on a distinguished road
Send a message via Skype™ to Likun
Dear Daniel,

Thank you for your reply. I think the initial perturbation should not influence the final results as long as the perturbation is enough to trigger turbulence. I simulated to pipe flow over a long time. The resolved kinetic energy seems does not change much over time. So, I think this should be converged.

Best,
Likun
Likun is offline   Reply With Quote

Old   December 14, 2016, 05:34
Default streamwise or spanwise vortices
  #36
New Member
 
Nitin
Join Date: Mar 2012
Location: Bombay
Posts: 16
Rep Power: 14
Nitin Minocha is on a distinguished road
Dear Daniel
I am doing DNS channel flow in openfoam. I am unable to found streamwise or spanwise vortices even after 8000s. I would like to know how you solve your problem.
Nitin Minocha is offline   Reply With Quote

Old   December 24, 2017, 10:26
Default Hi
  #37
gu1
Senior Member
 
Guilherme
Join Date: Apr 2017
Posts: 245
Rep Power: 10
gu1 is on a distinguished road
Quote:
Originally Posted by RodriguezFatz View Post
This is a picture of a pipe flow just as you do, but with higher Re and wall modeled LES. It was initialized without any turbulence.
Attachment 34955

This is a picture of the kinetic energy (perpendicular to the main flow) to track the convergence of the case. You see, it is not fully converged after 40000 time steps. This means after 1.6s or about 100 flow through times. Of course, this is due to very bad initial guess, but you see, this can take some time.
Attachment 34956

I track the energy by putting this in my controlDict:
Code:
functions
(
AverageResolvedKineticEnergyVxVy
    {
        type swakExpression;
        valueType cellZone;
        zoneName FLUID;
        accumulations (
            average
        );
        expression "U.x*U.x + U.y*U.y";
        verbose true;
    }
);
I only use Ux and Uy for tracking, because I only want to track the kinetic energy of the turbulent structures and Uz is my flow direction. I was too lazy to calculate the average Uz at each point. So this is a fast and good work around.
Could you teach me how to calcukou the magU in paraview?
gu1 is offline   Reply With Quote

Old   December 26, 2017, 15:42
Default
  #38
Member
 
Arnout
Join Date: Nov 2010
Posts: 46
Rep Power: 16
The King is on a distinguished road
Quote:
Originally Posted by gu1 View Post
Could you teach me how to calcukou the magU in paraview?


Paraview is showing the magnitude of the velocity if you have a new enough version.
The King is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Issues on the simulation of high-speed compressible flow within turbomachinery dowlee OpenFOAM Running, Solving & CFD 11 August 6, 2021 07:40
setup problems - LES pipe flow with cyclic BC (1) and direct mapped inlet (2) florian_krause OpenFOAM 22 June 13, 2013 22:25
Pipe flow with pressure-inlet lummz FLUENT 3 October 13, 2012 14:29
Question regarding Fluent's Turbulent Pipe Flow Problem clueless Main CFD Forum 0 May 15, 2009 04:59
Question regarding Fluent's Turbulent Pipe Flow Problem clueless FLUENT 0 May 15, 2009 04:33


All times are GMT -4. The time now is 19:22.