[RodriguezFatz]

But does it work now, with a correct mesh?

Btw: You need to change p solver to GAMG as I wrote above...

[Dan1788]

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?

[RodriguezFatz]

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...

[RodriguezFatz]

Originally Posted by Dan1788

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.

[Dan1788]

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

[RodriguezFatz]

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.

[Dan1788]

Appreciate your help Philipp :-)

let me know if you happen to find anything.

[RodriguezFatz]

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

[RodriguezFatz]

Ok, It doesn't work either. I give up... maybe someone else can help.

[Dan1788]

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

[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

[Dan1788]

Originally Posted by 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

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.

[Likun]

Originally Posted by Dan1788

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

[Dan1788]

Originally Posted by Likun

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!

[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

[Nitin Minocha]

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.

[gu1]

Originally Posted by RodriguezFatz

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:

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?

[The King]

Originally Posted by gu1

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.