[kuwt]

Hello openfoam community,



I am trying to run a LES for a circular pipe flow problem. The problem is, I cannot observe any vortices as I would expect from a LES model, which is supposed to resolve all of the largest scale vortices.


The program is simulated to 2s and the time step is taken to be 1e-5s. The pipe is 2m long and 0.028m in radius. The cell size is around 0.001m. The kinematic viscosity is 1x10^-5 m^2s^{-1}, which corresponds to air at 20 deg Celcius. The boundary condition is a fixed velocity inlet of 15ms^-1. Zero gradient pressure outlet. No slip pipewall. This gives a Reynolds number = 84000, which is obviously the turbulence flow regime.



Smagorinsky model is used as the turbulence model, while nutUSpaldingWallFunction is used for the pipewall for nut.

[kuwt]

I am using pisoFoam. The cross section of the grid can be seen in crosssection.png. Prior to Les simulation, I have run ANS simulation. The integral length scale is k^(1.5)/epsilon = from 0.004 to 0.026m. My grid size is 0.001m so it is much smaller than the integral length scale and should be able to capture the vortices.


The complete case is attached as les_case.tar.gz

[Tobermory]

Well, you are feeding in laminar flow at the inlet (fixedValue velocity boundary condition) and are watching this advect down the pipe a distance of 35 diameters. Seems like the results are pretty realistic.

If you want turbulent pipe flow, and assuming that you are not interested in modelling the transition process (which either takes many many diameters to occur and some careful wall treatment, or needs some kind of artificial trip to kick start it ... and then many diameters of length to stabilise), then you need to inject turbulent flow at the upstream inlet.

In other words, it's rather more complex than you were expecting I am afraid. My suggestion is to think again about your boundary conditions and read up on modelling eg channel flows.

[kuwt]

Originally Posted by Tobermory

Well, you are feeding in laminar flow at the inlet (fixedValue velocity boundary condition) and are watching this advect down the pipe a distance of 35 diameters. Seems like the results are pretty realistic.

If you want turbulent pipe flow, and assuming that you are not interested in modelling the transition process (which either takes many many diameters to occur and some careful wall treatment, or needs some kind of artificial trip to kick start it ... and then many diameters of length to stabilise), then you need to inject turbulent flow at the upstream inlet.

In other words, it's rather more complex than you were expecting I am afraid. My suggestion is to think again about your boundary conditions and read up on modelling eg channel flows.

Thank you for the answer. Can you give me some more hint?

If I stay with my current geometry, I found that I can try turbulentInlet and the mapped boundary condition. I am still looking into the mapped boundary condition. But since the turbulentInlet looks easier, I will try this option first.

When I want to model the transitional flow, how many diameter do you suggest? From page 3 of this note https://innovationspace.ansys.com/co...es-Handout.pdf, it says the entrance length can be given by L/D ~4.4 *Re^(1/6), for my case Re~80000, L/D~29, so it looks like my 35 diameter is enough if that note is correct. Vortices should appear at the outlet region. I plan to double my pipe length to see what the result is. In addition, you said careful wall treatment, do you mean i need y+ to be around 1 or is it more complicated than I think?

[Tobermory]

Laminar - turbulent transition is a complex phenomenon, and is not easy to reproduce with a standard turbulence model and without much more refinement at the wall etc.

If you are only interested in the turbulent flow post-transition, then my first bit of advice is to avoid trying to model it directly. Instead I would recommend looking at one or more of the following approaches:
- use a numerical trip to kick start the transition (google perturbU for channel flow and the thesis by deVilliers for more info)
- consider cyclic inlet/outlet boundary conditions, with a streasmwise dPdX force, to shorten your domain
- or use a pseudo-turbulent inlet boundary condition at the upstream end - this will generate pseduo 3D turbulence that will seed the flow and will, given enough downstream distance, become a properly turbulent field downstream

Finally - just be aware - what you are trying to model is not trivial ... it may take some months to get right, unless someone has a ready made case that they can offer you. Good luck.