CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Periodic Pipe Flow LES (https://www.cfd-online.com/Forums/cfx/94603-periodic-pipe-flow-les.html)

 dvolkind November 21, 2011 02:20

Periodic Pipe Flow LES

5 Attachment(s)
Dear all!
I need some advice on modeling a fully developed pipe flow with periodic boundary conditions using LES.
My goal is to get a realistic transient inlet BC for my problem. That's how I'm trying to achieve this:
1. Consider a circular pipe (5*D long) with periodic BCs (mass flow rate).
2. Obtain a steady state solution with RANS (I used SST).
3. Run LES using the RANS solution as initial conditions.
4. Import transient boundary profile as an inlet BC for the LES of my actual problem.
I'm using a hexa-mesh with Y+ at wall around 1, growth ratio around 1,1. Re = 8400, Courant number < 1.
The major problem is that I can't get a converged (judged by residuals) solution with periodic BCs both in transient and steady state. When I run the same model with mass flow inlet and pressure outlet it does converge, but the velocity profile looks unphysical. The other problem is that the flow pattern doesn't become turbulent, even if I add significant velocity fluctuations for the initial velocity field, they tend to damping. So, I would like to ask the following:
1. What are the possible reasons of convergence problems?
2. Probably different convergence criteria should be used with periodic BCs?
3. What kind of grid is better for LES? As far as I know it should be as uniform as possible and have aspect ratios around 1. But what type of mesh is more preferable - tetra or hexa? And why? CFX Reference Guide says it should be isotropic, so tetra is better (4.1.11.4.2. Meshing). I've also seen a post by Mr. Horrocks, where he recommended to use hexa. When I use a tetrahedral mesh with approximately the same sizes I get the same results.
4. What is the reason of the turbulence damping?
Attachment 10158
Residuals plot for transient:
Attachment 10159
Velocity profile with mass flow inlet and pressure outlet:
Attachment 10160
Velocity profile with periodic BCs with specified mass flow rate:
Attachment 10161
Mesh:
Attachment 10162
Thanks to everyone in advance! Any help will be greatly appreciated.

 ghorrocks November 21, 2011 06:02

Quote:
 What are the possible reasons of convergence problems?
This FAQ is not exactly on your topic but is related and should give you some tips. http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Quote:
 Probably different convergence criteria should be used with periodic BCs?
Your approach sounds good. I do not think your problem is with the periodic BCs.

Quote:
 What kind of grid is better for LES?
A high quality hex grid is superior, but if the geometry is difficult and you cannot do a hex grid (or only a low quality one) then a tet grid is superior. If you have a cylinder then you should be able to do a good hex grid.

High quality grids have less numerical dissipation, converge easier, use less memory (for hex grids) and can handle aspect ratio changes better.

Your comment about not getting turbulent structures confirms you have too much dissipation, so this is a problem for you. You will need central differencing and second order time differencing.

 dvolkind November 23, 2011 13:34

Hello, Glenn!
Thanks a lot for your answers! I'm now trying to get the steady state problem converged. To do this I started with agressive physical time scale, then I switched to local timescale factor, and it does converge that way (incredibly slowly though). The text on the link you gave me says not to run with local timescale all the way to convergence. So I switch back to physical time scale, and all important residuals and imbalances (characterizing flow-aligned coordinate) begin to oscillate. And, if you don't mind, I would like to ask some more questions:
1. Is it necessary to get the final convergence without local time scale factor and why?
2. If it is, how to determine how many iterations are sufficient?
3. Will it be possible to reduce the amplitude of residuals/imbalances oscillations on the final iterations with physical timescale if I achive tighter convergence with local time scale factor? (I surely can try it myself, but it takes really long with my available hardware)
4. Probably I still go wrong somewhere? (convergence seems too tough for such a primitve steady-state problem)
5. Concerning LES: how else could I avoid dissipation you mentioned if I was already using central differencing / Euler second order backward and a "structured" hexa mesh?

Thank you again! Sorry for asking too much.

 ghorrocks November 23, 2011 19:51

1) Yes, there has been some posts on this on the forum, search for them.
2) Not sure. I would suggest until things settle out. To be completely sure do a sensitivity analysis.
3) Possibly. But if the oscillations are physical then it will not make a difference.
4) You will need quite a large physical time step for this to work. Also be careful about making your mesh too fine for the RANS model.
5) Then you have done the main things. There are also some other options to consider regarding the detailed numerical approach such as Rhie-Chow and interpolation schemes (and others).

 dvolkind November 24, 2011 00:03

 ghorrocks November 24, 2011 07:04

Oh yes, and I forgot the main way to reduce dissipation - finer mesh and smaller time steps.

 dvolkind January 10, 2017 05:58

Hello, guys!

1) To obtain LES-like content in a globally stable flow, an artificial turbulence synthesizer is required. It's available both in Fluent and CFX, however, the implementation is slightly different.

2) Whoever interested in the problem setup, be sure to check this manual by Dr. Menter from ANSYS. I don't have the 2.0 version, but in 1.02 they suggested to use WMLES for channel flow. I think, that DDES and SLES/SBES (new at R17) are also worth trying.

3) I should also note, that I haven't been able to obtain converged monitors in CFX with periodic boundary conditions applied to a straight channel (and I'm not the only one). However, if the channel has variable cross-section (i.e. not only skin friction, but also acceleration/deceleration affects pressure loss), it works fine. Fluent's implementation works in all cases, so I prefer it for periodic problems.

4) Some years ago I've compared different turbulence models in Fluent (steady periodic RANS circular pipe flow) against Blasius's solution for pressure drop and various laws (2 and 3-layer von Karman, power law 1/6 and 1/7) for velocity profile. According to my comparison, Spalart-Allmaras and RSM Stress-Omega yield best results. I can e-mail my results and a project to demonstrate the problem setup.

With kind regards,
Dmitry

 All times are GMT -4. The time now is 13:24.