CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Periodic Pipe Flow LES

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

Like Tree1Likes
  • 1 Post By dvolkind

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 21, 2011, 01:20
Default Periodic Pipe Flow LES
  #1
Member
 
Dmitry Volkind
Join Date: Jan 2010
Location: Ekaterinburg, Russia
Posts: 64
Rep Power: 13
dvolkind is on a distinguished road
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?
Residuals plot for steady state:
steady.jpg
Residuals plot for transient:
transient.jpg
Velocity profile with mass flow inlet and pressure outlet:
Profile_Inlet&Outlet.jpg
Velocity profile with periodic BCs with specified mass flow rate:
Profile_Periodic.jpg
Mesh:
mesh.jpg
Thanks to everyone in advance! Any help will be greatly appreciated.
dvolkind is offline   Reply With Quote

Old   November 21, 2011, 05:02
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,643
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   November 23, 2011, 12:34
Default
  #3
Member
 
Dmitry Volkind
Join Date: Jan 2010
Location: Ekaterinburg, Russia
Posts: 64
Rep Power: 13
dvolkind is on a distinguished road
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.
dvolkind is offline   Reply With Quote

Old   November 23, 2011, 18:51
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,643
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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).
ghorrocks is offline   Reply With Quote

Old   November 23, 2011, 23:03
Default
  #5
Member
 
Dmitry Volkind
Join Date: Jan 2010
Location: Ekaterinburg, Russia
Posts: 64
Rep Power: 13
dvolkind is on a distinguished road
Thank yor for your answers!
dvolkind is offline   Reply With Quote

Old   November 24, 2011, 06:04
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,643
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Oh yes, and I forgot the main way to reduce dissipation - finer mesh and smaller time steps.
ghorrocks is offline   Reply With Quote

Old   January 10, 2017, 04:58
Default
  #7
Member
 
Dmitry Volkind
Join Date: Jan 2010
Location: Ekaterinburg, Russia
Posts: 64
Rep Power: 13
dvolkind is on a distinguished road
Hello, guys!

It's been several years since my last post, but I've been asked about this problem privately. So I decided to add some comments here in case someone else is interested.

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
fresty likes this.
dvolkind is offline   Reply With Quote

Old   March 20, 2020, 12:44
Default
  #8
New Member
 
Matt Campbell
Join Date: Apr 2015
Posts: 6
Rep Power: 7
mcampbell is on a distinguished road
I am working on LES periodic pipe flows and came across this. First, from my understanding, using translational Periodic BC, there is no 'inlet' or 'outlet' and specifying a profile will cause periodic cycling in the solution. The whole point is to let the solution develop without inlet conditions (which is difficult to get right for LES). The periodic condition 'ties' the outlet and inlet together numerically so flow structures and turbulent eddies persist over the boundary (you can show a large persistent structure move through the domain repeatedly.) Secondly, we have had a difficult time getting the 'right' solution for wall bounded LES in Fluent. Our assumption is that for fully developed pipe flow all turbulence originates at the wall (or rather due to the velocity gradients). If you look at the scales adequately the 'large' energy containing eddies approach the kolomogrov scale near the wall but quickly scale larger as you move away. This essentially results in a DNS at Y+<10 with a heavily adapting mesh to a well resolved LES (90%) by y+=100. Finally, we have struggled to get consistently good results and believe wall bounded LES is a relatively open topic in the CFD community (as opposed to many external flows like free shear and jets). I welcome anyone with experience to comment, correct or clarify any of this!
mcampbell is offline   Reply With Quote

Old   March 21, 2020, 05:30
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,643
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
A periodic inlet/outlet is one approach, but it is still not perfect as it introduces a frequency into the simulation of the fluid residence time, and the length of your domain sets that frequency. Obviously this can be minimised by making the domain long enough that the residence time frequency is easily separated from the LES frequencies. And secondly, you still have to drive the flow somehow, and that is normally done by a source term in the periodic inlet/outlet approach, and this source term is not physically accurate either.

If you are struggling to get good results in LES that is not surprising. It requires large computing power and carefully developed CFD solvers with very low dissipation to work. You have to be very careful in doing accurate LES with commercial solvers, getting the dissipation low enough is challenging.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Tags
convergence, les, periodic bc

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
setup problems - LES pipe flow with cyclic BC (1) and direct mapped inlet (2) florian_krause OpenFOAM 22 June 13, 2013 21:25
flow in perforated pipe distributor pertupd ANSYS 0 August 12, 2009 08:36
Reverse Flow at Rotating Pipe Outlet vismech STAR-CCM+ 1 August 11, 2009 10:38
About Turbulence Intensity (Pipe flow assimilated) gRomK13 Main CFD Forum 1 July 10, 2009 03:11
Hydrostatic pressure in 2-phase flow modeling (CFX4.2) HB &DS CFX 0 January 9, 2000 13:19


All times are GMT -4. The time now is 03:03.