Large Eddy Simulation of turbulent channel flow

daroz · March 14, 2017, 12:41

I am trying to reproduce the well known turbulent channel flow simulation of Kim, Moin and Moser (1987) where they provide a DNS solution of the problem.

In my case, I am trying approach the problem with the available LES in ANSYS Fluent R.17.2. I am using Smagorinsky-Lilly (Dynamic Stresses) for the SGS modelling and periodic conditions in both stream and spanwise directions. The flow is driven by a constant mass flow rate.

The problem is that I am getting a laminarized solution after several flowthrough times. I have tryied to use RANS and URANS solutions as initital flow fields as well as a perturbated field via an UDF.

The space and time discretization requirements are being fullfiled, at least I guess they are (CFL < 1, y+ < 1, etc)...

Does anyone have any idea of what I am doing wrong or have experienced the same problem?

Thank you.

qianquan · March 30, 2017, 13:23

recently i do circle cylinder flow with les , smagorinsky-lily (dynamic), re=140000, boundry layers are 40. at first, using ke turbulent model with steady , when it converged, tap 'solve/initialize/init-instantaneous-vel' in GUI , and then switch to les , spatial discretion is bound central differing , max cfl around 2, the results looks ok

Sent from my iPhone using CFD Online Forum mobile app

sbaffini · March 30, 2017, 14:23

The plane channel flow is quite tough to get started, especially if your discretization is adding dissipation (yes, the bounded central scheme might still be too much diffusive). Also, the spectral synthesizer as implemented in Fluent is not the best tool out there. It all depends from the scale at which energy is supplied in your turbulent velocity field. In plane channel this happens to be very small and numerics dominated. For the cylinder it is much more large and manageable in Fluent.

Long story short, check out my initialization routine here:

https://www.cfd-online.com/Forums/bl...nt-part-1.html

and use the unbounded central scheme at least for the first few hundred iterations. Obviously, I assume that everything else is ok with your setup.

daroz · March 30, 2017, 15:18

Thank you for the support!

I have handled the simulation of the plane channel flow since the post.

I've used a steady solution obtained with the SST model as initial field.

I am trying to employ the same methodology for the turbulent duct flow. I will let you know if I succeeded.

Thank you "sbaffini" for the routines you provided. I am sure they will be very useful.

LuckyTran · March 30, 2017, 16:06

I never encountered consistent relaminarization, but I also do not typically use the bounded schemes. I.e. I used second order Euler and not bounded second order, and plain central instead of bounded central.

For me the problem was the initial perturbation. It could be reasonably turbulent for a few flow through times but because of the streamwise periodic BC, it relaminarizes after say 3 or 4 flow-thru times (but not 1 because it takes a flow-thru to recycle the initial flow). However, this was entirely my fault because I gave a bad initial perturbation. For example uniform random perturbations everywhere had a tendency to relaminarize. Sometimes I messed up my script and put perturbations on only the upper-half of the channel. An interesting flow develops which is turbulent on the upper side but laminar on the lower side!

I haven't tried the "solve/initialize/ init-instantaneous-vel" option in Fluent for channel flow, but I would think that it should work reasonably well. Unfortunately, this option requires you to have a current RANS solution so that you cannot re-do the perturbations in the middle of your LES run.

So yeah, maybe the solution is to give a good perturbation and run with unbounded schemes.

daroz · March 30, 2017, 17:38

I haven't encountered any problem in obtaining the RANS solution. Actually it reaches convergence very quickly.

The only things I have changed from the time I was having problems is that I reduced the time-step and switched the pressure-velocity coupling to the COUPLED method. I am still using bounded central differencing for momentum but in the next time I will follow the advises and use an unbounded scheme for the first few hundred iterations.

March 14, 2017, 12:41	Large Eddy Simulation of turbulent channel flow	#1
daroz New Member Join Date: Mar 2011 Posts: 8 Rep Power: 15	I am trying to reproduce the well known turbulent channel flow simulation of Kim, Moin and Moser (1987) where they provide a DNS solution of the problem. In my case, I am trying approach the problem with the available LES in ANSYS Fluent R.17.2. I am using Smagorinsky-Lilly (Dynamic Stresses) for the SGS modelling and periodic conditions in both stream and spanwise directions. The flow is driven by a constant mass flow rate. The problem is that I am getting a laminarized solution after several flowthrough times. I have tryied to use RANS and URANS solutions as initital flow fields as well as a perturbated field via an UDF. The space and time discretization requirements are being fullfiled, at least I guess they are (CFL < 1, y+ < 1, etc)... Does anyone have any idea of what I am doing wrong or have experienced the same problem? Thank you.

March 30, 2017, 15:18		#4
daroz New Member Join Date: Mar 2011 Posts: 8 Rep Power: 15	Thank you for the support! I have handled the simulation of the plane channel flow since the post. I've used a steady solution obtained with the SST model as initial field. I am trying to employ the same methodology for the turbulent duct flow. I will let you know if I succeeded. Thank you "sbaffini" for the routines you provided. I am sure they will be very useful. sbaffini likes this.

March 30, 2017, 16:06		#5
LuckyTran Senior Member Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,761 Rep Power: 66	I never encountered consistent relaminarization, but I also do not typically use the bounded schemes. I.e. I used second order Euler and not bounded second order, and plain central instead of bounded central. For me the problem was the initial perturbation. It could be reasonably turbulent for a few flow through times but because of the streamwise periodic BC, it relaminarizes after say 3 or 4 flow-thru times (but not 1 because it takes a flow-thru to recycle the initial flow). However, this was entirely my fault because I gave a bad initial perturbation. For example uniform random perturbations everywhere had a tendency to relaminarize. Sometimes I messed up my script and put perturbations on only the upper-half of the channel. An interesting flow develops which is turbulent on the upper side but laminar on the lower side! I haven't tried the "solve/initialize/ init-instantaneous-vel" option in Fluent for channel flow, but I would think that it should work reasonably well. Unfortunately, this option requires you to have a current RANS solution so that you cannot re-do the perturbations in the middle of your LES run. So yeah, maybe the solution is to give a good perturbation and run with unbounded schemes. Last edited by LuckyTran; March 30, 2017 at 19:47.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
About Some Concepts:Laminar flow, turbulent flow, steady flow and time-dependent flow	Jing	Main CFD Forum	8	October 5, 2018 18:02
Velocity profile is not turbulent (OPEN CHANNEL FLOW)	roi247	FLUENT	2	March 15, 2017 08:30
Accuracy of LRR and SSG in turbulent channel flow	dradenkovic	OpenFOAM Running, Solving & CFD	1	August 23, 2016 14:03
LES database for turbulent channel flow at Re_tau=590	sbaffini	Main CFD Forum	10	May 27, 2014 11:55
a symposium about large eddy simulation	dictatore_bozorg	FLUENT	1	April 29, 2012 11:47

March 30, 2017, 13:23		#2
qianquan New Member 钱权 Join Date: Mar 2017 Posts: 5 Rep Power: 9	recently i do circle cylinder flow with les , smagorinsky-lily (dynamic), re=140000, boundry layers are 40. at first, using ke turbulent model with steady , when it converged, tap 'solve/initialize/init-instantaneous-vel' in GUI , and then switch to les , spatial discretion is bound central differing , max cfl around 2, the results looks ok Sent from my iPhone using CFD Online Forum mobile app

March 30, 2017, 14:23		#3
sbaffini Senior Member Paolo Lampitella Join Date: Mar 2009 Location: Italy Posts: 2,195 Blog Entries: 29 Rep Power: 39	The plane channel flow is quite tough to get started, especially if your discretization is adding dissipation (yes, the bounded central scheme might still be too much diffusive). Also, the spectral synthesizer as implemented in Fluent is not the best tool out there. It all depends from the scale at which energy is supplied in your turbulent velocity field. In plane channel this happens to be very small and numerics dominated. For the cylinder it is much more large and manageable in Fluent. Long story short, check out my initialization routine here: https://www.cfd-online.com/Forums/bl...nt-part-1.html and use the unbounded central scheme at least for the first few hundred iterations. Obviously, I assume that everything else is ok with your setup.

March 30, 2017, 17:38		#6
daroz New Member Join Date: Mar 2011 Posts: 8 Rep Power: 15	I haven't encountered any problem in obtaining the RANS solution. Actually it reaches convergence very quickly. The only things I have changed from the time I was having problems is that I reduced the time-step and switched the pressure-velocity coupling to the COUPLED method. I am still using bounded central differencing for momentum but in the next time I will follow the advises and use an unbounded scheme for the first few hundred iterations.