
[Sponsors] 
January 11, 2012, 05:47 
LES in DES can't be actived!

#1 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 6 
Hello everybody!
I'm modeling the junction flow, that is, flow past a wing mounted on a plate. I use DES model in ansys CFX12. I'm sure the mesh is good and y+ is near 1. The transient calculation was initialized from a SST RANS result file. But until to 4000 timesteps, I found that LES hasn't been actived anywhere of the whole flowfiled because the blending function for DES is equal to 1 everywhere! The monitored variables also converged to steady values, which also indicated that only RANS is adopted all over the flowfield. I can't find why LES can't be actived in this DES simulation. I will be appreciate it very much for your help. 

January 11, 2012, 06:50 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Are you sure you are in a flow regime where you get LES style turbulent structures?


January 11, 2012, 10:39 

#3 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 6 

January 11, 2012, 11:47 

#4 
Senior Member
Join Date: Apr 2009
Posts: 532
Rep Power: 13 
Perhaps you need some inlet fluctuations to trigger the turbulence generation.


January 11, 2012, 23:06 

#5  
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 6 
Quote:
However, the two ways both seemed to fail because after several timesteps I checked the blending function for DES in CFDpost and found that it is still equal to 1 all over the flowfield. 

January 12, 2012, 05:34 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Can you post your CCL file and an image of the geometry?


January 12, 2012, 06:35 

#7 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 6 
The picture of the model:
junction flow.jpg 

January 12, 2012, 06:37 

#8 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 6 
# State file created: 2012/01/12 18:31:40
# CFX12.0.1 build 2009.04.1423.02 LIBRARY: CEL: FUNCTION: Inlet Porfile Argument Units = [m] Extend Max = true Extend Min = true File Name = K:\LEfillet3\ROOD\computation\Inlet \ Profile\inlet_profile_forCFX.csv Option = Profile Data Spatial Fields = y DATA FIELD: Turbulence Eddy Dissipation Field Name = Turbulence Eddy Dissipation Parameter List = Epsilon Result Units = [m^2 s^3] END DATA FIELD: Turbulence Kinetic Energy Field Name = Turbulence Kinetic Energy Parameter List = k Result Units = [m^2 s^2] END DATA FIELD: Velocity u Field Name = Velocity u Parameter List = U,Velocity r Component,Wall U,Wall Velocity r \ Component Result Units = [m s^1] END END END FLOW: Flow Analysis 1 SOLUTION UNITS: Angle Units = [rad] Length Units = [m] Mass Units = [kg] Solid Angle Units = [sr] Temperature Units = [K] Time Units = [s] END ANALYSIS TYPE: Option = Transient EXTERNAL SOLVER COUPLING: Option = None END INITIAL TIME: Option = Automatic with Value Time = 0 [s] END TIME DURATION: Option = Total Time Total Time = 1 [s] END TIME STEPS: First Update Time = 0.0 [s] Initial Timestep = 2e05 [s] Option = Adaptive Timestep Update Frequency = 1 TIMESTEP ADAPTION: Courant Number = 10 Maximum Timestep = 0.0001 [s] Minimum Timestep = 1e05 [s] Option = MAX Courant Number END END END DOMAIN: Default Domain Coord Frame = Coord 0 Domain Type = Fluid Location = FLOW BOUNDARY: bladewall Boundary Type = WALL Location = BLADEWALL BOUNDARY CONDITIONS: MASS AND MOMENTUM: Option = No Slip Wall END WALL ROUGHNESS: Option = Smooth Wall END END END BOUNDARY: centplane Boundary Type = SYMMETRY Location = CENTWALL END BOUNDARY: inlet Boundary Type = INLET Coord Frame = Coord 0 Location = INLET BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END MASS AND MOMENTUM: Option = Cartesian Velocity Components U = Inlet Porfile.Velocity u(y) V = 0 [m s^1] W = 0 [m s^1] END TURBULENCE: Epsilon = Inlet Porfile.Turbulence Eddy Dissipation(y) Option = k and Epsilon k = Inlet Porfile.Turbulence Kinetic Energy(y) END END END BOUNDARY: outlet Boundary Type = OPENING Coord Frame = Coord 0 Location = OUTLET BOUNDARY CONDITIONS: FLOW DIRECTION: Option = Normal to Boundary Condition END FLOW REGIME: Option = Subsonic END MASS AND MOMENTUM: Option = Opening Pressure and Direction Relative Pressure = 93730 [Pa] END TURBULENCE: Eddy Length Scale = 0.00717 [m] Fractional Intensity = 0.002 Option = Intensity and Length Scale END END END BOUNDARY: platewall Boundary Type = WALL Location = PLATEWALL BOUNDARY CONDITIONS: MASS AND MOMENTUM: Option = No Slip Wall END WALL ROUGHNESS: Option = Smooth Wall END END END BOUNDARY: sidewall Boundary Type = WALL Coord Frame = Coord 0 Location = SIDEWALL BOUNDARY CONDITIONS: MASS AND MOMENTUM: Option = Free Slip Wall END END END BOUNDARY: topwall Boundary Type = WALL Coord Frame = Coord 0 Location = TOPWALL BOUNDARY CONDITIONS: MASS AND MOMENTUM: Option = Free Slip Wall END END END DOMAIN MODELS: BUOYANCY MODEL: Option = Non Buoyant END DOMAIN MOTION: Option = Stationary END MESH DEFORMATION: Option = None END REFERENCE PRESSURE: Reference Pressure = 0 [atm] END END FLUID DEFINITION: Fluid 1 Material = Air at 25 C Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID MODELS: COMBUSTION MODEL: Option = None END HEAT TRANSFER MODEL: Fluid Temperature = 25 [C] Option = Isothermal END THERMAL RADIATION MODEL: Option = None END TURBULENCE MODEL: Option = DES SST END TURBULENT WALL FUNCTIONS: Option = Automatic END END END OUTPUT CONTROL: MONITOR OBJECTS: Monitor Coefficient Loop Convergence = Off MONITOR BALANCES: Option = Full END MONITOR FORCES: Option = Full END MONITOR PARTICLES: Option = Full END MONITOR POINT: Monitor Point 1 Cartesian Coordinates = 0.00741 [m], 0.003783 [m], 0 [m] Option = Cartesian Coordinates Output Variables List = Velocity u END MONITOR POINT: Monitor Point 2 Cartesian Coordinates = 0.01102 [m], 0.003783 [m], 0 [m] Option = Cartesian Coordinates Output Variables List = Velocity u END MONITOR POINT: Monitor Point 3 Cartesian Coordinates = 0.0146 [m], 0.003783 [m], 0 [m] Option = Cartesian Coordinates Output Variables List = Velocity u END MONITOR POINT: Monitor Point 4 Cartesian Coordinates = 0.018 [m], 0.003783 [m], 0 [m] Option = Cartesian Coordinates Output Variables List = Velocity u END MONITOR POINT: Monitor Point 5 Cartesian Coordinates = 0.02151 [m], 0.003783 [m], 0 [m] Option = Cartesian Coordinates Output Variables List = Velocity u END MONITOR POINT: Monitor Point 6 Cartesian Coordinates = 0.02519 [m], 0.003783 [m], 0 [m] Option = Cartesian Coordinates Output Variables List = Velocity u END MONITOR POINT: Monitor Point 7 Cartesian Coordinates = 0.02897 [m], 0.00254 [m], 0 [m] Option = Cartesian Coordinates Output Variables List = Velocity u END MONITOR RESIDUALS: Option = Full END MONITOR TOTALS: Option = Full END END RESULTS: File Compression Level = Default Option = Standard END TRANSIENT RESULTS: Transient Results 1 File Compression Level = Default Option = Standard OUTPUT FREQUENCY: Option = Timestep Interval Timestep Interval = 2 END END TRANSIENT STATISTICS: Transient Statistics 1 Option = Arithmetic Average Output Variables List = Pressure END END SOLVER CONTROL: Turbulence Numerics = First Order ADVECTION SCHEME: Option = Central Difference END CONVERGENCE CONTROL: Maximum Number of Coefficient Loops = 4 Minimum Number of Coefficient Loops = 1 Timescale Control = Coefficient Loops END CONVERGENCE CRITERIA: Residual Target = 0.000001 Residual Type = RMS END TRANSIENT SCHEME: Option = Second Order Backward Euler TIMESTEP INITIALISATION: Lower Courant Number = 0.1 Option = Automatic Upper Courant Number = 1 END END END EXPERT PARAMETERS: apply ic fluctuations for les = t END END COMMAND FILE: Version = 12.0.1 END 

January 12, 2012, 06:41 
Inlet Profile

#9 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 6 
# ROOD Juntion flows Inlet Boundary Conditions for CFX
[Name] Inlet Porfile [Spatial Fields] y [Data] y [ m ],Velocity u [ m s^1 ],Turbulence Kinetic Energy [ m^2 s^2 ],Turbulence Eddy Dissipation [ m^2 s^3 ] 2.54E04, 7.75E+00, 2.38E+00, 8.41E+01 3.05E04, 9.85E+00, 3.65E+00, 1.60E+02 3.55E04, 1.15E+01, 4.11E+00, 1.91E+02 4.57E04, 1.30E+01, 3.95E+00, 1.80E+02 5.33E04, 1.39E+01, 3.89E+00, 1.75E+02 6.60E04, 1.49E+01, 3.67E+00, 1.61E+02 8.12E04, 1.58E+01, 3.53E+00, 1.52E+02 9.90E04, 1.64E+01, 3.29E+00, 1.36E+02 1.22E03, 1.70E+01, 3.06E+00, 1.23E+02 1.47E03, 1.75E+01, 3.14E+00, 1.27E+02 1.80E03, 1.82E+01, 3.27E+00, 1.35E+02 2.21E03, 1.88E+01, 3.11E+00, 1.25E+02 2.67E03, 1.93E+01, 3.01E+00, 1.20E+02 3.25E03, 1.99E+01, 2.92E+00, 1.14E+02 3.96E03, 2.06E+01, 2.91E+00, 1.14E+02 4.85E03, 2.13E+01, 2.78E+00, 1.06E+02 5.89E03, 2.19E+01, 2.69E+00, 1.01E+02 7.21E03, 2.27E+01, 2.26E+00, 7.78E+01 8.73E03, 2.36E+01, 1.95E+00, 6.23E+01 1.07E02, 2.44E+01, 1.50E+00, 4.21E+01 1.29E02, 2.52E+01, 1.16E+00, 2.84E+01 1.58E02, 2.61E+01, 6.72E01, 1.26E+01 1.92E02, 2.69E+01, 2.61E01, 3.05E+00 2.34E02, 2.73E+01, 4.42E02, 2.13E01 2.85E02, 2.70E+01, 1.55E02, 4.40E02 3.46E02, 2.74E+01, 1.15E02, 2.82E02 4.22E02, 2.71E+01, 7.39E03, 1.45E02 5.14E02, 2.71E+01, 6.76E03, 1.27E02 6.25E02, 2.74E+01, 1.01E02, 2.33E02 2.15E01, 2.74E+01, 0 , 0 

January 12, 2012, 17:12 

#10 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
I see a few problems with your setup, and most of them are major problems:
1) Your outlet boundary is too close. You will have to move this further back. 2) You minimum time step of 1e5s may not be short enough. I would define a minimum time step of 1e10 or something very small so if it needs small time steps it can use them. 3) Have you worked out the turbulence time scale? I would do that for the larger eddies you expect to see and then define an initial time step size smaller than than (maybe 1/20 of the turbulence time scale). 4) I would not use adaptive time stepping on courant number, I recommend 35 coeff loops per iteration. Courant number has little relevance to CFX. 5) Your outlet pressure is about 90kPa. This should be 0kPa and you should use a reference pressure of 90kPa. 6) You have a max of 4 and a min of 1 coeff loops per iteration. Remove this, you are not allowing it to converge fully. 

January 12, 2012, 22:58 

#11 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 6 
Hi, Glenn,
thank you very much for giving your valuable advice and sharing your valuable experience of using CFX. Now I am trying to do it by your advice. I will report here if any good news about that comes. Best regards. 

January 17, 2012, 00:24 

#12 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 6 
Dear Glenn,
I followed most of your instruction, except that I didn't change the outlet position for some other reasons. But it seemed that LES in DES still can't be actived. I upload my .def file here: http://turboupload.com/4jd73298o9xe Could you help me to check it in detail? If you cann't download the file, Could you tell me your email by message? I can send it to you by email. Best regrads 

January 17, 2012, 01:26 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
The turbulent structures are going to be down stream of the object, but you do not have much room down stream before it hits the outlet boundary. You really will need to move the outlet boundary downstream.
If you cannot do this can you explain why not? I do not give out my email address on the forum. And do not private message me about this either  this issue is best discussed on the forum. 

April 16, 2012, 06:57 

#14 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 6 
Dear Glenn,
I'm sorry I haven't given a reply for so many days. Although I have followed all your tips, I haven't succeeded activing the LES in DES until today that I change the ADVECTION SCHEME from Central Difference to High Resolution. CFX help document suggest Central Difference for LES, so I changed the default advection scheme to Central Difference because I thought DES is similar to LES. HaHa, now it seems that Central Difference advection scheme would prevent LES in DES from being actived. I don't know why, and the help document doesn't give guideline about this. 

April 17, 2012, 01:21 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
I would recommend you talk to CFX support about this and get some DES tutorials from them. It is an advanced turbulence model and if you guess the settings to use you will definitely get it wrong. There is also some publications on the model, ask for them as well.


April 17, 2012, 05:27 

#16 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 6 
Thank you for your advice.


January 13, 2014, 11:15 

#17  
Member
Lorenzo Mazzei
Join Date: Dec 2010
Posts: 39
Rep Power: 7 
Quote:


January 23, 2014, 05:45 

#18 
Member
Lorenzo Mazzei
Join Date: Dec 2010
Posts: 39
Rep Power: 7 
Ok, I believe the problem is due to the application of the Central Differencing scheme to the RANS region. The issue could be fixed using the Bounded Central Differencing scheme. Refer to CFX Reference Guide for further details.


Tags 
des les 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
LES and DES models for wind turbine  mohammad  Main CFD Forum  6  April 30, 2011 22:01 
LES or DES in wind turbine  mohammad  CFX  2  April 19, 2011 22:16 
Spanwise Length and Grid Refinement for SASSST, DES, and LES  Josh  CFX  5  October 14, 2010 19:47 
How to use DES well?  Daniel  Main CFD Forum  0  October 26, 2008 06:59 
DES or LES  J.Gimbun  FLUENT  0  February 22, 2006 04:42 