CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   LES in DES can't be actived! (http://www.cfd-online.com/Forums/cfx/96048-les-des-cant-actived.html)

shenying0710 January 11, 2012 05:47

LES in DES can't be actived!
 
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.

ghorrocks January 11, 2012 06:50

Are you sure you are in a flow regime where you get LES style turbulent structures?

shenying0710 January 11, 2012 10:39

Quote:

Originally Posted by ghorrocks (Post 338782)
Are you sure you are in a flow regime where you get LES style turbulent structures?

Sure, the flow is full turbulent. Many other researchers have done DES on this flow with the same flow conditions.

stumpy January 11, 2012 11:47

Perhaps you need some inlet fluctuations to trigger the turbulence generation.

shenying0710 January 11, 2012 23:06

Quote:

Originally Posted by stumpy (Post 338833)
Perhaps you need some inlet fluctuations to trigger the turbulence generation.

Thanks, Stumpy. Your advice had made me excited and I tried to give some inlet fluctuations( I tried two ways, first, set fluctuations in domain initialisation; secondly, change the expert parameter " apply ic fluctuations for les" to 't' so that I can restart the fluctuations from RANS result file.)
However, the two ways both seemed to fail because after several timesteps I checked the blending function for DES in CFD-post and found that it is still equal to 1 all over the flowfield.

ghorrocks January 12, 2012 05:34

Can you post your CCL file and an image of the geometry?

shenying0710 January 12, 2012 06:35

1 Attachment(s)
The picture of the model:
Attachment 10815

shenying0710 January 12, 2012 06:37

# State file created: 2012/01/12 18:31:40
# CFX-12.0.1 build 2009.04.14-23.02
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 = 2e-05 [s]
Option = Adaptive
Timestep Update Frequency = 1
TIMESTEP ADAPTION:
Courant Number = 10
Maximum Timestep = 0.0001 [s]
Minimum Timestep = 1e-05 [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

shenying0710 January 12, 2012 06:41

Inlet Profile
 
# 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 ]
2.54E-04, 7.75E+00, 2.38E+00, 8.41E+01
3.05E-04, 9.85E+00, 3.65E+00, 1.60E+02
3.55E-04, 1.15E+01, 4.11E+00, 1.91E+02
4.57E-04, 1.30E+01, 3.95E+00, 1.80E+02
5.33E-04, 1.39E+01, 3.89E+00, 1.75E+02
6.60E-04, 1.49E+01, 3.67E+00, 1.61E+02
8.12E-04, 1.58E+01, 3.53E+00, 1.52E+02
9.90E-04, 1.64E+01, 3.29E+00, 1.36E+02
1.22E-03, 1.70E+01, 3.06E+00, 1.23E+02
1.47E-03, 1.75E+01, 3.14E+00, 1.27E+02
1.80E-03, 1.82E+01, 3.27E+00, 1.35E+02
2.21E-03, 1.88E+01, 3.11E+00, 1.25E+02
2.67E-03, 1.93E+01, 3.01E+00, 1.20E+02
3.25E-03, 1.99E+01, 2.92E+00, 1.14E+02
3.96E-03, 2.06E+01, 2.91E+00, 1.14E+02
4.85E-03, 2.13E+01, 2.78E+00, 1.06E+02
5.89E-03, 2.19E+01, 2.69E+00, 1.01E+02
7.21E-03, 2.27E+01, 2.26E+00, 7.78E+01
8.73E-03, 2.36E+01, 1.95E+00, 6.23E+01
1.07E-02, 2.44E+01, 1.50E+00, 4.21E+01
1.29E-02, 2.52E+01, 1.16E+00, 2.84E+01
1.58E-02, 2.61E+01, 6.72E-01, 1.26E+01
1.92E-02, 2.69E+01, 2.61E-01, 3.05E+00
2.34E-02, 2.73E+01, 4.42E-02, 2.13E-01
2.85E-02, 2.70E+01, 1.55E-02, 4.40E-02
3.46E-02, 2.74E+01, 1.15E-02, 2.82E-02
4.22E-02, 2.71E+01, 7.39E-03, 1.45E-02
5.14E-02, 2.71E+01, 6.76E-03, 1.27E-02
6.25E-02, 2.74E+01, 1.01E-02, 2.33E-02
2.15E-01, 2.74E+01, 0 , 0

ghorrocks January 12, 2012 17:12

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 1e-5s may not be short enough. I would define a minimum time step of 1e-10 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 3-5 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.

shenying0710 January 12, 2012 22:58

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.

shenying0710 January 17, 2012 00:24

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

ghorrocks January 17, 2012 01:26

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.

shenying0710 April 16, 2012 06:57

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. Ha-Ha, 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.

ghorrocks April 17, 2012 01:21

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.

shenying0710 April 17, 2012 05:27

Thank you for your advice.

Mazze[ITA] January 13, 2014 11:15

Quote:

Originally Posted by shenying0710 (Post 354857)
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. Ha-Ha, 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.

I have experienced the same issue. Did you find an explanation?

Mazze[ITA] January 23, 2014 05:45

Quote:

Originally Posted by Mazze[ITA] (Post 469824)
I have experienced the same issue. Did you find an explanation?

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.


All times are GMT -4. The time now is 08:21.