cyclone separator particle tracking prob..
 

Hi all,
I am working with a cyclone separator particle tracking model (by LES).
Here, it can be seen the velocity vector profile is quite strange. The vector profile of cyclone separator should be downward at free vortex region and upward in forced vortex region. Can anybody tell me why my results are deviate from this?

Also, I can see particle tracks at forced vortex, again extend to free vortex region. Even 0.5um particles are not exit from the domain. Any suggestions Please???

I am really stuck with this..

FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Dear Glenn,
Thanks a lot for the reply. I will consider these conditions.

But I have another doubt. I have set the bottom of the dustbin as a wall and perpendicular/parallel restitution factor as 1.
Now I am thinking that particles recirculate due to this, as I can see inside the dustbin, particle track is circulating and circulating up to end of simulation.
I can set stick to wall condition on dustbin bottom, but then there is a probability of sticking of particle range from 0-5um on there, as these range particles follow the full flow path.
I have seen in previous studies, particles are not having more circulation tracks at dust bin, but there is no any clear evidence about particle track settings for the dustbin.
Do you have any idea about this matter?

Sorry I do not understand your question. Can you explain it more?

Simply, how to set the boundary condition of the bottom of cyclone separator?
I used is as a smooth wall, bz of particles (2um) reach to cyclone bottom and then turn up. But from results I can see a huge particle recirculate are inside the cyclone separator.

I still don't understand what you are trying to do but I will ahve a guess. It seems like you need an outlet on the bottom to allow the large particles to exit, as expected. But you seem to be saying the small particles also exit through this outlet where they should turn and go up the riser. This is likely to be an error or inaccuracy in your simulation and not directly related to your choice of bottom BC.

Have you done a mesh sensitivity study? Convergence? Time step?

Dear Glenn, thanks a lot for the reply.
Actually, I don't have a outlet at the bottom, it is a wall.
Particles reach to this bottom wall turn and go up. it is ok.
But the problem is, those particle going upward, again join to the downward flow and come down again. There is no exit from the top outlet. Only a little bit of particles goes out from the top outlet.

You can see it by attached figures.

PT1: 1um diameter and PT2: 9um diameter particles.

Mesh is fine and simulation converge well. Time step is 0.001S.

+--------------------------------------------------------------------+
| |
| CFX Command Language for Run |
| |
+--------------------------------------------------------------------+

LIBRARY:
CEL:
EXPRESSIONS:
MFR = 1.414E-8 [kg s^-1]
PR = 1E5*step(0.021-t/1[s]) [s^-1]
END
END
MATERIAL: Air at 25 C
Material Description = Air at 25 C and 1 atm (dry)
Material Group = Air Data, Constant Property Gases
Option = Pure Substance
Thermodynamic State = Gas
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 1.185 [kg m^-3]
Molar Mass = 28.96 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 1.0044E+03 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0. [J/kg]
Reference Specific Entropy = 0. [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 1.831E-05 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 2.61E-02 [W m^-1 K^-1]
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 0.01 [m^-1]
Option = Value
END
SCATTERING COEFFICIENT:
Option = Value
Scattering Coefficient = 0.0 [m^-1]
END
REFRACTIVE INDEX:
Option = Value
Refractive Index = 1.0 [m m^-1]
END
THERMAL EXPANSIVITY:
Option = Value
Thermal Expansivity = 0.003356 [K^-1]
END
END
END
MATERIAL: Particles
Material Group = Particle Solids
Option = Pure Substance
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 500 [kg m^-3]
Molar Mass = 1.0 [kg kmol^-1]
Option = Value
END
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 = 3 [s]
END
TIME STEPS:
Option = Timesteps
Timesteps = 0.001 [s]
END
END
DOMAIN: cyclone
Coord Frame = Coord 0
Domain Type = Fluid
Location = CREATED_MATERIAL_12,CREATED_MATERIAL_13
BOUNDARY: Box walls
Boundary Type = WALL
Location = BOX
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
FLUID: particles
BOUNDARY CONDITIONS:
PARTICLE WALL INTERACTION:
Option = Equation Dependent
END
VELOCITY:
Option = Restitution Coefficient
Parallel Coefficient of Restitution = 1.0
Perpendicular Coefficient of Restitution = 1.0
END
END
END
END
BOUNDARY: cyclone walls
Boundary Type = WALL
Location = \
VORTEX_FINDER_1,VORTEX_FINDER_2,TOP_CAP,OULLET_TUB E,INLET_TUBE,HOPPER\
_BASE,HOPPER,BODY
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
FLUID: particles
BOUNDARY CONDITIONS:
PARTICLE WALL INTERACTION:
Option = Equation Dependent
END
VELOCITY:
Option = Restitution Coefficient
Parallel Coefficient of Restitution = 1.0
Perpendicular Coefficient of Restitution = 1.0
END
END
END
END
BOUNDARY: inlet
Boundary Type = INLET
Location = INLET
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Normal Speed = 2.4 [m s^-1]
Option = Normal Speed
END
END
FLUID: particles
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Normal Speed = 2.4 [m s^-1]
Option = Normal Speed
END
PARTICLE MASS FLOW RATE:
Mass Flow Rate = MFR
END
PARTICLE POSITION:
Option = Uniform Injection
Particle Locations = Random
NUMBER OF POSITIONS:
Number per Unit Time = PR
Option = Direct Specification
END
END
END
END
END
BOUNDARY: oultet
Boundary Type = OPENING
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 = 0 [Pa]
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 1.2 [kg m^-3]
Gravity X Component = 0 [m s^-2]
Gravity Y Component = -9.81 [m s^-2]
Gravity Z Component = 0 [m s^-2]
Option = Buoyant
BUOYANCY REFERENCE LOCATION:
Option = Automatic
END
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 101325 [Pa]
END
END
FLUID DEFINITION: Air
Material = Air at 25 C
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: particles
Material = Particles
Option = Material Library
MORPHOLOGY:
Option = Dispersed Particle Transport Solid
PARTICLE DIAMETER DISTRIBUTION:
Maximum Diameter = 10.08 [micron]
Mean Diameter = 3.78 [micron]
Minimum Diameter = 0.647 [micron]
Option = Normal in Diameter by Number
Standard Deviation in Diameter = 2.44 [micron]
END
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
FLUID: Air
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
FLUID: particles
EROSION MODEL:
Option = None
END
FLUID BUOYANCY MODEL:
Option = Density Difference
END
PARTICLE ROUGH WALL MODEL:
Option = None
END
END
HEAT TRANSFER MODEL:
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = LES Smagorinsky
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
FLUID PAIR: Air | particles
Particle Coupling = Fully Coupled
MOMENTUM TRANSFER:
DRAG FORCE:
Option = Schiller Naumann
END
PRESSURE GRADIENT FORCE:
Option = None
END
TURBULENT DISPERSION FORCE:
Option = None
END
VIRTUAL MASS FORCE:
Option = None
END
END
END
END
OUTPUT CONTROL:
RESULTS:
File Compression Level = Default
Option = Standard
END
TRANSIENT RESULTS: Transient Results 1
File Compression Level = Default
Option = Standard
OUTPUT FREQUENCY:
Option = Time Interval
Time Interval = 0.5 [s]
END
END
TRANSIENT STATISTICS: velocity max
Option = Maximum
Output Variables List = Velocity
END
TRANSIENT STATISTICS: velocity min
Option = Maximum
Output Variables List = Velocity
END
TRANSIENT STATISTICS: velocity rms
Option = Root Mean Square
Output Variables List = Velocity
END
TRANSIENT STATISTICS: velocity std
Option = Standard Deviation
Output Variables List = Velocity
END
END
SOLVER CONTROL:
ADVECTION SCHEME:
Bounded CDS = No
Option = Central Difference
END
CONVERGENCE CONTROL:
Maximum Number of Coefficient Loops = 3
Minimum Number of Coefficient Loops = 1
Timescale Control = Coefficient Loops
END
CONVERGENCE CRITERIA:
Residual Target = 0.00001
Residual Type = RMS
END
PARTICLE CONTROL:
PARTICLE INTEGRATION:
First Iteration for Particle Calculation = 3
Iteration Frequency = 3
Option = Forward Euler
END
PARTICLE TERMINATION CONTROL:
Maximum Number of Integration Steps = 50000
Maximum Tracking Distance = 10 [m]
Maximum Tracking Time = 10 [s]
END
PARTICLE UNDER RELAXATION FACTORS:
Velocity Under Relaxation Factor = 0.1
END
END
TRANSIENT SCHEME:
Option = Second Order Backward Euler
TIMESTEP INITIALISATION:
Lower Courant Number = 0.00001
Option = Automatic
Upper Courant Number = 1
END
END
END
END
COMMAND FILE:
Version = 14.0
Results Version = 14.0
END
SIMULATION CONTROL:
EXECUTION CONTROL:
EXECUTABLE SELECTION:
Double Precision = On
END
INTERPOLATOR STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
END
PARALLEL HOST LIBRARY:
HOST DEFINITION: master.local
Installation Root = /share/apps/ansys_inc/v%v/CFX
Host Architecture String = linux-amd64
END
HOST DEFINITION: node10.local
Host Architecture String = linux-amd64
Installation Root = /share/apps/ansys_inc/v%v/CFX
Number of Processors = 24
END
END
PARTITIONER STEP CONTROL:
Multidomain Option = Independent Partitioning
Runtime Priority = Standard
EXECUTABLE SELECTION:
Use Large Problem Partitioner = Off
END
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARTITIONING TYPE:
MeTiS Type = k-way
Option = MeTiS
Partition Size Rule = Automatic
Partition Weight Factors = 0.04000, 0.04000, 0.04000, 0.04000, \
0.04000, 0.04000, 0.04000, 0.04000, 0.04000, 0.04000, 0.04000, \
0.04000, 0.04000, 0.04000, 0.04000, 0.04000, 0.04000, 0.04000, \
0.04000, 0.04000, 0.04000, 0.04000, 0.04000, 0.04000, 0.04000
END
END
RUN DEFINITION:
Run Mode = Full
Solver Input File = /home/particleP/M2.4.def
INITIAL VALUES SPECIFICATION:
INITIAL VALUES CONTROL:
Continue History From = Initial Values 1
Use Mesh From = Solver Input File
END
INITIAL VALUES: Initial Values 1
File Name = /home/particleP/M2.4_001.res
Option = Results File
END
END
END
SOLVER STEP CONTROL:
Runtime Priority = High
MEMORY CONTROL:
Memory Allocation Factor = 10
END
PARALLEL ENVIRONMENT:
Parallel Host List = master.local,node10.local*24
Start Method = MPICH Distributed Parallel
END
END
END
END

Are you sure 3s run time is enough to create the central vortex which does the separation?

Why do you say your mesh is OK? How did you check?

Why have you limited it to 1-3 coeff loops per iteration? The recommended setting is 10, then use adaptive time stepping to home in on 3-5 coeff loops per iteration.

Gear Glenn,
It is very kind of you.

01. I haven't check the mesh sensitivity, as I am doing course and fine mesh conditions. Total mesh elements= 2698757
02. The cyclone geometry is very small (D=66.04mm). After 1S, particle start to exit (only a little amount). Its ok I can extend the time, but have you noticed particles are recirculating without exiting?
03. I haven't used adaptive time step before. Ok, let me to try it.

Why do I get a feeling that there is only one particle in your plots? Something doesn't seem right.

Are you sure about BCs, ie mass flow rate of fluid and the particles? In my experience, the collection efficiency increases with increase in mass flow.

Also, have you tried this with kw-SST/RSM etc first? Why jump to LES?

OJ

Dear Oj,
I have used 2000 particles but, shown here are only two tracks, 1um and 9um.
Boundary conditions are;
Inlet: 2.4ms velocity for both fluid and particles.
Particle injection: 100 particles injected at each time step up to 0.02S and then particle injection stopped.
Outlet: Opening boundary condition
Walls: smooth walls, restitution factor=1.0

I have found that LES gives accurate results than RSM or SST. That is why I used it.

One more thing,
I can see in convergence charts of my simulation, fluid flow has no oscillations but in particle source rate change chart has huge oscillations.
If then, does particle source diverge? There is no any solver crash.

LES is very mesh sensitive and requires a MUCH finer mesh than SST or RSM. You will need to do a very careful mesh sensitivity study to be confident you are accurate. And I agree with OJ, I would work on SST (with curvature correction option enabled) and RSM before considering LES.

LES really is a very complex model - have you checked your mesh size is in the correct range? The turbulence energy spectrum is about right? The inlet boundary includes resolved turbulent structures? Unless you have checked these issues you are kidding yourself with LES.

And yes, I am suspicious that you simply have not run this model for long enough to establish the flow field which does the separation. I would definitely try running it longer.

Hi Glenn,
I have checked mesh quality, and it is in acceptable range. But I haven'd done a turbulence kinetic energy spectrum. I tried to define a point in CFX post to monitor velocity components, but failed.

For inlet boundary, I used steady state results as initial conditions.

If I do RSM, how can I make sure about accuracy of LES?

LES requires a lot of additional checks and care or the results will be rubbish. You will need to refer to a turbulence modelling textbook such as Turbulence modelling for CFD by Wilcox for details.

I do not understand the link between RSM and LES you seem to imply. One is a Reynolds averaged approach and one is LES. Very different approaches and may well give quite different results. But RSM is easier to apply than LES so I would definitely use RSM in preference to LES if it is applicable.

I was referring to more than mesh quality - what about the mesh density? You need a fine enough mesh to be accurate.

Hi Glenn,
What do you mean by "mesh quality"? Sorry, if I don't understand wrongly, I have a prism mesh, and had not created any mesh densities.
These are the mesh qualities.

Histogram of Quality values
0.95 -> 1.0 : 92262 (3.495%)
0.9 -> 0.95 : 605925 (22.955%)
0.85 -> 0.9 : 337262 (12.777%)
0.8 -> 0.85 : 237633 (9.003%)
0.75 -> 0.8 : 190340 (7.211%)
0.7 -> 0.75 : 165458 (6.268%)
0.65 -> 0.7 : 147791 (5.599%)
0.6 -> 0.65 : 144001 (5.455%)
0.55 -> 0.6 : 131775 (4.992%)
0.5 -> 0.55 : 206697 (7.831%)
0.45 -> 0.5 : 299196 (11.335%)
0.4 -> 0.45 : 81146 (3.074%)
0.35 -> 0.4 : 78 (0.003%)
0.3 -> 0.35 : 11 (0.000%)
0.25 -> 0.3 : 0 (0.000%)
0.2 -> 0.25 : 0 (0.000%)
0.15 -> 0.2 : 0 (0.000%)
0.1 -> 0.15 : 0 (0.000%)
0.05 -> 0.1 : 0 (0.000%)
0.0 -> 0.05 : 0 (0.000%)

Histogram of Aspect ratio values
0.95 -> 1.0 : 92262 (3.495%)
0.9 -> 0.95 : 605925 (22.955%)
0.85 -> 0.9 : 337262 (12.777%)
0.8 -> 0.85 : 237633 (9.003%)
0.75 -> 0.8 : 190340 (7.211%)
0.7 -> 0.75 : 165458 (6.268%)
0.65 -> 0.7 : 147791 (5.599%)
0.6 -> 0.65 : 144001 (5.455%)
0.55 -> 0.6 : 131775 (4.992%)
0.5 -> 0.55 : 206697 (7.831%)
0.45 -> 0.5 : 299196 (11.335%)
0.4 -> 0.45 : 81146 (3.074%)
0.35 -> 0.4 : 78 (0.003%)
0.3 -> 0.35 : 11 (0.000%)
0.25 -> 0.3 : 0 (0.000%)
0.2 -> 0.25 : 0 (0.000%)
0.15 -> 0.2 : 0 (0.000%)
0.1 -> 0.15 : 0 (0.000%)
0.05 -> 0.1 : 0 (0.000%)
0.0 -> 0.05 : 0 (0.000%)

Histogram of Volume values
427.5 -> 450.0 : 1 (0.000%)
405.0 -> 427.5 : 1 (0.000%)
382.5 -> 405.0 : 2 (0.000%)
360.0 -> 382.5 : 4 (0.000%)
337.5 -> 360.0 : 24 (0.001%)
315.0 -> 337.5 : 303 (0.011%)
292.5 -> 315.0 : 1119 (0.042%)
270.0 -> 292.5 : 585 (0.022%)
247.5 -> 270.0 : 316 (0.012%)
225.0 -> 247.5 : 152 (0.006%)
202.5 -> 225.0 : 128 (0.005%)
180.0 -> 202.5 : 149 (0.006%)
157.5 -> 180.0 : 581 (0.022%)
135.0 -> 157.5 : 1386 (0.053%)
112.5 -> 135.0 : 669 (0.025%)
90.0 -> 112.5 : 807 (0.031%)
67.5 -> 90.0 : 5402 (0.205%)
45.0 -> 67.5 : 3773 (0.143%)
22.5 -> 45.0 : 46705 (1.769%)
0.0 -> 22.5 : 2364858 (89.592%)

Histogram of Determinant values
0.95 -> 1.0 : 2426965 (91.945%)
0.9 -> 0.95 : 0 (0.000%)
0.85 -> 0.9 : 0 (0.000%)
0.8 -> 0.85 : 0 (0.000%)
0.75 -> 0.8 : 0 (0.000%)
0.7 -> 0.75 : 0 (0.000%)
0.65 -> 0.7 : 0 (0.000%)
0.6 -> 0.65 : 0 (0.000%)
0.55 -> 0.6 : 0 (0.000%)
0.5 -> 0.55 : 0 (0.000%)
0.45 -> 0.5 : 0 (0.000%)
0.4 -> 0.45 : 0 (0.000%)
0.35 -> 0.4 : 0 (0.000%)
0.3 -> 0.35 : 0 (0.000%)
0.25 -> 0.3 : 0 (0.000%)
0.2 -> 0.25 : 0 (0.000%)
0.15 -> 0.2 : 0 (0.000%)
0.1 -> 0.15 : 0 (0.000%)
0.05 -> 0.1 : 0 (0.000%)
0.0 -> 0.05 : 0 (0.000%)

Histogram of Skew values
0.95 -> 1.0 : 139224 (5.274%)
0.9 -> 0.95 : 42732 (1.619%)
0.85 -> 0.9 : 16992 (0.644%)
0.8 -> 0.85 : 6398 (0.242%)
0.75 -> 0.8 : 2734 (0.104%)
0.7 -> 0.75 : 1680 (0.064%)
0.65 -> 0.7 : 1326 (0.050%)
0.6 -> 0.65 : 840 (0.032%)
0.55 -> 0.6 : 441 (0.017%)
0.5 -> 0.55 : 157 (0.006%)
0.45 -> 0.5 : 69 (0.003%)
0.4 -> 0.45 : 17 (0.001%)
0.35 -> 0.4 : 0 (0.000%)
0.3 -> 0.35 : 0 (0.000%)
0.25 -> 0.3 : 0 (0.000%)
0.2 -> 0.25 : 0 (0.000%)
0.15 -> 0.2 : 0 (0.000%)
0.1 -> 0.15 : 0 (0.000%)
0.05 -> 0.1 : 0 (0.000%)
0.0 -> 0.05 : 0 (0.000%)

Mesh quality is an indication of how proportionate individual cells of mesh are, but mesh density decides whether there are "enough" number of cells in the critical regions of high gradients, ie the regions where flow properties change significantly. If you have perfect hexagonal cells with good quality in these regions, but if they are larger and too few in number, the mesh is not adequate. That is the reason why mesh independence study is imperative.

How have you decided the cell size of the mesh used for LES? I think if you believe that you need accurate modelling than normal k-eps/SST models which assume isotropic turbulence, you can go for RSM which can cater to anisotropic turbulence.

I have seen studies which recommend that with LES, one should model a small part of the domain rather than the whole domain, because the grid size for LES is typically very small and hence this model is restrictive in terms of its use for a full domain.

OJ

Hi Oj,
Thanks a lot for information. Actually I haven't used mesh density.
Also, for cell size, I used Auto sizing for max. size. Scale factor was 2. And for surface mesh size, used o.5 for inlet surface and 1 for other surfaces. Curve mesh size was 0.

Histogram of Max length values
18.05 -> 19.0 : 8 (0.000%)
17.1 -> 18.05 : 107 (0.004%)
16.15 -> 17.1 : 1483 (0.056%)
15.2 -> 16.15 : 1512 (0.057%)
14.25 -> 15.2 : 1749 (0.066%)
13.3 -> 14.25 : 2324 (0.088%)
12.35 -> 13.3 : 4633 (0.176%)
11.4 -> 12.35 : 816 (0.031%)
10.45 -> 11.4 : 209 (0.008%)
9.5 -> 10.45 : 1530 (0.058%)
8.55 -> 9.5 : 3742 (0.142%)
7.6 -> 8.55 : 44848 (1.699%)
6.65 -> 7.6 : 23499 (0.890%)
5.7 -> 6.65 : 49650 (1.881%)
4.75 -> 5.7 : 8295 (0.314%)
3.8 -> 4.75 : 275717 (10.446%)
2.85 -> 3.8 : 415674 (15.748%)
1.9 -> 2.85 : 1607418 (60.897%)
0.95 -> 1.9 : 196252 (7.435%)
0.0 -> 0.95 : 109 (0.004%)

According to you two, I am trying with RSM, but seems it takes longer time to simulate than LES (I haven't used particles this time to see flow is correct or not). And also, more fluctuations.

Hi Sakura,

I think you are misunderstanding what OJ and I are saying about mesh density. We are not talking about the mesh density tool in ICEM. Imagine you have a 1m cube region you are meshing. If you use a hex mesh with 0.1m edge length you will have 1000 mesh elements to fill it. If you use a hex mesh with a 0.01m edge length you will need 10^6 elements to fill it. The 0.01m edge length mesh is a denser mesh and has a much better chance of capturing important flow details as the coarser 0.1m mesh has inadequate resolution. Of course the down side is you need a big computer to run it, it will take far longer to converge and it has less numerical stability. But the skill of the CFD expert is to keep this issues under control and still get a simulation which resolves the important flow features.

ANd another important point - just because you turn on the LES turbulence model does not mean you are doing a LES simulation. The mesh, convergence and timestep requirements for a LES simulation are very different to a RANS simulation, so if you just flicked the turbulence model over and did no other adjustments your results are almost certainly rubbish.

The statistics you are providing indicates the mesh quality. But this won't help us identify if you reduce the mesh cell size, whether the results will change, ie, whether your solution is independent of mesh.

I was surprised when you said it took longer with RSM than LES. RSM models all the lengthscales while LES resolves the larger lengthscales and models the smaller ones. Ideally, LES should be more expensive than RSM, unless of course, if it is not done the way it is meant to be! This again brings up the point, how are you sure about the grid size, timescales, initial conditions and criteria for filtering the lengthscales in your LES?

I'd start with a 2-eqn model like kw-SST or RNG (since you have a lot of circulation) and get a decent converged solution, after doing a mesh independence study. Then switch it to RSM to finally converge it to the best modeled solution you can have. This way, you will at least know what you are doing. Beats fancy LES with so many doubts!


OJ

If the Smagorinsky SGS model is used in LES with a mesh which is grossly too large then the SGS viscosity goes very high (the SGS viscosity is proportional to mesh length scale squared see eqn 2-161 in the theory manual) and is therefore highly dissipative.

This means fast, easy convergence to a solution which is completely wrong.

So Sakura's comment that RSM is harder to converge and slower than LES is further evidence that the mesh size he is using is far too large for LES.

Dear Glenn and OJ,
Really really thankful for helping.
I got what you meant. Yes, I can understand there is a problem with my mesh.
If RSM takes more time than LES is impossible, because it is two times slower than LES now.
I'll check mesh again.

Hi Glenn,
Of course I am using Smagorinsky LES. :(

If that so, the problem definitely with the mesh. Thank you, thank you very much for help me to find the wrong point, as I have very limited time to complete this.

Hi All,
I have done mesh sensitivity analysis for 5 mesh types and considered a significant point rms velocity.
M1(elements:2500000): 6.474m/s
M2(elements:3250000): 6.501m/s
M3(elements:5300000): 6.511m/s
M4(elements:6450000): 6.443m/s
M5(elements:9700000): 6.489m/s
Although there is no much variation, I used M5 for RSM as M1 is the mesh size that gave the wrong results.

Meanwhile I ran LES with mesh size M5, it runs with smaller time step than RSM, but still I can see it runs faster than RMS. (no. of time steps per a given time). Can you please tell me is this ok?

I am using adaptive time steps now and can also see LES reaches convergence quicker than RSM.

As Glenn suggests, the faster convergence is probably attributed to the numerical dissipation. LES can't be trusted unless you use adequate grid size and timescales, and the "mesh independence study" you are doing doesn't seem to be an appropriate way to conclude, without taking into account if adequate lengthscales are resolved.

You should resolve the scales only to the extent that below it, the turbulence is isotropic, which is handled well by the SGS models. Often this lengthscale is considered to be close to Taylor's lengthscale. The accuracy lost in modelling the anisotropic turbulence by SGS models, when you use larger than appropriate grid size, will be decided by your physics.

Situation is aggravated when you have wall bounded flows, where the grid size requirements are still critical!

OJ

Dear OJ,
Thanks a lot.
I can see the mesh is very fine, but as you said, still it is not appropriate for LES. Then, how can I check if adequate lengthscales are resolved?
The other problem is, by this way, are results from RSM also incorrect? It takes more computational cost, like to run 0.5S, uses 5days.

The key check for an LES model that your mesh and timescales are adequately resolved is to plot the turbulence power spectrum (intensity versus frequency, eg http://theeternaluniverse.blogspot.c...ber-space.html). If you get the -5/3 decay in the spectrum down to your filtering size then you know you are on the right track.

Dear Glenn,
Thanks a lot.
But again I have a problem. Is there anyway to monitor Turbulence intensity(I) in CFX Pre?
I=u'/U
u'=(2k/3)^0.5 ----- k-kinetic energy relates to rms velocities
So how can I monitor rms velocities? I have already used them in trn statistics.
I can calculate U(mean velocity) by monitoring u,v,w velocity components.

Thanks.

You have to define all these variables as CEL expressions. The tricky one is the u' terms - are you doing spatial or temporal averaging to obtain them? Neither of these are easy to implement in CEL.

Dear Glenn,
I am thinking about temporal averaging velocities.

Another issue is when use expressions in monitor tab, I cannot specify a location.

I heard TI can be calculated by FFT.

CEL cannot calculate anything in time, so you are either going to have to do this in post processing or write your own user fortran to do it (and that will not be easy).

When I did this previously in CFX I set monitor points at the locations I wanted the turbulence intensity at and wrote the UVW velocity components to monitor points. Then you can externally process the monitor point data to get your u'v'w' parameters. Then you do FFT on the u'v'w' to get the turbulence intensity spectrum.

I think RSM is tuned to handle anisotropic turbulence far better than SGS models. So if your grid is not small enough to capture the anisotropy-range lengthscales, they are passed on to SGS models and I am not sure if these are robust enough to deal with it, as they are tuned for isotropic turbulence.

OJ

The SGS models in LES are generally based on the assumption (which is generally a good assumption) that all the anisotropy in turbulence resides in the largest turbulence scales and the small scale turbuelnce is isotropic. In LES the large scale turbulence is modelled by the solver and the small scale stuff is modelled by the SGS, so an isotropic SGS is adequate for LES.

But for this assumption to be correct you need to show that your mesh and filtering is in fact correctly set up for this distinction.

I have data of u,v,w and can do the fft. but my problem is how to get the frequency?

in matlab we can write write code,
N=--; %no. of data points (2^n value)
T=--; %sample length
fc=(0:N)/T; %sample frequency

but my problem is I have omitted first half of data, so sampling time does not start from 0S, it has a value (t).

then, fc should be,
fc=(t:N)/T; ????? Am I correct?

Thanks.