[Spray_Ansys]

Hello everyone!

I'm currently simulating a steady state spray breakup and found this video on youtube:
https://www.youtube.com/watch?v=NAdZhoBEwtA

Unfortunately there are no details given and there isn't existing a good tutorial on the Internet. Therefore I want to ask you:

I'm working with a nozzle diameter of 0.75mm and simulation area of 2mm diameter and 200mm length. Flow velocity (Water) is 150 m/s. Calculating the LISA Model, the breakup should happen at a length of around 170mm. I'm using a hexaeder mesh with 3.5 million nodes. The air is compressible and there exists a heat transfer between water and air.

What are the most important settings to achieve such a spray breakup? Which turbulence model, what time scale do you recommend? I'm looking for the roughly details or ways that I should try to go with.

If you need more details, please ask me

[ghorrocks]

Spray breakup using Lagrangian particle tracking with models like LISA are not affected greatly by the turbulence model (as far as I know). So your choice of turbulence model should be made on other factors.

The most important thing to do in any simulation where you are looking for accuracy is a validation and verification process. This FAQ discusses some of the issues you want to avoid: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

[Spray_Ansys]

Thank you!
What do you think about the following setup? Is there something essential missing? Could it work like that?

LIBRARY:
CEL:
EXPRESSIONS:
R0 = 0.75 [mm]
VOFaxialAir = 1*step((radius-0.5*R0)/R0)
VOFaxialDiesel = 1*step((0.5*R0-radius)/R0)
massINLET = Diesel.massFlow()@Inlet
massOPENING = Diesel.massFlow()@Opening
radius = sqrt((x^2)+(y^2))
w0 = 150 [m/s]
w1 = w0*(exp(-(radius-0.5*R0)/(0.25*R0)))
waxial = min(w0, w1)
END
END
MATERIAL: Air Ideal Gas
Material Description = Air Ideal Gas (constant Cp)
Material Group = Air Data, Calorically Perfect Ideal Gases
Option = Pure Substance
Thermodynamic State = Gas
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Molar Mass = 28.96 [kg kmol^-1]
Option = Ideal Gas
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-2 [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
END
END
MATERIAL: Water
Material Description = Water (liquid)
Material Group = Water Data, Constant Property Liquids
Option = Pure Substance
Thermodynamic State = Liquid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 997.0 [kg m^-3]
Molar Mass = 18.02 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 4181.7 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0.0 [J/kg]
Reference Specific Entropy = 0.0 [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 8.899E-4 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 0.6069 [W m^-1 K^-1]
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 1.0 [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 = 2.57E-04 [K^-1]
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 = Steady State
EXTERNAL SOLVER COUPLING:
Option = None
END
END
DOMAIN: Default Domain
Coord Frame = Coord 0
Domain Type = Fluid
Location = BODY
BOUNDARY: Inlet
Boundary Type = INLET
Location = INLET
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
HEAT TRANSFER:
Option = Fluid Dependent
END
MASS AND MOMENTUM:
Option = Cartesian Velocity Components
U = 0 [m s^-1]
V = 0 [m s^-1]
W = w0
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
FLUID: Air
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Static Temperature
Static Temperature = 298 [K]
END
VOLUME FRACTION:
Option = Value
Volume Fraction = 0
END
END
END
FLUID: Diesel
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Static Temperature
Static Temperature = 310 [K]
END
VOLUME FRACTION:
Option = Value
Volume Fraction = 1
END
END
END
END
BOUNDARY: Opening
Boundary Type = OPENING
Location = SIDE,BACK
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
HEAT TRANSFER:
Option = Fluid Dependent
END
MASS AND MOMENTUM:
Option = Opening Pressure and Direction
Relative Pressure = 0 [bar]
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
FLUID: Air
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Static Temperature
Static Temperature = 298 [K]
END
VOLUME FRACTION:
Option = Value
Volume Fraction = 1
END
END
END
FLUID: Diesel
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Static Temperature
Static Temperature = 310 [K]
END
VOLUME FRACTION:
Option = Value
Volume Fraction = 0
END
END
END
END
BOUNDARY: Wall
Boundary Type = WALL
Location = WALL
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = Free Slip Wall
END
END
FLUID PAIR: Air | Diesel
BOUNDARY CONDITIONS:
WALL ADHESION:
Option = None
END
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 = 1 [atm]
END
END
FLUID DEFINITION: Air
Material = Air Ideal Gas
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: Diesel
Material = Water
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
FLUID: Air
HEAT TRANSFER MODEL:
Include Viscous Work Term = True
Option = Total Energy
END
END
FLUID: Diesel
HEAT TRANSFER MODEL:
Option = Thermal Energy
END
END
HEAT TRANSFER MODEL:
Homogeneous Model = Off
Option = Fluid Dependent
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = SST
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
FLUID PAIR: Air | Diesel
Surface Tension Coefficient = 0.072 [N m^-1]
INTERPHASE HEAT TRANSFER:
Heat Transfer Coefficient = 10 [W m^-2 K^-1]
Option = Heat Transfer Coefficient
END
INTERPHASE TRANSFER MODEL:
Option = Free Surface
END
MASS TRANSFER:
Option = None
END
SURFACE TENSION MODEL:
Option = Continuum Surface Force
Primary Fluid = Diesel
END
END
MULTIPHASE MODELS:
Homogeneous Model = On
FREE SURFACE MODEL:
Option = Standard
END
END
END
INITIALISATION:
Option = Automatic
FLUID: Air
INITIAL CONDITIONS:
TEMPERATURE:
Option = Automatic with Value
Temperature = 298 [K]
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = VOFaxialAir
END
END
END
FLUID: Diesel
INITIAL CONDITIONS:
TEMPERATURE:
Option = Automatic with Value
Temperature = 310 [K]
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = VOFaxialDiesel
END
END
END
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = waxial
END
STATIC PRESSURE:
Option = Automatic
END
TURBULENCE INITIAL CONDITIONS:
Option = High Intensity and Eddy Viscosity Ratio
END
END
END
OUTPUT CONTROL:
MONITOR OBJECTS:
MONITOR BALANCES:
Option = Full
END
MONITOR FORCES:
Option = Full
END
MONITOR PARTICLES:
Option = Full
END
MONITOR POINT: massIN
Coord Frame = Coord 0
Expression Value = Diesel.massFlow()@Inlet
Option = Expression
END
MONITOR POINT: massOUT
Coord Frame = Coord 0
Expression Value = Diesel.massFlow()@Opening
Option = Expression
END
MONITOR RESIDUALS:
Option = Full
END
MONITOR TOTALS:
Option = Full
END
END
RESULTS:
File Compression Level = Default
Option = Standard
END
END
SOLVER CONTROL:
Turbulence Numerics = First Order
ADVECTION SCHEME:
Option = Upwind
END
CONVERGENCE CONTROL:
Maximum Number of Iterations = 1000
Minimum Number of Iterations = 1
Physical Timescale = 1e-005 [s]
Timescale Control = Physical Timescale
END
CONVERGENCE CRITERIA:
Conservation Target = 0.01
Residual Target = 1e-04
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
MULTIPHASE CONTROL:
Volume Fraction Coupling = Coupled
END
END
END
COMMAND FILE:
Version = 17.0
Results Version = 17.0
END
SIMULATION CONTROL:
EXECUTION CONTROL:
EXECUTABLE SELECTION:
Double Precision = No
END
PARALLEL HOST LIBRARY:
HOST DEFINITION: bx5005
Remote Host Name = bx500-5
Host Architecture String = linux-amd64
Installation Root = /share/soft/ansys/17.0/v%v/CFX
END
END
PARTITIONER STEP CONTROL:
PARTITIONING TYPE:
Option = MeTiS
MeTiS Type = k-way
Partition Size Rule = Automatic
Partition Weight Factors = 0.12500, 0.12500, 0.12500, 0.12500, \
0.12500, 0.12500, 0.12500, 0.12500
END
END
RUN DEFINITION:
Solver Input File = \
/home/student/SUBMITTED/student.GDF_P6_Sim100.4067/GDF_P6_Sim100.def
Run Mode = Full
Solver Results File = \
/scr/bx500-5/cfx/student/SGE-cfx_GDF_P6_Sim100-212736/cfx_GDF_P6_Sim1\
00_001.res
END
SOLVER STEP CONTROL:
Runtime Priority = Low
PARALLEL ENVIRONMENT:
Start Method = Platform MPI Distributed Parallel
Parallel Host List = bx5005*8
END
END
END
END

[ghorrocks]

Sorry, it looks like I misread your initial question. You are not using the LISA model, you are comparing against the LISA model. Looking at your CCL I see you are using a free surface model and are attempting to match the breakup results from LISA.

Right from the start I see you are modelling this with a steady state model whereas this flow is inherently transient. It is never going to work unless you do a transient model.

Your question is familiar now - it is this thread: Injection Spray into Air with Opening Pressure of 30bar

In this case, my final post on that thread still applies:

To get straight to the point: You appear to be a beginner at CFD with very limited resources (student license, 500k nodes) attempting a simulation which is a big task for an experienced CFD person with access to a supercomputer. To put it bluntly, you are not going to successfully complete this simulation.

That is why I asked the question "why are you doing this?".

If the answer is because my professor told me to - then your professor set an impossible task and you need to get your professor to be realistic.

If the answer is because I thought it would be interesting to simulate it - then you should change it to a more reasonable simulation, for instance reducing the spray pressure/speed as Gert-Jan suggests would be a good approach.

If the answer is because it is part of a machine I am designing which uses this device to spray fluid - then you should look at either the literature for experimental/empirical work on high pressure sprays and estimate the spray performance from there, or use models like the lagrangian spray model in CFD to model the spray process.

[Spray_Ansys]

In my case, it is not necessary to simulate a Lagrangian particle tracking. I want to simulate a steady state flow of a spray (as mentioned in the beginning of this thread). The LISA model I used to estimate the dimensions of my simulation area and ergo of my mesh.

As I mentioned, I want to simulate something in the kind of the youtube video, BUT for steady state flow. My only question is, which way should I approach and what is the importance for such a setup? What should be bared in mind?

Thanks for every help and friendly support.

[ghorrocks]

But you can't simulate spray breakup with a steady state model. It is an inherently transient effect. Anybody who claims to have directly modelled (ie free surface model) using a steady state model is deluded.

I suspect the video link you post is using the Eularian particle model, with the particles defined as liquid drops. The free surface approach you are using is a direct modelling approach which is not going to be possible with the resources you have available to you.

You might be able to model this steady state using a eularian model. I am not sure on that, I would have to research the model to check that. I will that check up to you . The other approach you can model spray breakup steady state is using lagrangian particle tracking but you have already stated you don't want to do that.

[Spray_Ansys]

Thank you for your answer and help ghorrocks!

[ghorrocks]

I have just looked in the CFX Eularian droplet model. I can't find any support for droplet breakup models there, only in the Lagrangian particle tracking. The only spray/droplet breakup model which appears suitable for your case is the Lagrangian particle tracking model.

[Spray_Ansys]

Hi Glenn,
thanks for your answer.

What about this video:
https://www.youtube.com/watch?v=KBYd_O0ucdg&t=185s

Is here the Particle Tracking also the case? If yes, how do you know?

[Gert-Jan]

No. This movie is not Lagrangian particle tracking. It is Eulerian: it treats water as continuous phase with droplet size of 5 mu.
To activate Lagrangian you need to select the water droplets as Particle Transport Fluid.

[Spray_Ansys]

Ok, thank you. This looks suitable for my case.

[Gert-Jan]

But in the youtube example, water is injected at the inlet as droplets of 5 mu with a mass fraction of 1. You could argue whether if that is physically correct, but ok.

In Lagrangian particle tracking, the droplets are point masses. So, they contain no volume. Therefore there is no way you can get a water volume fraction of 1 at the inlet with only particles. You need a supporting gas for the droplets.

[Spray_Ansys]

Originally Posted by Gert-Jan

But in the youtube example, water is injected at the inlet as droplets of 5 mu with a mass fraction of 1. You could argue whether if that is physically correct, but ok.

In Lagrangian particle tracking, the droplets are point masses. So, they contain no volume. Therefore there is no way you can get a water volume fraction of 1 at the inlet with only particles. You need a supporting gas for the droplets.

Ok, thank you very much for your reply Gert-Jan!
I've tried it with a similar setup like in the youtube example. But unfortunately I dont get such a nice spreading like there (see my picture).

My setup is a steady state case, where I expect a spreading of the spray/jet. The Volume Fraction keeps cylindrical and I don't really understand why? What cause such spreading? Did I forget something? I can't find any difference between my setup and the setup of youtube..

[ghorrocks]

If you fire the drops in a straight line, they will stay in a straight line. You need to fire them at the spray angle of your injector to get a spread.

But please remember that the youtube model you show simply has the drops radiating out and the volume fraction decreasing as the drops spread. There is no spray break up in this model. You cannot model spray breakup with this model. The only model in CFX which has a spray breakup model is Lagrangian particle tracking.

If you are trying to model spray breakup, the youtube model you show is not a good example as it does not contain any spray breakup.

[Spray_Ansys]

Thanks for all your help!
Actually, I'm looking for a change in my spray / jet stream, since in my opinion, it isn't realistic that the spray keeps that straight over a length of 200mm. I'm trying to get some sort of spreading or inequalities on the stream surface. At the moment, I'm searching my error.

Just for recapitulation:
So, to simulate a steady state spray situation with water and air as ideal gas (both as continuous fluid)
- NO Homogeneous Model
- NO Free Surface Model
- Interphase Transfer: Mixture Model
- Volume Fraction Coupling: Coupled
should be a more or less good way to setup the simulation, right?
Or are there any other suggestions / points to look at?

Thanks for help, once again!

[ghorrocks]

You really need to understand the models before you can choose a physical model. All physical models have compromises, so you need to work out which compromise is the best for you - and then means you need to understand exactly what you are trying to do.

You have three main choices that I can see:
* homogeneous free surface model (which is what you appear to be using when you started this discussion): This will give you a direct model of the spray and breakup process. The compromise here is that it will require a supercomputer to run and years of development and CFD experience to get working accurately.
* Eularian particle model (which is what you appear to be using now): quick and easy to model, and will give a steady state result. The compromise here is that it will not model spray break up, so the drops will stay constant size.
* Lagrangian particle model: A bit trickier to set up than the Eularian model but not too hard. Should run reasonably quickly as well. Has a number of spray ejection and spray breakup models available using various models developed for IC engine fuel injectors. The compromise here is.... not much really. It should be able to model everything I am aware you wish to model and be manageable on a modest sized computer.

This is why all along I have been recommending the Lagrangian particle tracking model.

[Spray_Ansys]

Originally Posted by ghorrocks

homogeneous free surface model (which is what you appear to be using when you started this discussion): This will give you a direct model of the spray and breakup process. The compromise here is that it will require a supercomputer to run and years of development and CFD experience to get working accurately.

I've already tried this way and unfortunately the flow keeps cylindrical over 200mm although I have a supercomputer available. Would you like to have a look on my .out-file? Maybe you will discover the setup fault.

[ghorrocks]

The Lagrangian Particle tracking model is the ONLY model which is going to do what you appear to want it to do in the resources you have available.

[ghorrocks]

Alternatively: If you considered moving to Fluent they have lots more models which would be useful for you. Here is an ANSYS webinar which goes into it: http://view.email.ansys.com/?qs=d647...6be9913ef0a43f

[Spray_Ansys]

Ok, I tried it to setup with Particle Tracking. Hope it will finally work now..