
[Sponsors] 
February 26, 2016, 09:21 
problems at multiphase flows, emptying a bottle

#1 
New Member
Maximilian
Join Date: Feb 2016
Location: RLP, Germany
Posts: 6
Rep Power: 2 
Hallo
i have a problem at multiphase flows simulation with CFX. I would like to simulate the emptying of a bottle which stands on the head and is at a time=0 completely filled with water. I set a opening boundary condition at the outlet with a volume fraction of air=1 (air can flow into the bottle) and water=0 (i hope this means that water can only flows out of the bottle). But the water does not flow out of the bottle (gravity is on an has the right direction). I know that my problem lies at the boundary conditions at the outlet, but i have no idea which kind of boundary condition i must choose in CFX. In principle i need an inlet/outlet boundary condition for both phases at my outlet. Can anybody help me? Told me if more information are needed. thanks and greets Max 

February 27, 2016, 04:39 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Please post an image of what you are modelling and your CCL. Make sure you show where your boundary conditions are located.


February 27, 2016, 12:45 

#3  
New Member
Maximilian
Join Date: Feb 2016
Location: RLP, Germany
Posts: 6
Rep Power: 2 
Quote:
Have i set the reference density wrong or must i switch the air to a disperse phase. Thanks bottle height = 0.228 m bottle neck diameter = 0.017 m CCLFile  LIBRARY: CEL: EXPRESSIONS: iniLiquid = inside()@REGION:LIQUID iniPressure = (1.185997)[kg/m^3]*g*if(y>0.21335[m],(0.228[m]y),y) 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 = 10 [s] END TIME STEPS: Option = Timesteps Timesteps = 0.0005 [s] END END DOMAIN: ControlVolume Coord Frame = Coord 0 Domain Type = Fluid Location = AIR,LIQUID BOUNDARY: WALL Boundary Type = WALL Location = WALL,BOTTOM BOUNDARY CONDITIONS: MASS AND MOMENTUM: Option = No Slip Wall END WALL ROUGHNESS: Option = Smooth Wall END END FLUID PAIR: AIR  LIQUID BOUNDARY CONDITIONS: WALL ADHESION: Option = None END END END END BOUNDARY: outlet Boundary Type = OPENING Location = OPENING 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 TURBULENCE: Option = Medium Intensity and Eddy Viscosity Ratio END END FLUID: AIR BOUNDARY CONDITIONS: VOLUME FRACTION: Option = Value Volume Fraction = 1 END END END FLUID: LIQUID BOUNDARY CONDITIONS: VOLUME FRACTION: Option = Value Volume Fraction = 0 END END END END DOMAIN MODELS: BUOYANCY MODEL: Buoyancy Reference Density = 1.185 [kg m^3] Gravity X Component = 0 [m s^2] Gravity Y Component = g Gravity Z Component = 0 [m s^2] Option = Buoyant BUOYANCY REFERENCE LOCATION: Cartesian Coordinates = 0 [m], 1 [m], 0 [m] Option = Cartesian Coordinates END END DOMAIN MOTION: Option = Stationary END MESH DEFORMATION: Option = None END REFERENCE PRESSURE: Reference Pressure = 1 [atm] END END FLUID DEFINITION: AIR Material = Air at 25 C Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID DEFINITION: LIQUID Material = Water Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID MODELS: COMBUSTION MODEL: Option = None END FLUID: AIR FLUID BUOYANCY MODEL: Option = Density Difference END END FLUID: LIQUID FLUID BUOYANCY MODEL: Option = Density Difference END END HEAT TRANSFER MODEL: Fluid Temperature = 25 [C] Homogeneous Model = True Option = Isothermal END THERMAL RADIATION MODEL: Option = None END TURBULENCE MODEL: Option = RNG k epsilon BUOYANCY TURBULENCE: Option = None END END TURBULENT WALL FUNCTIONS: Option = Scalable END END FLUID PAIR: AIR  LIQUID Surface Tension Coefficient = 0.072 [N m^1] INTERPHASE TRANSFER MODEL: Option = None END MASS TRANSFER: Option = None END SURFACE TENSION MODEL: Option = Continuum Surface Force Primary Fluid = LIQUID Volume Fraction Smoothing Type = VolumeWeighted END END MULTIPHASE MODELS: Homogeneous Model = On FREE SURFACE MODEL: Interface Compression Level = 2 Option = Standard END END END INITIALISATION: Option = Automatic FLUID: AIR INITIAL CONDITIONS: VOLUME FRACTION: Option = Automatic with Value Volume Fraction = 1iniLiquid END END END FLUID: LIQUID INITIAL CONDITIONS: VOLUME FRACTION: Option = Automatic with Value Volume Fraction = iniLiquid 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 = 0 [m s^1] END STATIC PRESSURE: Option = Automatic with Value Relative Pressure = iniPressure END TURBULENCE INITIAL CONDITIONS: Option = Medium Intensity and Eddy Viscosity Ratio END END END OUTPUT CONTROL: RESULTS: File Compression Level = Default Option = Standard END TRANSIENT RESULTS: Transient Results 1 ... END END SOLVER CONTROL: Turbulence Numerics = First Order ADVECTION SCHEME: Option = High Resolution END BODY FORCES: Body Force Averaging Type = Harmonic END CONVERGENCE CONTROL: Maximum Number of Coefficient Loops = 20 Minimum Number of Coefficient Loops = 5 Timescale Control = Coefficient Loops END CONVERGENCE CRITERIA: Residual Target = 0.00001 Residual Type = RMS END MULTIPHASE CONTROL: Volume Fraction Coupling = Coupled END TRANSIENT SCHEME: Option = Second Order Backward Euler TIMESTEP INITIALISATION: Option = Automatic END END END END COMMAND FILE: Version = 14.5 END 

February 28, 2016, 06:12 

#4  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
I have lots of suggestions:
Quote:
Quote:
Quote:
Quote:
Quote:
Quote:
Quote:
A final point: Surface tension models are EXTREMELY sensitive to mesh quality. They are the most sensitive model I know of. You will find your surface tension model starts loosing significant accuracy with hex elements with an aspect ratio of 1.2  this is very hard to achieve. But you should try to mesh your geometry is hex elements with aspect ratio as close to 1 as possible. You really should not do mesh grading when you are using a surface tension model. 

February 28, 2016, 10:22 

#5  
New Member
Maximilian
Join Date: Feb 2016
Location: RLP, Germany
Posts: 6
Rep Power: 2 
Thank you ghorrocks for your help and i try to implement directly your tipps
But i still have some questions. First to the mesh quality: I use triangles as cell with a constant growth rate of 1, because this is only a test case. My original geometry is more complex and only with triangles justifiable. I've found out that when i try to dissolve my boundary layer leads that to a smearing in that region. Is it generally better to pass up or the transition from cell to cell must be better? Surface tension coefficent Are you sure? At my script and at wikipedia you can find for the surface coefficient for water/air PHP Code:
Surface tension Model Quote:
Turbulence model You're right the flow is laminar and not turbulent. I've chosen the wrong model. But when my flow becomes turbulent is the SSTModel really better? In some publications i found for the VoFMethod, that the RNGkModel would be better (at least for FLUENT)? 

February 28, 2016, 17:56 

#6  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Quote:
My comment about the surface tension model details was that often changing the defaults improves simulation speed and accuracy. But it is highly problem dependant so you will have to try the options and find out for yourself which ones help your case. Turbulence mode choice: For laminar flow use a laminar model. So far so good. But which model for a turbulent flow? I would recommend researching that in the literature and see what other researchers have found. You are not the first person to model this type of flow. 

February 29, 2016, 10:28 

#7 
New Member
Maximilian
Join Date: Feb 2016
Location: RLP, Germany
Posts: 6
Rep Power: 2 
I've made a comparison between a "quasi" 2D oscillation rod with a hexa and a tetra mesh similar to this
PHP Code:
P.S. Thank you for your tip with adaptive timestep it runs more faster and just as stable 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Choose of the good multiphase flows model  Miki12  Main CFD Forum  1  June 4, 2014 02:33 
Low Mach Number Compressible Multiphase Flows  DarrenC  CFX  10  May 26, 2014 08:52 
Difference of multicomponent and multiphase homogenous flows  Luk_Fiz  CFX  11  April 4, 2013 05:29 
Multiphase and FreeSurface Flows at OpenFOAM Workshop Milan 2008  egp  OpenFOAM  0  March 20, 2008 07:34 
Editting section on Multiphase flows  Sam  CFDWiki  1  April 26, 2007 14:50 