problems at multiphase flows, emptying a bottle
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 |
Please post an image of what you are modelling and your CCL. Make sure you show where your boundary conditions are located.
|
1 Attachment(s)
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 CCL-File ------------------------------------------------------------------------- LIBRARY: CEL: EXPRESSIONS: iniLiquid = inside()@REGION:LIQUID iniPressure = (1.185-997)[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 = Volume-Weighted 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 = 1-iniLiquid 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 |
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. |
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. |
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 |
All times are GMT -4. The time now is 02:41. |