
[Sponsors] 
Simulation of a single bubble with a VOFmethod 

LinkBack  Thread Tools  Search this Thread  Display Modes 
April 28, 2009, 05:52 
Simulation of a single bubble with a VOFmethod

#1 
Member
Susann
Join Date: Apr 2009
Location: Dresden
Posts: 33
Rep Power: 15 
Hellow there,
I'm dealing with the topic of air bubbles ascending in stagnant water. When i was trying to simulate a bubble with 4 mm in diameter in a rectangular 2D column of 40 mm width and 100 mm height with a grid size of 0.125 mm (as recommended in a paper called "Simulating the motion of gas bubbles in a liquid" by Krishna, you can find it here http://ctcr4.chem.uva.nl/ ), the results first looked pretty well, but after a timestep of 10500 ( time steps = 10e05 s ) the bubble abruptly breaks up. And I have the problem that the inner pressure field inside of the bubble is not developing. There is always the same pressure as in the surrounding water. I used a uniform cartesiancoordinate grid. The front and rear faces of the column are modelled as symmetry planes and at the two walls the noslip boundary condition is imposed. I used the homogenous model and the free surface model. I initialized the interface by using a stepfunctionexpression that defines a circle near the lower bound of the domain. Then i smeared the interface by using a User Function so that CFX can handle the interface numerically in a better way. I used double precision to solve it....to make it short here the cclfile: # State file created: 2009/04/28 11:42:47 # CFX11.0 build 2006.11.1722.59 FLOW: DOMAIN:Fluids Coord Frame = Coord 0 Domain Type = Fluid Fluids List = Air at 25 C,Water Location = Assembly BOUNDARY:Opening Boundary Type = OPENING Location = TOP 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 FLUID:Air at 25 C BOUNDARY CONDITIONS: VOLUME FRACTION: Option = Value Volume Fraction = 0 END END END FLUID:Water BOUNDARY CONDITIONS: VOLUME FRACTION: Option = Value Volume Fraction = 1 END END END END BOUNDARY:Symmetry Boundary Type = SYMMETRY Location = BACK,FRONT END BOUNDARY:Walls Boundary Type = WALL Location = BOTTOM,LEFT,RIGHT BOUNDARY CONDITIONS: WALL INFLUENCE ON FLOW: Option = No Slip END END FLUID PAIR:Air at 25 C  Water BOUNDARY CONDITIONS: WALL ADHESION: Option = None 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 = 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 = 1 [atm] END END FLUID:Air at 25 C FLUID MODELS: FLUID BUOYANCY MODEL: Option = Density Difference END MORPHOLOGY: Minimum Volume Fraction = 10e15 Option = Continuous Fluid END END END FLUID:Water FLUID MODELS: FLUID BUOYANCY MODEL: Option = Density Difference END MORPHOLOGY: Option = Continuous Fluid END END END FLUID MODELS: COMBUSTION MODEL: Option = None END HEAT TRANSFER MODEL: Fluid Temperature = 300 [K] Homogeneous Model = True Option = Isothermal END THERMAL RADIATION MODEL: Option = None END TURBULENCE MODEL: Option = Laminar END END FLUID PAIR:Air at 25 C  Water Surface Tension Coefficient = 0.073 [N m^1] INTERPHASE TRANSFER MODEL: Option = None END MASS TRANSFER: Option = None END SURFACE TENSION MODEL: Curvature Under Relaxation Factor = 0.5 Option = Continuum Surface Force Primary Fluid = Water Volume Fraction Smoothing Type = VolumeWeighted END END INITIALISATION: Option = Automatic FLUID:Air at 25 C INITIAL CONDITIONS: VOLUME FRACTION: Option = Automatic with Value Volume Fraction = VF Init END END END FLUID:Water INITIAL CONDITIONS: VOLUME FRACTION: Option = Automatic with Value Volume Fraction = 1VF Init 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 = 0 [Pa] END END END MULTIPHASE MODELS: Homogeneous Model = On FREE SURFACE MODEL: Interface Compression Level = 2 Option = Standard END END SOURCE POINT:Source Point 1 Cartesian Coordinates = 0.02 [m], 0.005 [m], 0 [m] Option = Cartesian Coordinates END END EXPERT PARAMETERS: ggi permit no intersection = t old surface tension numerics = t 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 = Timestep Interval Timestep Interval = 50 END END END SIMULATION 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 = 2 [s] END TIME STEPS: Option = Timesteps Timesteps = 1e05 [s] END END SOLUTION UNITS: Angle Units = [rad] Length Units = [m] Mass Units = [kg] Solid Angle Units = [sr] Temperature Units = [K] Time Units = [s] END SOLVER CONTROL: ADVECTION SCHEME: Option = High Resolution END BODY FORCES: Body Force Averaging Type = Harmonic END CONVERGENCE CONTROL: Maximum Number of Coefficient Loops = 10 Timescale Control = Coefficient Loops END CONVERGENCE CRITERIA: Residual Target = 1.E4 Residual Type = RMS END MULTIPHASE CONTROL: Volume Fraction Coupling = Coupled END PRESSURE LEVEL INFORMATION: Option = Automatic Pressure Level = 1 [atm] END TRANSIENT SCHEME: Option = Second Order Backward Euler TIMESTEP INITIALISATION: Option = Automatic END END END END LIBRARY: CEL: EXPRESSIONS: VF Init = Verschmierung((2[mm]sqrt((x20[mm] )^2+(y5[mm] )^2))) END FUNCTION:Verschmierung Argument Units = mm Option = Interpolation Result Units = m/m INTERPOLATION DATA: Data Pairs = 0.2,0,0.2,1 Extend Max = On Extend Min = On Option = One Dimensional END 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 ABSORPTION COEFFICIENT: Absorption Coefficient = 0.01 [m^1] Option = Value END DYNAMIC VISCOSITY: Dynamic Viscosity = 1.831E05 [kg m^1 s^1] Option = Value END EQUATION OF STATE: Molar Mass = 28.96 [kg kmol^1] Option = Ideal Gas 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 REFRACTIVE INDEX: Option = Value Refractive Index = 1.0 [m m^1] END SCATTERING COEFFICIENT: Option = Value Scattering Coefficient = 0.0 [m^1] END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 1.0044E+03 [J kg^1 K^1] Specific Heat Type = Constant Pressure END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 2.61E2 [W m^1 K^1] END END END MATERIAL:Water Ideal Gas Material Description = Water Vapour Ideal Gas (100 C and 1 atm) Material Group = Calorically Perfect Ideal Gases, Water Data Option = Pure Substance Thermodynamic State = Gas PROPERTIES: Option = General Material ABSORPTION COEFFICIENT: Absorption Coefficient = 1.0 [m^1] Option = Value END DYNAMIC VISCOSITY: Dynamic Viscosity = 9.4E06 [kg m^1 s^1] Option = Value END EQUATION OF STATE: Molar Mass = 18.02 [kg kmol^1] Option = Ideal Gas END REFERENCE STATE: Option = Specified Point Reference Pressure = 1.014 [bar] Reference Specific Enthalpy = 0. [J/kg] Reference Specific Entropy = 0. [J/kg/K] Reference Temperature = 100 [C] END REFRACTIVE INDEX: Option = Value Refractive Index = 1.0 [m m^1] END SCATTERING COEFFICIENT: Option = Value Scattering Coefficient = 0.0 [m^1] END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 2080.1 [J kg^1 K^1] Specific Heat Type = Constant Pressure END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 193E04 [W m^1 K^1] END END END MATERIAL:Aluminium Material Group = CHT Solids, Particle Solids Option = Pure Substance Thermodynamic State = Solid PROPERTIES: Option = General Material EQUATION OF STATE: Density = 2702 [kg m^3] Molar Mass = 26.98 [kg kmol^1] Option = Value END REFERENCE STATE: Option = Specified Point Reference Specific Enthalpy = 0 [J/kg] Reference Specific Entropy = 0 [J/kg/K] Reference Temperature = 25 [C] END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 9.03E+02 [J kg^1 K^1] END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 237 [W m^1 K^1] END END END MATERIAL:Steel Material Group = CHT Solids, Particle Solids Option = Pure Substance Thermodynamic State = Solid PROPERTIES: Option = General Material EQUATION OF STATE: Density = 7854 [kg m^3] Molar Mass = 55.85 [kg kmol^1] Option = Value END REFERENCE STATE: Option = Specified Point Reference Specific Enthalpy = 0 [J/kg] Reference Specific Entropy = 0 [J/kg/K] Reference Temperature = 25 [C] END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 4.34E+02 [J kg^1 K^1] END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 60.5 [W m^1 K^1] END END END MATERIAL:Copper Material Group = CHT Solids, Particle Solids Option = Pure Substance Thermodynamic State = Solid PROPERTIES: Option = General Material EQUATION OF STATE: Density = 8933 [kg m^3] Molar Mass = 63.55 [kg kmol^1] Option = Value END REFERENCE STATE: Option = Specified Point Reference Specific Enthalpy = 0 [J/kg] Reference Specific Entropy = 0 [J/kg/K] Reference Temperature = 25 [C] END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 3.85E+02 [J kg^1 K^1] END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 401.0 [W m^1 K^1] END END END MATERIAL:Soot Material Group = Soot Option = Pure Substance Thermodynamic State = Solid PROPERTIES: Option = General Material ABSORPTION COEFFICIENT: Absorption Coefficient = 0 [m^1] Option = Value END EQUATION OF STATE: Density = 2000 [kg m^3] Molar Mass = 12 [kg kmol^1] Option = Value END REFERENCE STATE: Option = Automatic END 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 Thermal Expansivity = 0.003356 [K^1] ABSORPTION COEFFICIENT: Absorption Coefficient = 0.01 [m^1] Option = Value END DYNAMIC VISCOSITY: Dynamic Viscosity = 1.831E05 [kg m^1 s^1] Option = Value END EQUATION OF STATE: Density = 1.185 [kg m^3] Molar Mass = 28.96 [kg kmol^1] Option = Value 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 REFRACTIVE INDEX: Option = Value Refractive Index = 1.0 [m m^1] END SCATTERING COEFFICIENT: Option = Value Scattering Coefficient = 0.0 [m^1] END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 1.0044E+03 [J kg^1 K^1] Specific Heat Type = Constant Pressure END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 2.61E02 [W m^1 K^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 Thermal Expansivity = 2.57E04 [K^1] ABSORPTION COEFFICIENT: Absorption Coefficient = 1.0 [m^1] Option = Value END DYNAMIC VISCOSITY: Dynamic Viscosity = 8.899E4 [kg m^1 s^1] Option = Value END EQUATION OF STATE: Density = 997.0 [kg m^3] Molar Mass = 18.02 [kg kmol^1] Option = Value 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 REFRACTIVE INDEX: Option = Value Refractive Index = 1.0 [m m^1] END SCATTERING COEFFICIENT: Option = Value Scattering Coefficient = 0.0 [m^1] END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 4181.7 [J kg^1 K^1] Specific Heat Type = Constant Pressure END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 0.6069 [W m^1 K^1] END END END I hope there is anybody out there who tried the bubble simulation a bit more successfully than i did......i would be very thankful about some help and hints.....blubb 

April 29, 2009, 19:28 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
Hi:
Some comments: Why have you set "ggi permit no intersection = t" and "old surface tension numerics = t". Unless you have a specific reason to set them I would return to the defaults. Turn volume fraction smoothing to "none" Use adaptive timestepping, adapting to give 36 iterations per timestep. With surface tension modelling you have to use MUCH smaller timesteps than otherwise (and much smaller than you probably expect). Glenn Horrocks 

April 30, 2009, 05:05 

#3 
Member
Susann
Join Date: Apr 2009
Location: Dresden
Posts: 33
Rep Power: 15 
Thanks ghorrocks,
i set the old surface tension numerics=t because this option reduces the so called spurious currents. That are little eddies that develop near the interface by using a VOFmethod. The ggi permit no intersection=t should have no effect on my simulation as no ggi interface is used for my model. But I returned it to default and now i'm giving the adaptive timestepping a try....the timestep should be fine enough as i found papers about bubble simulations in cfx with the same timestepsize! I'll let u know what happened... 

May 2, 2009, 08:24 

#4 
Member
Susann
Join Date: Apr 2009
Location: Dresden
Posts: 33
Rep Power: 15 
Bad news...adaptive timestepping leads to an even faster breakup. It happens after timestep 3950. I`m really desperate...isn`t there anybody who succeeded in simulating a little single bubble?


May 2, 2009, 08:40 

#5 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
Hi,
Have you tried "Volume Fraction Smoothing = None"? I suggested it because it has caused weird surface behaviour for me before and as long as your mesh is fine enough to resolve the surface nicely you don't need any smoothing (in my experience). Also if you could post some images of the initial condition and bubble breakup that would help. Glenn Horrocks 

May 4, 2009, 06:24 

#6 
Member
Susann
Join Date: Apr 2009
Location: Dresden
Posts: 33
Rep Power: 15 
That are pics from the results of my first settings i've posted...
a ....after 0 timesteps b.... after 4000 timesteps c....after 8000 timesteps d....after 1200 timesteps 

May 4, 2009, 06:28 

#7 
Member
Susann
Join Date: Apr 2009
Location: Dresden
Posts: 33
Rep Power: 15 
And that are pics from the results of adaptive timestepping...the number behind the name of the file shows the timestep...now i`ll try to set the volume fraction smoothing type to none and hope that will work...thanks for your help


May 4, 2009, 07:51 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
Hi,
A finer mesh will definitely help and tighter convergence might also help. You need to establish mesh, timestep and convergence sensitivity for your simulation before it will be accurate. Glenn Horrocks 

May 4, 2009, 08:51 

#9 
Member
Susann
Join Date: Apr 2009
Location: Dresden
Posts: 33
Rep Power: 15 
Which mesh size can you recommend? Until now i`ve worked with a mesh size of 0.125 mm in all directories, so that there are 32 grid cells per bubblediameter and 804 grid cells per bubblecross section...thought this might me fine enough...


May 4, 2009, 20:07 

#10 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
Hi,
A quote from my last post  "You need to establish mesh, timestep and convergence sensitivity for your simulation before it will be accurate." These parameters are all problem dependent so you have to establish it for each case. With a bit of experience you should be able to make a pretty good guess as to the required mesh, timestep and convergence levels required for your work, but if you have not done it yet then you must do it if you want accurate simulations. Glenn Horrocks 

May 6, 2009, 06:02 

#11 
Member
Susann
Join Date: Apr 2009
Location: Dresden
Posts: 33
Rep Power: 15 
Hellowww....me again
Thank u Glenn. Here are the first results with the volume fraction smoothing type set to none...i`m still wondering why the pressure inside the bubble is not developing, there should be a higher pressure than in the surrounding fluid. And additionally there should develop a higher pressure at the front side of the bubble than at the bottom side... Has anybody an idea why it looks that way? Has it something to do with the homogeneous model i`m using? Kind regards Susann 

May 6, 2009, 06:03 

#12 
Member
Susann
Join Date: Apr 2009
Location: Dresden
Posts: 33
Rep Power: 15 
and the rest of the pics...


May 6, 2009, 06:24 

#13 
Senior Member
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 449
Rep Power: 18 
hi,
is it possible to get a higher inner bubble pressure with the homogeneous transport? Homogeneous model means shared velocityfield, so there it could only be the surface tension increasing the inner pressure? Or am i missing smth? neewbie Last edited by mvoss; May 6, 2009 at 07:20. 

May 6, 2009, 07:25 

#14 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
Hi,
I will quote it for the third time. "You need to establish mesh, timestep and convergence sensitivity for your simulation before it will be accurate." If you are having problems with accuracy have you checked that your mesh is fine enough to be accurate, your timestep is OK and you are converging tight enough? I can see from your volume fraction plot you have a relatively coarse mesh so you will be heaps more accurate with a finer mesh. Also surface tension models often require double precision to run well. I would turn double precision on anyway just to be sure. Also to see the pressure effects you will have to zoom into the pressure range near the bubble rather than the full range. Or even better look at the pressure without the hydrostatic head component. The pressure effects are likely to be small compared to the hydrostatic head so you will have to be careful to see it. Glenn Horrocks 

September 30, 2009, 13:00 
please help me

#15  
New Member
mehdi
Join Date: Sep 2009
Posts: 3
Rep Power: 14 
hi suzzn
I modeled a bubble of gas in a tube with rectungular cross section at cfx 10. But can you briefly tell me how to apply VOF and multiphase flow in this model? thanks Quote:


September 30, 2009, 19:30 

#16 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
Do the tutorials, and have a look at the CCL you quoted. Also upgrade to V12, it has much improved free surface modelling capbilities.


October 1, 2009, 11:59 

#17 
New Member
mehdi
Join Date: Sep 2009
Posts: 3
Rep Power: 14 
hi
thanks for your help but,I do all of the tutorials, and apply vof and multiphase to my model. my model: a bubble of air modeled by a sphere,and the tube by a box. but i want to move sphere through a tube? what do I do? thanks 

October 1, 2009, 18:36 

#18 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
If the tutorials and descriptions here aren't enough to get you started then I think you need to do a CFX multiphase training course. Talk to your CFX support people about what training courses they offer.


October 2, 2009, 04:18 

#19 
Member

If you have done ALL the tutorials:
 Do again the relevant tutorials for your problem (and try to understand what you're doing)  Try to implement your problem. Start by the simplest possible case.  When asking questions here, you have to give more information about what you have done and what you cannot do (do really think someone is going to understand what you're asking by "I want to move sphere. What do I do?" ? ... and don't say your English is bad, because the your English is perfectly understandable)
__________________
Rui 

January 28, 2018, 07:04 

#20 
New Member
behnam
Join Date: Dec 2017
Posts: 2
Rep Power: 0 
hi
i just try to simulate this ccl file everything goes fine except timestep interval option that i don't have it in my cfx 18 ? what should i do to use that option in output frequency? and in general how should i use that? i search all over net but didn't get much info. look for it in cfx help but it isn't useful. if you have tutorial or any comment i will be thank for that. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
How to apply VOF method?  yeeking86  CFX  7  August 23, 2010 18:24 
About bubble size distribution simulation  tchllc  FLUENT  0  August 12, 2007 04:07 
VOF method on intertank transfer  Louis  FLUENT  0  March 14, 2006 09:28 
Simulation of condensation/evaporation using VOF model in Fluent4.5  Yuwen Zhang  Main CFD Forum  0  April 27, 1999 11:48 
Engine simulation (seeking help with method to use)  Geoff Rathbun  Main CFD Forum  4  April 13, 1999 14:19 