CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

problems at multiphase flows, emptying a bottle

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   February 26, 2016, 09:21
Default problems at multiphase flows, emptying a bottle
  #1
mvo
New Member
 
Maximilian
Join Date: Feb 2016
Location: RLP, Germany
Posts: 6
Rep Power: 2
mvo is on a distinguished road
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
mvo is offline   Reply With Quote

Old   February 27, 2016, 04:39
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Please post an image of what you are modelling and your CCL. Make sure you show where your boundary conditions are located.
ghorrocks is offline   Reply With Quote

Old   February 27, 2016, 12:45
Default
  #3
mvo
New Member
 
Maximilian
Join Date: Feb 2016
Location: RLP, Germany
Posts: 6
Rep Power: 2
mvo is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Please post an image of what you are modelling and your CCL. Make sure you show where your boundary conditions are located.
I progressed with my simulation. The liquid is drained out of the bottle neck but i think the settings of my simulation are currently wrong. Since the bubbles not really rise up? However i'm not sure, because i'm with my simulation at a time of 0.5s.
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
Attached Images
File Type: png 0dot48seconds.png (194.8 KB, 19 views)
mvo is offline   Reply With Quote

Old   February 28, 2016, 06:12
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I have lots of suggestions:

Quote:
Timesteps = 0.0005 [s]
Unless you have done a careful validation study to show this time step size is correct then this will be wrong. The recommended approach (especially in this case - I will explain later) is to use adaptive time steps, homing in on 3-5 coeff loops per iteration. Make sure the max and min time step size are wide enough that you never hit them.


Quote:
Surface Tension Coefficient = 0.072 [N m^-1]
This is for pure water. Are you modelling pure water or something else? Any surface active additive will dramatically reduce this.


Quote:
TURBULENCE MODEL:
Option = RNG k epsilon
Is this model really turbulent? I suspect it is not. If it is turbulent then it will be a low Re turbulence and RNG is not a suitable model for that. If the model is laminar then use the laminar turbulence model, if it is turbulent then use SST as it handle low Re flow much better.


Quote:
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
.....
BODY FORCES:
Body Force Averaging Type = Harmonic
END
Modifications to thee defaults can make major differences in surface tension models. I recommend you try some alternate options for these parameters as others might work better.

Quote:
CONVERGENCE CONTROL:
Maximum Number of Coefficient Loops = 20
Minimum Number of Coefficient Loops = 5
Timescale Control = Coefficient Loops
END
These are bad settings. Set minimum = 1 and Max =10. Then use the adaptive time steps to home in on 3-5 coeff loops. You want lots of short time steps which you converge quickly - especially for a surface tension model like this.

Quote:
CONVERGENCE CRITERIA:
Residual Target = 0.00001
Residual Type = RMS
END
This is very tight, you almost certainly can loosen this. With adaptive time stepping as you loosen the convergence criteria you automatically get bigger time steps and then you solve faster - so getting the convergence tolerance correct is important. I recommend you do a sensitivity study on convergence tolerance.

Quote:
TRANSIENT SCHEME:
Option = Second Order Backward Euler
It is likely your time steps are going to be so small that the difference between first and second order is insignificant. Check this, and if so just go back to first order.



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.
ghorrocks is offline   Reply With Quote

Old   February 28, 2016, 10:22
Default
  #5
mvo
New Member
 
Maximilian
Join Date: Feb 2016
Location: RLP, Germany
Posts: 6
Rep Power: 2
mvo is on a distinguished road
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:
https://en.wikipedia.org/wiki/Surface-tension_values 
. For the real problem is it oil with a surface coefficient of 0.03008 [N/m] for the combi oil / air.

Surface tension Model
Quote:
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
.....
BODY FORCES:
Body Force Averaging Type = Harmonic
END
Did you mean that it's better not to choose: Volume Fraction Smoothing Type, Interface Compression Level and Body Force Averaging Type?

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 SST-Model really better? In some publications i found for the VoF-Method, that the RNG-k-\epsilon-Model would be better (at least for FLUENT)?
mvo is offline   Reply With Quote

Old   February 28, 2016, 17:56
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
I use triangles as cell
You will not get good surface tension accuracy with tets or inflation layers. If you do not believe me, try modelling the laplacian pressure of a spherical bubble. You define the initial condition as a sphere and see how close to the analytical bubble pressure the surface tension gets you. Give it a try and find out for yourself.

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.
ghorrocks is offline   Reply With Quote

Old   February 29, 2016, 10:28
Default
  #7
mvo
New Member
 
Maximilian
Join Date: Feb 2016
Location: RLP, Germany
Posts: 6
Rep Power: 2
mvo is on a distinguished road
I've made a comparison between a "quasi" 2D oscillation rod with a hexa and a tetra mesh similar to this
PHP Code:
http://ainastran.org/staticassets/ANSYS/staticassets/resourcelibrary/confpaper/2006-Int-ANSYS-Conf-192.pdf 
for checking the surface tension. I know that a hexa grid shows a better solution but unfortunately for the real geometry which i need it is easier to simulate with tetra.

P.S. Thank you for your tip with adaptive timestep it runs more faster and just as stable
mvo is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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 CFD-Wiki 1 April 26, 2007 14:50


All times are GMT -4. The time now is 08:13.