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

Overflow Error in Multiphase Modelling with Two Continuous Fluids

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 11, 2014, 03:52
Question Overflow Error in Multiphase Modelling with Two Continuous Fluids
  #1
Senior Member
 
Ashkan Javadzadegan
Join Date: Sep 2010
Posts: 255
Rep Power: 12
ashtonJ is on a distinguished road
Dear all,

I am trying to model the mixing of two liquids (foam & blood) in a varicose vein (please see the attached image). The model consists of two parts; needle and vein. Liquid 1 (foam; density: 210 kg/m3 and viscosity: 63400 mPa.s) flows with velocity of 188 [cm/s] in the needle and enters the vein which initially contains stationary blood (Liquid 2) with density and viscosity of 993.72 kg/m3 and 1.42 mPa.s.
I get an overflow error at the first iteration. I’ve read through the FAQ and previous comments on “Overflow” and tested several ways such as double precision, changing the turbulent model to SST, using small physical time steps in steady modelling, checking the boundary conditions and …. But none of them has helped so far and I am still stuck with this error at the beginning of my simulation.
I would be too pleased if anybody have a look at my following CCL file and let me know what the problem is.


FLOW: Flow Analysis 1
ANALYSIS TYPE:
Option = Steady State
EXTERNAL SOLVER COUPLING:
Option = None
END
END
DOMAIN: Needle
Coord Frame = Coord 0
Domain Type = Fluid
Location = needle
BOUNDARY: Default Fluid Fluid Interface Side 1
Boundary Type = INTERFACE
Location = Primitive 2D A
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Inlet
Boundary Type = INLET
Location = Needle_inlet
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Fluid Velocity
END
TURBULENCE:
Option = Fluid Dependent
END
END
FLUID: Blood
BOUNDARY CONDITIONS:
TURBULENCE:
Option = Zero Gradient
END
VELOCITY:
Normal Speed = 0 [cm s^-1]
Option = Normal Speed
END
VOLUME FRACTION:
Option = Value
Volume Fraction = 0
END
END
END
FLUID: Foam
BOUNDARY CONDITIONS:
TURBULENCE:
Option = Zero Gradient
END
VELOCITY:
Normal Speed = 188 [cm s^-1]
Option = Normal Speed
END
VOLUME FRACTION:
Option = Value
Volume Fraction = 1
END
END
END
END
BOUNDARY: Needle Symmetry
Boundary Type = SYMMETRY
Location = symmetry needle
END
BOUNDARY: Needle Wall
Boundary Type = WALL
Location = wall needle
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL CONTACT MODEL:
Option = Use Volume Fraction
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 210 [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 DEFINITION: Blood
Material = Blood
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: Foam
Material = Foam
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
FLUID: Blood
FLUID BUOYANCY MODEL:
Option = Density Difference
END
TURBULENCE MODEL:
Option = SST
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
FLUID: Foam
FLUID BUOYANCY MODEL:
Option = Density Difference
END
TURBULENCE MODEL:
Option = SST
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
HEAT TRANSFER MODEL:
Homogeneous Model = False
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Homogeneous Model = False
Option = Fluid Dependent
END
END
FLUID PAIR: Blood | Foam
INTERPHASE TRANSFER MODEL:
Interface Length Scale = 1. [mm]
Option = Mixture Model
END
MASS TRANSFER:
Option = None
END
MOMENTUM TRANSFER:
DRAG FORCE:
Drag Coefficient = 0.44
Option = Drag Coefficient
END
END
END
INITIALISATION:
Option = Automatic
FLUID: Blood
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic
END
TURBULENCE INITIAL CONDITIONS:
Option = Low Intensity and Eddy Viscosity Ratio
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 0
END
END
END
FLUID: Foam
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic
END
TURBULENCE INITIAL CONDITIONS:
Option = Low Intensity and Eddy Viscosity Ratio
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 1
END
END
END
INITIAL CONDITIONS:
STATIC PRESSURE:
Option = Automatic
END
END
END
MULTIPHASE MODELS:
Homogeneous Model = False
FREE SURFACE MODEL:
Option = None
END
END
END
DOMAIN: Vein
Coord Frame = Coord 0
Domain Type = Fluid
Location = vein
BOUNDARY: Default Fluid Fluid Interface Side 2
Boundary Type = INTERFACE
Location = Primitive 2D
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Outlet
Boundary Type = OUTLET
Location = pressure_outlet
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Average Static Pressure
Pressure Profile Blend = 0.05
Relative Pressure = 0 [mm Hg]
END
PRESSURE AVERAGING:
Option = Average Over Whole Outlet
END
END
END
BOUNDARY: Vein Symmetry
Boundary Type = SYMMETRY
Location = symmetry vein
END
BOUNDARY: Vein Wall
Boundary Type = WALL
Location = wall vein
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL CONTACT MODEL:
Option = Use Volume Fraction
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 210 [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 DEFINITION: Blood
Material = Blood
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: Foam
Material = Foam
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
FLUID: Blood
FLUID BUOYANCY MODEL:
Option = Density Difference
END
TURBULENCE MODEL:
Option = SST
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
FLUID: Foam
FLUID BUOYANCY MODEL:
Option = Density Difference
END
TURBULENCE MODEL:
Option = SST
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
HEAT TRANSFER MODEL:
Homogeneous Model = False
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Homogeneous Model = False
Option = Fluid Dependent
END
END
FLUID PAIR: Blood | Foam
INTERPHASE TRANSFER MODEL:
Interface Length Scale = 1. [mm]
Option = Mixture Model
END
MASS TRANSFER:
Option = None
END
MOMENTUM TRANSFER:
DRAG FORCE:
Drag Coefficient = 0.44
Option = Drag Coefficient
END
END
END
INITIALISATION:
Option = Automatic
FLUID: Blood
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic
END
TURBULENCE INITIAL CONDITIONS:
Option = Low Intensity and Eddy Viscosity Ratio
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 1
END
END
END
FLUID: Foam
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic
END
TURBULENCE INITIAL CONDITIONS:
Option = Low Intensity and Eddy Viscosity Ratio
END
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 0
END
END
END
INITIAL CONDITIONS:
STATIC PRESSURE:
Option = Automatic
END
END
END
MULTIPHASE MODELS:
Homogeneous Model = False
FREE SURFACE MODEL:
Option = None
END
END
END
DOMAIN INTERFACE: Default Fluid Fluid Interface
Boundary List1 = Default Fluid Fluid Interface Side 1
Boundary List2 = Default Fluid Fluid Interface Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = None
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
PITCH CHANGE:
Option = None
END
END
MESH CONNECTION:
Option = GGI
END
END
OUTPUT CONTROL:
RESULTS:
File Compression Level = Default
Option = Standard
END
END
SOLVER CONTROL:
Turbulence Numerics = First Order
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Length Scale Option = Conservative
Maximum Number of Iterations = 1000
Minimum Number of Iterations = 1
Timescale Control = Auto Timescale
Timescale Factor = 1.0
END
CONVERGENCE CRITERIA:
Residual Target = 1.E-4
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
MULTIPHASE CONTROL:
Volume Fraction Coupling = Coupled
END
END
EXPERT PARAMETERS:
outer loop relaxations default = 0.45
END
END
COMMAND FILE:
Version = 15.0
END

Thank you.
Attached Images
File Type: jpg Varicose Vein.jpg (49.4 KB, 28 views)
ashtonJ is offline   Reply With Quote

Old   August 11, 2014, 05:51
Default
  #2
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10
JuPa is on a distinguished road
In my opinion: first off, forget blood, forget foam, does your setup work with water?

Secondly I note you're using the mixture model, with an interface lengths scale of 1 mm. How did you come to this?

Thirdlt you are using interfaces. Describe them to me.
JuPa is offline   Reply With Quote

Old   August 11, 2014, 06:09
Default
  #3
Senior Member
 
Ashkan Javadzadegan
Join Date: Sep 2010
Posts: 255
Rep Power: 12
ashtonJ is on a distinguished road
Thanks Ricochet.
I tried with water, it worked with automatic initial condition; however, when I use automatic initial condition with value, I get the same overflow error. As needle initially contains only Liquid 1, lets say water, and vein contains only stationary blood, therefore in initial condition for needle I specified 1 for volume fraction of water and 0 for volume fraction of blood. In contrast, I set volume fraction 0 for water and 1 for blood in the vein as the initial condition. In this case, I get overflow error at the first iteration.
I read through the CFX documents and could not find a detailed description of length scale, so I used the default value, which is 1 mm.
My model consists of two parts, needle and vein. The interface is where these two parts connect to each other.
ashtonJ is offline   Reply With Quote

Old   August 11, 2014, 06:50
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,805
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You seem to have missed the most important point in the overflow FAQ: mesh quality. I bet your mesh quality is not as good as it could be and improving it will assist greatly. It always does.

Can you post an image of your mesh near the junctions?
ghorrocks is offline   Reply With Quote

Old   August 11, 2014, 07:00
Default
  #5
Senior Member
 
Ashkan Javadzadegan
Join Date: Sep 2010
Posts: 255
Rep Power: 12
ashtonJ is on a distinguished road
Thanks Glenn. You are right.
However, this model was already used by a friend of mine who could converge it using Fluent. I am using the same model with the same mesh topology, however I use CFX as the solver and the fluids properties in my model are different than the ones used by him.
ashtonJ is offline   Reply With Quote

Old   August 11, 2014, 08:40
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,805
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Don't forget the key differences between CFX and Fluent: Fluent's default differencing is upwind which is highly diffusive and can smooth over these sort of things (at the expense of simulation accuracy); and the segregated solver in Fluent may well be different in convergence behaviour than CFX's coupled solver.
ghorrocks is offline   Reply With Quote

Old   August 11, 2014, 14:32
Default
  #7
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10
JuPa is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Don't forget the key differences between CFX and Fluent: Fluent's default differencing is upwind which is highly diffusive and can smooth over these sort of things (at the expense of simulation accuracy); and the segregated solver in Fluent may well be different in convergence behaviour than CFX's coupled solver.
Also it's worth mentioning by default volume fractions in CFX are segregated. Coupling volume fractions with the pressure and velocity matrix can aid convergence.
JuPa is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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
multiphase modelling Sumeet FLUENT 12 February 24, 2017 02:38
Multiphase flow with two continuous fluids and one dispersed fluid ashtonJ CFX 5 July 25, 2014 06:31
Multiphase modelling using Fluent VOF: Solver settings akash FLUENT 0 February 22, 2013 06:29
Multiphase Upwards flow modelling sebasmagri OpenFOAM Running, Solving & CFD 0 January 1, 2012 13:56
three fluids modelling P Hsieh Main CFD Forum 4 March 7, 2001 02:18


All times are GMT -4. The time now is 09:23.