
[Sponsors] 
Overflow Error in Multiphase Modelling with Two Continuous Fluids 

LinkBack  Thread Tools  Search this Thread  Display Modes 
August 11, 2014, 03:52 
Overflow Error in Multiphase Modelling with Two Continuous Fluids

#1 
Senior Member
Ashkan Javadzadegan
Join Date: Sep 2010
Posts: 255
Rep Power: 12 
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.E4 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. 

August 11, 2014, 05:51 

#2 
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10 
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. 

August 11, 2014, 06:09 

#3 
Senior Member
Ashkan Javadzadegan
Join Date: Sep 2010
Posts: 255
Rep Power: 12 
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. 

August 11, 2014, 06:50 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,805
Rep Power: 122 
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? 

August 11, 2014, 07:00 

#5 
Senior Member
Ashkan Javadzadegan
Join Date: Sep 2010
Posts: 255
Rep Power: 12 
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. 

August 11, 2014, 08:40 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,805
Rep Power: 122 
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.


August 11, 2014, 14:32 

#7  
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10 
Quote:


Thread Tools  Search this Thread 
Display Modes  


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 