Error in Two phase (condensation) modeling

adilsyyed · June 22, 2015, 20:39

I am modeling direct contact condensation in nozzle-tank arrangement.
The tank is filled with water at 30 degree Celsius and the nozzle is used to inject saturated steam at 2 bar absolute.
I am using thermal phase change model.

I have tried many things but the solver still give error.

It runs normally for more than 300 iterations converging slowly, and out of nowhere sudden peaks in residuals happens and solver gives error.

I have tried everything in the FAQ, but still no success.
I have used a variety of meshes, very small timescale, played with boundary conditions, initial conditions and what not.

PS, single phase simulation converges just fine in the same arrangement.

I could really use some help regarding pin pointing the source of the error.

ghorrocks · June 23, 2015, 03:16

Is this steady state or transient?

This sounds like a tricky simulation to me - compressible flow with phase change.

I would run the simulation generating a results file every timestep/coeff loop (or at least the ones just before it crashes). Have a look at what happens around the time it crashes - does some steam first hit the outlet boundary? Does some water backflow into the nozzle? Does a water vapour bubble collapse?

adilsyyed · June 23, 2015, 05:21

Quote:

Originally Posted by ghorrocks

Is this steady state or transient?

This sounds like a tricky simulation to me - compressible flow with phase change.

I would run the simulation generating a results file every timestep/coeff loop (or at least the ones just before it crashes). Have a look at what happens around the time it crashes - does some steam first hit the outlet boundary? Does some water backflow into the nozzle? Does a water vapour bubble collapse?

This is a steady state analysis, I would do transient analysis after that.

I switched from opening boundary condition to Outlet boundary condition and now the solver doesn't crash, but doesn't converge either.

The rate of convergence is 1 for all equations for a 1000 iterations now. I should think of it as a step in the right direction, right?

ghorrocks · June 23, 2015, 07:09

Quote:

a step in the right direction, right?

It is too early to tell.

Firstly - did you read my previous post? Unless you have a look at what is happening you are just guessing.

Secondly - it is quite likely this flow is transient and no steady state answer is possible. The FAQ talks about this.

Finally - if you want us to help you you need to provide more information. Please post your CCL and some images of the flow you are getting and the mesh you are using.

adilsyyed · June 23, 2015, 21:36

You were right, thanks. I gave Steam volume fraction at Opening/outlet to be zero as boundary condition. When steam reaches the boundary, the solver crashes, or at least that is my interpretation. Because I removed that condition and the error disappeared.

Now my solver is running but the solution neither converges nor diverges.

Code:

  LIBRARY:
   MATERIAL: H2O
     Material Description = Water Vapour
     Material Group = Gas Phase Combustion,Interphase Mass Transfer,Water Data
     Option = Pure Substance
     Thermodynamic State = Gas
     PROPERTIES:
       Option = General Material
       EQUATION OF STATE:
         Molar Mass = 18.02 [kg kmol^-1]
         Option = Ideal Gas
       END
       SPECIFIC HEAT CAPACITY:
         Option = NASA Format
         LOWER INTERVAL COEFFICIENTS:
           NASA a1 = 0.03386842E+02 []
           NASA a2 = 0.03474982E-01 [K^-1]
           NASA a3 = -0.06354696E-04 [K^-2]
           NASA a4 = 0.06968581E-07 [K^-3]
           NASA a5 = -0.02506588E-10 [K^-4]
           NASA a6 = -0.03020811E+06 [K]
           NASA a7 = 0.02590233E+02 []
         END
         TEMPERATURE LIMITS:
           Lower Temperature = 300 [K]
           Midpoint Temperature = 1000 [K]
           Upper Temperature = 5000 [K]
         END
         UPPER INTERVAL COEFFICIENTS:
           NASA a1 = 0.02672146E+02 []
           NASA a2 = 0.03056293E-01 [K^-1]
           NASA a3 = -0.08730260E-05 [K^-2]
           NASA a4 = 0.01200996E-08 [K^-3]
           NASA a5 = -0.06391618E-13 [K^-4]
           NASA a6 = -0.02989921E+06 [K]
           NASA a7 = 0.06862817E+02 []
         END
       END
       REFERENCE STATE:
         Option = NASA Format
         Reference Pressure = 1 [atm]
         Reference Temperature = 25 [C]
       END
       DYNAMIC VISCOSITY:
         Dynamic Viscosity = 9.4E-06 [kg m^-1 s^-1]
         Option = Value
       END
       THERMAL CONDUCTIVITY:
         Option = Value
         Thermal Conductivity = 193E-04 [W m^-1 K^-1]
       END
       ABSORPTION COEFFICIENT:
         Absorption Coefficient = 1.0 [m^-1]
         Option = Value
       END
       SCATTERING COEFFICIENT:
         Option = Value
         Scattering Coefficient = 0.0 [m^-1]
       END
       REFRACTIVE INDEX:
         Option = Value
         Refractive Index = 1.0 [m m^-1]
       END
     END
   END
   MATERIAL: H2Ol
     Material Description = Water Liquid (H2O)
     Material Group = Interphase Mass Transfer, Liquid Phase Combustion, \
       Water Data
     Option = Pure Substance
     Thermodynamic State = Liquid
     PROPERTIES:
       Option = General Material
       EQUATION OF STATE:
         Density = 958.37 [kg/m^3]
         Molar Mass = 18.02 [kg kmol^-1]
         Option = Value
       END
       SPECIFIC HEAT CAPACITY:
         Option = Value
         Specific Heat Capacity = 4215.6 [J/kg/K]
         Specific Heat Type = Constant Pressure
       END
       REFERENCE STATE:
         Option = Specified Point
         Reference Pressure = 3.169 [kPa]
         Reference Specific Enthalpy = -15860961.15 [J/kg]
         Reference Specific Entropy = 2824.82 [J/kg/K]
         Reference Temperature = 298.15 [K]
       END
       DYNAMIC VISCOSITY:
         Dynamic Viscosity = 0.00028182 [Pa s]
         Option = Value
       END
       THERMAL CONDUCTIVITY:
         Option = Value
         Thermal Conductivity = 0.67908 [W m^-1 K^-1]
       END
       ABSORPTION COEFFICIENT:
         Absorption Coefficient = 1 [m^-1]
         Option = Value
       END
       SCATTERING COEFFICIENT:
         Option = Value
         Scattering Coefficient = 0 [m^-1]
       END
       REFRACTIVE INDEX:
         Option = Value
         Refractive Index = 1 [m m^-1]
       END
     END
   END
   MATERIAL: H2Ovl
     Binary Material1 = H2O
     Binary Material2 = H2Ol
     Material Description = Water Mixture (H2O)
     Material Group = Interphase Mass Transfer,Gas Phase Combustion,Liquid \
       Phase Combustion
     Option = Homogeneous Binary Mixture
     SATURATION PROPERTIES:
       Option = General
       PRESSURE:
         Antoine Enthalpic Coefficient B = 1687.54 [K]*ln(10)
         Antoine Pressure Scale = 1 [bar]
         Antoine Reference State Constant A = 5.11564*ln(10)
         Antoine Temperature Offset C = (230.23-273.15) [K]
         Option = Antoine Equation
       END
       TEMPERATURE:
         Option = Automatic
       END
     END
   END
 END
 FLOW: Flow Analysis 1
   SOLUTION UNITS:
     Angle Units = [rad]
     Length Units = [mm]
     Mass Units = [kg]
     Solid Angle Units = [sr]
     Temperature Units = [K]
     Time Units = [s]
   END
   ANALYSIS TYPE:
     Option = Steady State
     EXTERNAL SOLVER COUPLING:
       Option = None
     END
   END
   DOMAIN: Domain Nozzle
     Coord Frame = Coord 0
     Domain Type = Fluid
     Location = B31
     BOUNDARY: Default Fluid Fluid Interface Side 1
       Boundary Type = INTERFACE
       Location = F47.31
       BOUNDARY CONDITIONS:
         HEAT TRANSFER:
           Option = Conservative Interface Flux
         END
         MASS AND MOMENTUM:
           Option = Conservative Interface Flux
         END
         TURBULENCE:
           Option = Conservative Interface Flux
         END
       END
     END
     BOUNDARY: Domain Nozzle Default
       Boundary Type = WALL
       Location = F124.31,F32.31,F33.31
       BOUNDARY CONDITIONS:
         HEAT TRANSFER:
           Option = Adiabatic
         END
         MASS AND MOMENTUM:
           Option = Fluid Dependent
         END
         WALL CONTACT MODEL:
           Option = Use Volume Fraction
         END
         WALL ROUGHNESS:
           Option = Smooth Wall
         END
       END
       FLUID: Steam
         BOUNDARY CONDITIONS:
           MASS AND MOMENTUM:
             Option = No Slip Wall
           END
         END
       END
       FLUID: Water
         BOUNDARY CONDITIONS:
           MASS AND MOMENTUM:
             Option = No Slip Wall
           END
         END
       END
     END
     BOUNDARY: Inlet
       Boundary Type = INLET
       Location = F123.31
       BOUNDARY CONDITIONS:
         FLOW DIRECTION:
           Option = Normal to Boundary Condition
         END
         FLOW REGIME:
           Option = Subsonic
         END
         HEAT TRANSFER:
           Option = Static Temperature
           Static Temperature = 120.212 [C]
         END
         MASS AND MOMENTUM:
           Option = Total Pressure
           Relative Pressure = 2 [bar]
         END
         TURBULENCE:
           Option = Medium Intensity and Eddy Viscosity Ratio
         END
       END
       FLUID: Steam
         BOUNDARY CONDITIONS:
           VOLUME FRACTION:
             Option = Value
             Volume Fraction = 1
           END
         END
       END
       FLUID: Water
         BOUNDARY CONDITIONS:
           VOLUME FRACTION:
             Option = Value
             Volume Fraction = 0
           END
         END
       END
     END
     DOMAIN MODELS:
       BUOYANCY MODEL:
         Buoyancy Reference Density = 998 [kg m^-3]
         Gravity X Component = 0 [mm s^-2]
         Gravity Y Component = -9.8 [m s^-2]
         Gravity Z Component = 0 [mm 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 = 0 [atm]
       END
     END
     FLUID DEFINITION: Steam
       Material = H2O
       Option = Material Library
       MORPHOLOGY:
         Mean Diameter = 1 [mm]
         Option = Dispersed Fluid
       END
     END
     FLUID DEFINITION: Water
       Material = H2Ol
       Option = Material Library
       MORPHOLOGY:
         Option = Continuous Fluid
       END
     END
     FLUID MODELS:
       COMBUSTION MODEL:
         Option = None
       END
       FLUID: Steam
         FLUID BUOYANCY MODEL:
           Option = Density Difference
         END
         TURBULENCE MODEL:
           Option = Dispersed Phase Zero Equation
         END
       END
       FLUID: Water
         FLUID BUOYANCY MODEL:
           Option = Density Difference
         END
         TURBULENCE MODEL:
           Option = k epsilon
           BUOYANCY TURBULENCE:
             Option = None
           END
         END
         TURBULENT WALL FUNCTIONS:
           High Speed Model = Off
           Option = Scalable
         END
       END
       HEAT TRANSFER MODEL:
         Homogeneous Model = Off
         Option = Total Energy
       END
       THERMAL RADIATION MODEL:
         Option = None
       END
       TURBULENCE MODEL:
         Homogeneous Model = False
         Option = Fluid Dependent
       END
     END
     FLUID PAIR: Steam | Water
       INTERPHASE HEAT TRANSFER:
         Option = Two Resistance
         FLUID1 INTERPHASE HEAT TRANSFER:
           Option = Zero Resistance
         END
         FLUID2 INTERPHASE HEAT TRANSFER:
           Option = Ranz Marshall
         END
       END
       INTERPHASE TRANSFER MODEL:
         Option = Particle Model
       END
       MASS TRANSFER:
         Option = Phase Change
         PHASE CHANGE MODEL:
           Option = Thermal Phase Change
         END
       END
       MOMENTUM TRANSFER:
         DRAG FORCE:
           Drag Coefficient = 0.44
           Option = Drag Coefficient
         END
         LIFT FORCE:
           Option = None
         END
         TURBULENT DISPERSION FORCE:
           Option = None
         END
         VIRTUAL MASS FORCE:
           Option = None
         END
         WALL LUBRICATION FORCE:
           Option = None
         END
       END
       TURBULENCE TRANSFER:
         ENHANCED TURBULENCE PRODUCTION MODEL:
           Option = None
         END
       END
     END
     INITIALISATION:
       Option = Automatic
       FLUID: Steam
         INITIAL CONDITIONS:
           Velocity Type = Cartesian
           CARTESIAN VELOCITY COMPONENTS:
             Option = Automatic
           END
           TEMPERATURE:
             Option = Automatic with Value
             Temperature = 120.212 [C]
           END
           VOLUME FRACTION:
             Option = Automatic with Value
             Volume Fraction = 1
           END
         END
       END
       FLUID: Water
         INITIAL CONDITIONS:
           Velocity Type = Cartesian
           CARTESIAN VELOCITY COMPONENTS:
             Option = Automatic with Value
             U = 0 [mm s^-1]
             V = 0 [mm s^-1]
             W = 0 [mm s^-1]
           END
           TEMPERATURE:
             Option = Automatic
           END
           TURBULENCE INITIAL CONDITIONS:
             Option = k and Epsilon
             EPSILON:
               Option = Automatic
             END
             K:
               Option = Automatic
             END
           END
           VOLUME FRACTION:
             Option = Automatic with Value
             Volume Fraction = 0
           END
         END
       END
       INITIAL CONDITIONS:
         STATIC PRESSURE:
           Option = Automatic with Value
           Relative Pressure = 2 [bar]
         END
       END
     END

1.png

adilsyyed · June 23, 2015, 21:37

Code:

MULTIPHASE MODELS:
       Homogeneous Model = Off
       FREE SURFACE MODEL:
         Option = None
       END
     END
   END
   DOMAIN: Domain Tank
     Coord Frame = Coord 0
     Domain Type = Fluid
     Location = B122
     BOUNDARY: Default Fluid Fluid Interface Side 2
       Boundary Type = INTERFACE
       Location = F47.122
       BOUNDARY CONDITIONS:
         HEAT TRANSFER:
           Option = Conservative Interface Flux
         END
         MASS AND MOMENTUM:
           Option = Conservative Interface Flux
         END
         TURBULENCE:
           Option = Conservative Interface Flux
         END
       END
     END
     BOUNDARY: Domain Tank Default
       Boundary Type = WALL
       Location = \
         F100.122,F101.122,F91.122,F92.122,F93.122,F95.122,F96.122,F97.122,F98\
         .122,F99.122
       BOUNDARY CONDITIONS:
         HEAT TRANSFER:
           Option = Adiabatic
         END
         MASS AND MOMENTUM:
           Option = Fluid Dependent
         END
         WALL CONTACT MODEL:
           Option = Use Volume Fraction
         END
         WALL ROUGHNESS:
           Option = Smooth Wall
         END
       END
       FLUID: Steam
         BOUNDARY CONDITIONS:
           MASS AND MOMENTUM:
             Option = No Slip Wall
           END
         END
       END
       FLUID: Water
         BOUNDARY CONDITIONS:
           MASS AND MOMENTUM:
             Option = No Slip Wall
           END
         END
       END
     END
     BOUNDARY: Outlet
       Boundary Type = OPENING
       Location = F94.122
       BOUNDARY CONDITIONS:
         FLOW DIRECTION:
           Option = Normal to Boundary Condition
         END
         FLOW REGIME:
           Option = Subsonic
         END
         HEAT TRANSFER:
           Opening Temperature = 30 [C]
           Option = Opening Temperature
         END
         MASS AND MOMENTUM:
           Option = Opening Pressure and Direction
           Relative Pressure = 1 [atm]
         END
         TURBULENCE:
           Option = Medium Intensity and Eddy Viscosity Ratio
         END
       END
       FLUID: Steam
         BOUNDARY CONDITIONS:
           VOLUME FRACTION:
             Option = Zero Gradient
           END
         END
       END
       FLUID: Water
         BOUNDARY CONDITIONS:
           VOLUME FRACTION:
             Option = Zero Gradient
           END
         END
       END
     END
     DOMAIN MODELS:
       BUOYANCY MODEL:
         Buoyancy Reference Density = 998 [kg m^-3]
         Gravity X Component = 0 [mm s^-2]
         Gravity Y Component = -9.8 [m s^-2]
         Gravity Z Component = 0 [mm 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 = 0 [atm]
       END
     END
     FLUID DEFINITION: Steam
       Material = H2O
       Option = Material Library
       MORPHOLOGY:
         Mean Diameter = 1 [mm]
         Option = Dispersed Fluid
       END
     END
     FLUID DEFINITION: Water
       Material = H2Ol
       Option = Material Library
       MORPHOLOGY:
         Option = Continuous Fluid
       END
     END
     FLUID MODELS:
       COMBUSTION MODEL:
         Option = None
       END
       FLUID: Steam
         FLUID BUOYANCY MODEL:
           Option = Density Difference
         END
         TURBULENCE MODEL:
           Option = Dispersed Phase Zero Equation
         END
       END
       FLUID: Water
         FLUID BUOYANCY MODEL:
           Option = Density Difference
         END
         TURBULENCE MODEL:
           Option = k epsilon
           BUOYANCY TURBULENCE:
             Option = None
           END
         END
         TURBULENT WALL FUNCTIONS:
           High Speed Model = Off
           Option = Scalable
         END
       END
       HEAT TRANSFER MODEL:
         Homogeneous Model = Off
         Option = Total Energy
       END
       THERMAL RADIATION MODEL:
         Option = None
       END
       TURBULENCE MODEL:
         Homogeneous Model = False
         Option = Fluid Dependent
       END
     END
     FLUID PAIR: Steam | Water
       INTERPHASE HEAT TRANSFER:
         Option = Two Resistance
         FLUID1 INTERPHASE HEAT TRANSFER:
           Option = Zero Resistance
         END
         FLUID2 INTERPHASE HEAT TRANSFER:
           Option = Ranz Marshall
         END
       END
       INTERPHASE TRANSFER MODEL:
         Option = Particle Model
       END
       MASS TRANSFER:
         Option = Phase Change
         PHASE CHANGE MODEL:
           Option = Thermal Phase Change
         END
       END
       MOMENTUM TRANSFER:
         DRAG FORCE:
           Drag Coefficient = 0.44
           Option = Drag Coefficient
         END
         LIFT FORCE:
           Option = None
         END
         TURBULENT DISPERSION FORCE:
           Option = None
         END
         VIRTUAL MASS FORCE:
           Option = None
         END
         WALL LUBRICATION FORCE:
           Option = None
         END
       END
       TURBULENCE TRANSFER:
         ENHANCED TURBULENCE PRODUCTION MODEL:
           Option = None
         END
       END
     END
     INITIALISATION:
       Option = Automatic
       FLUID: Steam
         INITIAL CONDITIONS:
           Velocity Type = Cartesian
           CARTESIAN VELOCITY COMPONENTS:
             Option = Automatic with Value
             U = 0 [mm s^-1]
             V = 0 [mm s^-1]
             W = 0 [mm s^-1]
           END
           TEMPERATURE:
             Option = Automatic
           END
           VOLUME FRACTION:
             Option = Automatic with Value
             Volume Fraction = 0
           END
         END
       END
       FLUID: Water
         INITIAL CONDITIONS:
           Velocity Type = Cartesian
           CARTESIAN VELOCITY COMPONENTS:
             Option = Automatic with Value
             U = 0 [mm s^-1]
             V = 0 [mm s^-1]
             W = 0 [mm s^-1]
           END
           TEMPERATURE:
             Option = Automatic with Value
             Temperature = 30 [C]
           END
           TURBULENCE INITIAL CONDITIONS:
             Option = k and Epsilon
             EPSILON:
               Option = Automatic
             END
             K:
               Option = Automatic
             END
           END
           VOLUME FRACTION:
             Option = Automatic with Value
             Volume Fraction = 1
           END
         END
       END
       INITIAL CONDITIONS:
         STATIC PRESSURE:
           Option = Automatic with Value
           Relative Pressure = 1 [atm]
         END
       END
     END
     MULTIPHASE MODELS:
       Homogeneous Model = Off
       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 = Upwind
     END
     CONVERGENCE CONTROL:
       Maximum Number of Iterations = 1500
       Minimum Number of Iterations = 1
       Physical Timescale = 0.001 [s]
       Timescale Control = Physical Timescale
     END
     CONVERGENCE CRITERIA:
       Residual Target = 1.E-4
       Residual Type = RMS
     END
     DYNAMIC MODEL CONTROL:
       Global Dynamic Model Control = Yes
     END
   END
 END
 COMMAND FILE:
   Version = 15.0
   Results Version = 15.0.7
 END
 SIMULATION CONTROL:
   EXECUTION CONTROL:
     EXECUTABLE SELECTION:
       Double Precision = On
     END
     INTERPOLATOR STEP CONTROL:
       Runtime Priority = Standard
       DOMAIN SEARCH CONTROL:
         Bounding Box Tolerance = 0.01
       END
       INTERPOLATION MODEL CONTROL:
         Enforce Strict Name Mapping for Phases = Off
         Mesh Deformation Option = Automatic
         Particle Relocalisation Tolerance = 0.01
       END
       MEMORY CONTROL:
         Memory Allocation Factor = 1.0
       END
     END
     PARALLEL HOST LIBRARY:
       HOST DEFINITION: syyed
         Host Architecture String = winnt-amd64
         Installation Root = C:\Program Files\ANSYS Inc\v%v\CFX
       END
     END
     PARTITIONER STEP CONTROL:
       Multidomain Option = Independent Partitioning
       Runtime Priority = Standard
       EXECUTABLE SELECTION:
         Use Large Problem Partitioner = Off
       END
       MEMORY CONTROL:
         Memory Allocation Factor = 1.0
       END
       PARTITIONING TYPE:
         MeTiS Type = k-way
         Option = MeTiS
         Partition Size Rule = Automatic
       END
     END
     RUN DEFINITION:
       Run Mode = Full
       Solver Input File = Single phase test.def
       INITIAL VALUES SPECIFICATION:
         INITIAL VALUES CONTROL:
           Continue History From = Initial Values 1
           Use Mesh From = Solver Input File
         END
         INITIAL VALUES: Initial Values 1
           File Name = D:\My Docs\ANSYS Working Directory\Test\Project new \
             start 1st ramadan_files\dp0\CFX-4\CFX\Single phase test_041.res
           Option = Results File
         END
       END
     END
     SOLVER STEP CONTROL:
       Runtime Priority = Standard
       MEMORY CONTROL:
         Memory Allocation Factor = 1.0
       END
       PARALLEL ENVIRONMENT:
         Number of Processes = 1
         Start Method = Serial
       END
     END
   END
 END

adilsyyed · June 24, 2015, 02:01

I have used different meshes but right now I am using this one. It is automatically generated mesh by CFX.

The result file gives these values for Steam Volume fraction and Steam Mach number. Isn't the mach number supposed to be highest at the outlet of nozzle?

M3.png M1.png M2.png

R1.jpg R2.jpg

ghorrocks · June 24, 2015, 03:57

The shock wave can occur in the divergent section in some flow regimes.

You do not need the long pipe leading to the nozzle. You could put your inlet boundary much closer to the nozzle and save lots of mesh.

Given that this simulation appears to have:
* compressible flow
* Shock waves, sonic flow
* free surface
* phase change

This is a very difficult model and I would expect a lot of difficulties in getting this to converge. This is going to take a CFD expert quite a while to get working. Unless you are an expert in CFD I fear you have taken on too advanced a model. This model is going to be too hard to fix over the forum.

adilsyyed · June 24, 2015, 07:34

Quote:

Originally Posted by ghorrocks

This is a very difficult model and I would expect a lot of difficulties in getting this to converge. This is going to take a CFD expert quite a while to get working. Unless you are an expert in CFD I fear you have taken on too advanced a model. This model is going to be too hard to fix over the forum.

Thanks for your valuable tips.
This is my for Masters Project so I am stuck with it anyway. I will try different approaches, and will ask the experts of the forum whenever I get jammed.

Questions arise in mind during the course of a study, and I will ask them rather than asking to solve the entire problem.

ghorrocks · June 24, 2015, 07:57

If are doing a masters on it then you have time to become an expert in the topic. So you have some time to get it right.

I would recommend a staged approach:
1) incompressible, single phase flow (you have already done this)
2) compressible flow, single phase flow
3) compressible water vapour flow, single phase
4) incompressible free surface multi phase, simple fluids (air and water- if this is a free surface simulation)

Once you can successfully do all these only then would I consider combining them. And don't just get them to converge, do some sensitivity studies to show that your results are accurate.

adilsyyed · June 24, 2015, 08:12

This is not a free surface simulation. And thanks for moral support Glenn. I really appreciate it.

I will start doing exactly that.

I have two questions for you Sir,

1. What type of mesh do you think should be adequate for this purpose?
2. Generally, to simulate a real life bigger tank, on the sides of the the tank in the simulation is given Opening boundary conditions.
My question is, buoyancy being ON, hydrostatic pressure in play, can I give the static pressure at opening BC to be atmospheric pressure? This opening BC being at the sides and/or at the bottom of the tank.

JuPa · June 24, 2015, 09:33

Tip:

1) Read the CFX theory guide as to which sources you are solving for.
2) Find the derivative of those sources and supply the information to CFX as a linearisation coefficient for all the sources you have.
3) The residuals should behave better with a linearisation coefficient .

Read the theory guide on "linearization coefficient" and read up Patanker's book on numerical heat transfer. It has a good section on source term linearisation.

adilsyyed · June 24, 2015, 09:46

Quote:

Originally Posted by RicochetJ

Tip:

1) Read the CFX theory guide as to which sources you are solving for.
2) Find the derivative of those sources and supply the information to CFX as a linearisation coefficient for all the sources you have.
3) The residuals should behave better with a linearisation coefficient .

Read the theory guide on "linearization coefficient" and read up Patanker's book on numerical heat transfer. It has a good section on source term linearisation.

Thanks a lot.
Well you must be right, because I didn't get anything you said.
Going to research on everything you recommended. I really appreciate the help Sir.

JuPa · June 24, 2015, 10:28

Quote:

Originally Posted by adilsyyed

Thanks a lot.
Well you must be right, because I didn't get anything you said.
Going to research on everything you recommended. I really appreciate the help Sir.

It sounds very fancy but it's quite simple. This is a good nutshell guide:

http://www.cfd-online.com/Wiki/Sourc..._linearization

adilsyyed · June 24, 2015, 19:49

I used a ridiculously coarse mesh and my solution converged, in terms of residuals. The residuals dropped all the way to E-05. The domain imbalances found were away from the region of interest.

The mach number is maximum at the tip of the nozzle as one would expect. I put a moniter point at the tip of the nozzle for Steam Mach number and the value is stable.

I refined the mesh and again the residuals started to repeat a trend.

I know this solution is not to be trusted, but I do want to know why this happens generally.

I would appreciate any help.

R3g.jpg R3converged.png R3mach.jpg

ghorrocks · June 24, 2015, 20:42

There is not much point theorising into the details of a coarse mesh simulation. The coarse mesh will mean the result is not accurate, so I see little point in thinking too much about its details. Refine the mesh to a point where the results are trustworthy and then think about the result it tells you.

The answer to your problem is probably something to do with the exit shock moving about in the divergent section, and the location of this shock moves with mesh refinement. But as I said, I see little point in analysing this in too much detail as it is wrong to begin with.

June 22, 2015, 20:39	Error in Two phase (condensation) modeling	#1
adilsyyed Member Adil Syyed Join Date: May 2012 Posts: 49 Rep Power: 14	I am modeling direct contact condensation in nozzle-tank arrangement. The tank is filled with water at 30 degree Celsius and the nozzle is used to inject saturated steam at 2 bar absolute. I am using thermal phase change model. I have tried many things but the solver still give error. It runs normally for more than 300 iterations converging slowly, and out of nowhere sudden peaks in residuals happens and solver gives error. I have tried everything in the FAQ, but still no success. I have used a variety of meshes, very small timescale, played with boundary conditions, initial conditions and what not. PS, single phase simulation converges just fine in the same arrangement. I could really use some help regarding pin pointing the source of the error.

June 24, 2015, 03:57		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	The shock wave can occur in the divergent section in some flow regimes. You do not need the long pipe leading to the nozzle. You could put your inlet boundary much closer to the nozzle and save lots of mesh. Given that this simulation appears to have: * compressible flow * Shock waves, sonic flow * free surface * phase change This is a very difficult model and I would expect a lot of difficulties in getting this to converge. This is going to take a CFD expert quite a while to get working. Unless you are an expert in CFD I fear you have taken on too advanced a model. This model is going to be too hard to fix over the forum. adilsyyed likes this.

June 24, 2015, 07:57		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	If are doing a masters on it then you have time to become an expert in the topic. So you have some time to get it right. I would recommend a staged approach: 1) incompressible, single phase flow (you have already done this) 2) compressible flow, single phase flow 3) compressible water vapour flow, single phase 4) incompressible free surface multi phase, simple fluids (air and water- if this is a free surface simulation) Once you can successfully do all these only then would I consider combining them. And don't just get them to converge, do some sensitivity studies to show that your results are accurate. adilsyyed likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
two phase modeling	mehdimoradi.	Fluent Multiphase	0	October 16, 2013 08:13
Two continuous phases and one dispersed phase modeling using CFX	creddy_trddc	CFX	1	August 13, 2013 23:23
modeling of two phase flow combustion in fluidized bed with MFIX	ehsan.m	Main CFD Forum	0	July 17, 2013 17:47
phase change modeling	Danial Q	Main CFD Forum	0	April 5, 2012 02:14
Verification of this phase change modeling	kawamura	OpenFOAM	4	December 21, 2011 01:14

June 23, 2015, 03:16		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	Is this steady state or transient? This sounds like a tricky simulation to me - compressible flow with phase change. I would run the simulation generating a results file every timestep/coeff loop (or at least the ones just before it crashes). Have a look at what happens around the time it crashes - does some steam first hit the outlet boundary? Does some water backflow into the nozzle? Does a water vapour bubble collapse?

June 24, 2015, 02:01		#7
adilsyyed Member Adil Syyed Join Date: May 2012 Posts: 49 Rep Power: 14	I have used different meshes but right now I am using this one. It is automatically generated mesh by CFX. The result file gives these values for Steam Volume fraction and Steam Mach number. Isn't the mach number supposed to be highest at the outlet of nozzle? M3.png M1.png M2.png R1.jpg R2.jpg

June 24, 2015, 08:12		#11
adilsyyed Member Adil Syyed Join Date: May 2012 Posts: 49 Rep Power: 14	This is not a free surface simulation. And thanks for moral support Glenn. I really appreciate it. I will start doing exactly that. I have two questions for you Sir, 1. What type of mesh do you think should be adequate for this purpose? 2. Generally, to simulate a real life bigger tank, on the sides of the the tank in the simulation is given Opening boundary conditions. My question is, buoyancy being ON, hydrostatic pressure in play, can I give the static pressure at opening BC to be atmospheric pressure? This opening BC being at the sides and/or at the bottom of the tank.

June 24, 2015, 09:33		#12
JuPa Senior Member Mr CFD Join Date: Jun 2012 Location: Britain Posts: 361 Rep Power: 15	Tip: 1) Read the CFX theory guide as to which sources you are solving for. 2) Find the derivative of those sources and supply the information to CFX as a linearisation coefficient for all the sources you have. 3) The residuals should behave better with a linearisation coefficient . Read the theory guide on "linearization coefficient" and read up Patanker's book on numerical heat transfer. It has a good section on source term linearisation.

June 24, 2015, 19:49		#15
adilsyyed Member Adil Syyed Join Date: May 2012 Posts: 49 Rep Power: 14	I used a ridiculously coarse mesh and my solution converged, in terms of residuals. The residuals dropped all the way to E-05. The domain imbalances found were away from the region of interest. The mach number is maximum at the tip of the nozzle as one would expect. I put a moniter point at the tip of the nozzle for Steam Mach number and the value is stable. I refined the mesh and again the residuals started to repeat a trend. I know this solution is not to be trusted, but I do want to know why this happens generally. I would appreciate any help. R3g.jpg R3converged.png R3mach.jpg

June 24, 2015, 20:42		#16
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	There is not much point theorising into the details of a coarse mesh simulation. The coarse mesh will mean the result is not accurate, so I see little point in thinking too much about its details. Refine the mesh to a point where the results are trustworthy and then think about the result it tells you. The answer to your problem is probably something to do with the exit shock moving about in the divergent section, and the location of this shock moves with mesh refinement. But as I said, I see little point in analysing this in too much detail as it is wrong to begin with.