CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Error in Two phase (condensation) modeling (https://www.cfd-online.com/Forums/cfx/154937-error-two-phase-condensation-modeling.html)

adilsyyed June 22, 2015 19:39
Error in Two phase (condensation) modeling
 
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.
http://imagizer.imageshack.us/v2/xq90/661/l9yprh.jpg

ghorrocks June 23, 2015 02:16
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 04:21
Quote:
Originally Posted by ghorrocks (Post 551603)
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 06:09
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 20:36
1 Attachment(s)
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
Attachment 40350

adilsyyed June 23, 2015 20:37
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 01:01
5 Attachment(s)
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?


Attachment 40351Attachment 40352Attachment 40353

Attachment 40354Attachment 40355

ghorrocks June 24, 2015 02:57
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 06:34
Quote:
Originally Posted by ghorrocks (Post 551868)
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 06:57
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 07:12
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 08:33
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 08:46
Quote:
Originally Posted by RicochetJ (Post 551924)
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 09:28
Quote:
Originally Posted by adilsyyed (Post 551926)
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 18:49
3 Attachment(s)
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.

Attachment 40367 Attachment 40368Attachment 40369

ghorrocks June 24, 2015 19:42
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.


All times are GMT -4. The time now is 23:05.