
[Sponsors] 
June 22, 2015, 20:39 
Error in Two phase (condensation) modeling

#1 
Member
Adil Syyed
Join Date: May 2012
Posts: 49
Rep Power: 11 
I am modeling direct contact condensation in nozzletank 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 23, 2015, 03:16 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,876
Rep Power: 132 
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 23, 2015, 05:21 

#3  
Member
Adil Syyed
Join Date: May 2012
Posts: 49
Rep Power: 11 
Quote:
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? 

June 23, 2015, 07:09 

#4  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,876
Rep Power: 132 
Quote:
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. 

June 23, 2015, 21:36 

#5 
Member
Adil Syyed
Join Date: May 2012
Posts: 49
Rep Power: 11 
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 = 0.03474982E01 [K^1] NASA a3 = 0.06354696E04 [K^2] NASA a4 = 0.06968581E07 [K^3] NASA a5 = 0.02506588E10 [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 = 0.03056293E01 [K^1] NASA a3 = 0.08730260E05 [K^2] NASA a4 = 0.01200996E08 [K^3] NASA a5 = 0.06391618E13 [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 = 9.4E06 [kg m^1 s^1] Option = Value END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 193E04 [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 = (230.23273.15) [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 

June 23, 2015, 21:37 

#6 
Member
Adil Syyed
Join Date: May 2012
Posts: 49
Rep Power: 11 
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.E4 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 = winntamd64 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 = kway 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\CFX4\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 

June 24, 2015, 02:01 

#7 
Member
Adil Syyed
Join Date: May 2012
Posts: 49
Rep Power: 11 
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.pngM1.pngM2.png R1.jpgR2.jpg 

June 24, 2015, 03:57 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,876
Rep Power: 132 
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. 

June 24, 2015, 07:34 

#9  
Member
Adil Syyed
Join Date: May 2012
Posts: 49
Rep Power: 11 
Quote:
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. 

June 24, 2015, 07:57 

#10 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,876
Rep Power: 132 
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. 

June 24, 2015, 08:12 

#11 
Member
Adil Syyed
Join Date: May 2012
Posts: 49
Rep Power: 11 
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 
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 12 
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, 09:46 

#13  
Member
Adil Syyed
Join Date: May 2012
Posts: 49
Rep Power: 11 
Quote:
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. 

June 24, 2015, 10:28 

#14  
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 12 
Quote:
http://www.cfdonline.com/Wiki/Sourc..._linearization 

June 24, 2015, 19:49 

#15 
Member
Adil Syyed
Join Date: May 2012
Posts: 49
Rep Power: 11 
I used a ridiculously coarse mesh and my solution converged, in terms of residuals. The residuals dropped all the way to E05. 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.pngR3mach.jpg 

June 24, 2015, 20:42 

#16 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,876
Rep Power: 132 
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. 

Tags 
condensation, two phase 
Thread Tools  Search this Thread 
Display Modes  


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 