|
[Sponsors] |
Secondary liquid droplet breakup convergence issue |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 19, 2017, 23:53 |
Secondary liquid droplet breakup convergence issue
|
#1 |
New Member
Charlie
Join Date: Jun 2017
Posts: 6
Rep Power: 9 |
Hello all-
I have a steady-state (multiphase) model of a pipe carrying superheated steam into which I am injecting water via the particle injection feature in CFX, with particle evaporation. Without secondary breakup enabled, I can get convergence with reasonable results with 200 particles or so. I'm using IAPWS steam as the continuous fluid, with the CFX H2Og/l combo as my evaporating fluid. My mesh quality I think is ok: +--------------------------------------------------------------------+ | Domain Name | Orthog. Angle | Exp. Factor | Aspect Ratio | +----------------------+---------------+--------------+--------------+ | | Minimum [deg] | Maximum | Maximum | +----------------------+---------------+--------------+--------------+ | Default Domain | 56.0 OK | 7 ok | 5 OK | +----------------------+---------------+--------------+--------------+ | | %! %ok %OK | %! %ok %OK | %! %ok %OK | +----------------------+---------------+--------------+--------------+ | Default Domain | 0 0 100 | 0 <1 100 | 0 0 100 | +----------------------+---------------+--------------+--------------+ With secondary breakup enabled (I've tried a few different models), however, I cannot seem to achieve a similar convergence/stability. I tried remeshing, changing timesteps, and weighting. I use the input from the solved non-secondary model as initial conditions. I have changed the number of particles down to 5. Maybe I just haven't hit the right combination. I've read here elsewhere that I shouldn't have to enable relaxation on any of the equations, so I've tried to avoid that (I do use them for the particle equations). The static temperature and temperature variables during iterations appear to rise well outside of their expected range (shouldn't be above 1350R at the most, but are hitting 3000R+). I am stumped. I've explored this site (fantastic site, btw), as well as the CFX manuals and internet. I think maybe I just haven't happened upon someone with a similar issue. I've just started a run with the model that successfully solved without secondary breakup using a timestep of 1.0e-6 (this is the smallest I've gone yet) hoping this will help (to see the effect), at the risk of growing old. At this point, I'm wondering if I have switched an option on here to cause issues and don't realize it. Just baffled that turning on secondary breakup has such an effect. Any help is appreciated. Beginning of out file posted below. Thanks in advance, Charlie ------------- HTML Code:
FLOW: Flow Analysis 1 SOLUTION UNITS: Angle Units = [rad] Length Units = [ft] Mass Units = [lb] Solid Angle Units = [sr] Temperature Units = [R] Time Units = [s] END ANALYSIS TYPE: Option = Steady State EXTERNAL SOLVER COUPLING: Option = None END END DOMAIN: Default Domain Coord Frame = Coord 0 Domain Type = Fluid Location = B204, B225, B250, B256 BOUNDARY: Default Fluid Fluid Interface Side 1 Boundary Type = INTERFACE Location = F212.204,F222.225,F249.250 BOUNDARY CONDITIONS: COMPONENT: H2O Option = Conservative Interface Flux END HEAT TRANSFER: Option = Conservative Interface Flux END MASS AND MOMENTUM: Option = Conservative Interface Flux END TURBULENCE: Option = Conservative Interface Flux END END END BOUNDARY: Default Fluid Fluid Interface Side 2 Boundary Type = INTERFACE Location = F224.225,F252.256,F255.256 BOUNDARY CONDITIONS: COMPONENT: H2O Option = Conservative Interface Flux END HEAT TRANSFER: Option = Conservative Interface Flux END MASS AND MOMENTUM: Option = Conservative Interface Flux END TURBULENCE: Option = Conservative Interface Flux END END END BOUNDARY: Outlet Boundary Type = OUTLET Location = OutletPlane BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END MASS AND MOMENTUM: Option = Static Pressure Relative Pressure = 112.5 [psi] END END END BOUNDARY: Steam Inlet Boundary Type = INLET Location = InletPlane BOUNDARY CONDITIONS: COMPONENT: H2O Mass Fraction = 0.0 Option = Mass Fraction END FLOW DIRECTION: Option = Normal to Boundary Condition END FLOW REGIME: Option = Subsonic END HEAT TRANSFER: Option = Static Temperature Static Temperature = 704 [F] END MASS AND MOMENTUM: Mass Flow Rate = 55.6 [lb s^-1] Mass Flow Rate Area = As Specified Option = Mass Flow Rate END TURBULENCE: Option = Medium Intensity and Eddy Viscosity Ratio END END FLUID: Spray Water BOUNDARY CONDITIONS: END END END BOUNDARY: Walls Boundary Type = WALL Location = AllWalls BOUNDARY CONDITIONS: HEAT TRANSFER: Option = Adiabatic END MASS AND MOMENTUM: Option = No Slip Wall END WALL ROUGHNESS: Option = Smooth Wall END END FLUID: Spray Water BOUNDARY CONDITIONS: PARTICLE WALL INTERACTION: Option = Equation Dependent END VELOCITY: Option = Restitution Coefficient Parallel Coefficient of Restitution = 1.0 Perpendicular Coefficient of Restitution = 1.0 END END END END DOMAIN MODELS: BUOYANCY MODEL: Buoyancy Reference Density = 0.1642 [lb ft^-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 = 0 [psi] END END FLUID DEFINITION: RH Stm Material = Steam5 and H2Og VMix Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID DEFINITION: Spray Water Material = H2Ol Option = Material Library MORPHOLOGY: Option = Dispersed Particle Transport Fluid PARTICLE DIAMETER CHANGE: Option = Mass Equivalent END PARTICLE DIAMETER DISTRIBUTION: Option = Rosin Rammler Rosin Rammler Power = 3.76 Rosin Rammler Size = 566 [micron] END END END FLUID MODELS: COMBUSTION MODEL: Option = None END FLUID: RH Stm COMPONENT: H2O Option = Transport Equation END COMPONENT: Steam5 Option = Constraint END FLUID BUOYANCY MODEL: Option = Non Buoyant END HEAT TRANSFER MODEL: Include Viscous Dissipation Term = Off Option = Thermal Energy END WALL CONDENSATION MODEL: Option = None END END FLUID: Spray Water EROSION MODEL: Option = None END FLUID BUOYANCY MODEL: Option = Density Difference END HEAT TRANSFER MODEL: Option = Particle Temperature END PARTICLE ROUGH WALL MODEL: Option = None END END HEAT TRANSFER MODEL: Option = Fluid Dependent END THERMAL RADIATION MODEL: Option = None END TURBULENCE MODEL: Option = k epsilon BUOYANCY TURBULENCE: Option = None END END TURBULENT WALL FUNCTIONS: Option = Scalable END END FLUID PAIR: RH Stm | Spray Water Particle Coupling = Fully Coupled Surface Tension Coefficient = 0.04855 [N m^-1] COMPONENT PAIR: H2O | H2Ol Option = Liquid Evaporation Model LATENT HEAT: Option = From Material Properties END END INTERPHASE HEAT TRANSFER: Option = Ranz Marshall END MOMENTUM TRANSFER: DRAG FORCE: Option = Schiller Naumann END PRESSURE GRADIENT FORCE: Option = None END TURBULENT DISPERSION FORCE: Option = Particle Dispersion END VIRTUAL MASS FORCE: Option = None END END PARTICLE BREAKUP: Critical Weber Number for Bag Breakup = 6.0 Option = Reitz and Diwakar Time Factor for Bag Breakup = 3.1415927 Time Factor for Stripping = 20 Weber Number Factor for Stripping = 0.5 END END INITIALISATION: Option = Automatic INITIAL CONDITIONS: Velocity Type = Cartesian CARTESIAN VELOCITY COMPONENTS: Option = Automatic END COMPONENT: H2O Option = Automatic END STATIC PRESSURE: Option = Automatic with Value Relative Pressure = 114 [psi] END TEMPERATURE: Option = Automatic with Value Temperature = 700 [F] END TURBULENCE INITIAL CONDITIONS: Option = Medium Intensity and Eddy Viscosity Ratio END END END PARTICLE INJECTION REGION: Particle Injection Region 1 Coord Frame = Coord 0 FLUID: Spray Water INJECTION CONDITIONS: INJECTION METHOD: Option = Cone CONE DEFINITION: Injection Centre = 9.23 [m], 0 [m], -1.05 [m] Option = Hollow Cone Radius of Injection Plane = 0.5 [in] INJECTION DIRECTION: Injection Direction X Component = 0 Injection Direction Y Component = 0 Injection Direction Z Component = 1 Option = Cartesian Components END END INJECTION VELOCITY: Cone Angle = 30 [deg] Injection Velocity Magnitude = 71.58 [ft s^-1] Option = Velocity Magnitude DISPERSION ANGLE: Dispersion Angle = 5 [deg] Option = Dispersion Angle END END NUMBER OF POSITIONS: Number = 200 Option = Direct Specification END END PARTICLE DIAMETER DISTRIBUTION: Option = Rosin Rammler Rosin Rammler Power = 3.759 Rosin Rammler Size = 580.96 [micron] END PARTICLE MASS FLOW RATE: Mass Flow Rate = 8.333 [lb s^-1] END TEMPERATURE: Option = Value Temperature = 304 [F] END END 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 = Automatic END END OUTPUT CONTROL: MONITOR OBJECTS: MONITOR BALANCES: Option = Full END MONITOR FORCES: Option = Full END MONITOR PARTICLES: Option = Full END MONITOR POINT: Outlet Temp Coord Frame = Coord 0 Expression Value = areaAve(Temperature)@Outlet Option = Expression END MONITOR POINT: Particle Ave Temp Cartesian Coordinates = 0.0[m],0.0[m],0.0[m] Coord Frame = Coord 0 Option = Cartesian Coordinates Output Variables List = Spray Water.Averaged Temperature MONITOR LOCATION CONTROL: Interpolation Type = Nearest Vertex END POSITION UPDATE FREQUENCY: Option = Initial Mesh Only END END MONITOR POINT: Particle RMS Temp Cartesian Coordinates = 0.0[m],0.0[m],0.0[m] Coord Frame = Coord 0 Option = Cartesian Coordinates Output Variables List = Spray Water.RMS Temperature MONITOR LOCATION CONTROL: Interpolation Type = Nearest Vertex END POSITION UPDATE FREQUENCY: Option = Initial Mesh Only END END MONITOR RESIDUALS: Option = Full END MONITOR TOTALS: Option = Full END END RESULTS: File Compression Level = Default Option = Standard Output Equation Residuals = All END END SOLVER CONTROL: Turbulence Numerics = High Resolution ADVECTION SCHEME: Option = High Resolution END CONVERGENCE CONTROL: Maximum Number of Iterations = 2500 Minimum Number of Iterations = 20 Physical Timescale = 1e-006 [s] Timescale Control = Physical Timescale END CONVERGENCE CRITERIA: Conservation Target = 0.0001 Residual Target = 0.00001 Residual Type = RMS END DYNAMIC MODEL CONTROL: Global Dynamic Model Control = On END PARTICLE CONTROL: PARTICLE INTEGRATION: First Iteration for Particle Calculation = 40 Iteration Frequency = 40 Option = Forward Euler END PARTICLE TERMINATION CONTROL: Maximum Number of Integration Steps = 20000 Maximum Tracking Distance = 70 [foot] END PARTICLE UNDER RELAXATION FACTORS: Energy Under Relaxation Factor = 0.5 Mass Under Relaxation Factor = 0.5 Velocity Under Relaxation Factor = 0.5 END END END END COMMAND FILE: Version = 18.1 Results Version = 18.1 END |
|
June 20, 2017, 00:59 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
I would recommend:
* Having a close look at the results with particle breakup enabled. Write a backup file before it crashes (if it diverges). The results will not be converged but might give a clue as to why particle breakup is causing problems. Check that they are behaving as you would expect. * Pay close attention to the region where new particles are being generated, I suspect the spurious temperatures are occurring in this region. * To check whether there is anything to be gained by improving mesh quality, I would make a simplified geoemetry which can be meshed with 1:1 hexas or close to it. Run that and see if the particle breakup works or not. I know of some models where an aspect ratio of 1.2 is too much, and for these models the CFX built in mesh quality checks are useless. Your model already has IAPWS (which is well known to be numerically unstable), and adding particle breakup might push it over the edge. |
|
June 21, 2017, 16:22 |
|
#3 |
New Member
Charlie
Join Date: Jun 2017
Posts: 6
Rep Power: 9 |
Thank you for the advice, Mr. Horrocks. Based on your input, I actually tried to gain a numerical advantage by swapping to the H2O/v/l material set, replacing my IAPWS material (my test run w/o breakup shows this would work for me). So, I hope this gives me more chance for success.
I interrupted a run and took a look at the paused solution with the particle breakup enabled. The issue appears to occur at the outlet of my pipe elbow where it connects to a short straight piece (the geometry is a straight pipe with particle injection, a downstream 90 degree elbow, and a short straight pipe from the elbow outlet). The particle/droplet temperature, according to the particle track, drops below the water temperature coming into the pipe (which I think impossible). This is also the area of the lowest temperature in the entire domain. I didn't see anything suspicious at the injection location except the particle temperature is too low. Image attached of the elbow trace. I have not set up a simple geometry with the 1:1 hexas yet, but will work on something today if I can't resolve the issues. Based on the interrupted solution observations and suggestions you made, I did go ahead and refine the meshing in the elbow to test it and am trying a smaller physical timestep for the steady-state simulation as well. The residuals have dropped a bit and the monitor points (outlet temps) don't oscillate as much. I am also wondering if the concentration of coincident droplets in a particular volume/element in the elbow would overwhelm the solution, and would I benefit from a coarser mesh at the elbow. I included some images of residuals and outlet temp monitor that may provide more insight and clarity to my problem that I don't necessarily recognize: first signature is no breakup solution; second is breakup enabled (left it running overnight); and the last part is the refined elbow mesh with smaller physical timestep. I did notice that when plotting particle temperatures, some strange values appear and maybe I don't understand the plotted variables. For example, on a particle track, if I plot Particle.Temperature, the values are near 70 degrees lower than what should be the lowest temperature in the solution; if I plot Temperature along the particle track, the results seem reasonable. Could this also be an issue for me, or is Particle.Temperature simply a variable used by the solver and has no physical meaning? Or maybe I do understand, and this is actually the root of my problem? Thanks, Charlie |
|
June 21, 2017, 19:01 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,819
Rep Power: 144 |
You better check the documentation on this, but I suspect Particle.Temperature is the particle temperature and Temperature is the temperature of the continuous phase at that same point. That may explain the difference you are seeing.
I do not have an answer for your main question on why the temperature is not realistic. You are going to have to do some trial and error to work that one out. |
|
June 24, 2017, 13:50 |
|
#5 |
New Member
Charlie
Join Date: Jun 2017
Posts: 6
Rep Power: 9 |
I think you are correct. I have been working with a simpler model via your suggestion, and have discovered further questions about the particle fluid temperature effects and the sensitivity to pressure and inlet mass fraction of the fluid. This is a different question than I had before, so I will post in a newer thread concentrating on the particle temperatures themselves.
Thanks for your help. Charlie |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Convergence | Centurion2011 | FLUENT | 48 | June 14, 2022 23:29 |
Force can not converge | colopolo | CFX | 13 | October 4, 2011 22:03 |
Convergence issue in SST for Porous model | Raj | CFX | 0 | May 2, 2008 02:43 |
CFX-Solver, issue with convergence behavior | Andy | CFX | 7 | September 5, 2006 03:24 |
droplet breakup modelling | Birute | Main CFD Forum | 0 | August 5, 2003 07:39 |