|
[Sponsors] |
January 10, 2017, 08:36 |
Wrong multiphase flow at rotating interface
|
#1 |
Member
Sanyo
Join Date: Apr 2009
Location: India
Posts: 62
Rep Power: 17 |
Hello All,
I am trying simulate a rotating nozzle type arrangement. I have modeled two concentric cylinders. A cross type arrangement is at center of inner cylinder which is inlet for water. Rest of the domain is initialized with air. Inner cylinder rotates with 4000rpm. Interface is frozen-rotor type. Homogeneous multi phase, mixture model is used. While studying the results, I am seeing very odd behavior of water at interface. Instead of continuing its motion, water is suddenly changing its direction. This is not correct. If I move the interface away or close, same effect is seen. So I am sure that this must be interface problem. If I run with transient rotor-stator, same problem continues. Attached is image for reference. Does anybody know, whats wrong? Is it a bug or am I missing something? |
|
January 10, 2017, 16:24 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,828
Rep Power: 144 |
||
January 11, 2017, 01:31 |
|
#3 |
Member
Sanyo
Join Date: Apr 2009
Location: India
Posts: 62
Rep Power: 17 |
Thanks Glenn for reply.
But I am not puzzled about velocity. Its volume fraction of water. It should not be changing at interface. It appears that cfx uses local reference frame velocity for calculation of volume fraction. But its giving wrong results. Please see the image. Is there any way to resolve this? |
|
January 11, 2017, 16:39 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,828
Rep Power: 144 |
Can you post your CCL file?
You say you get the same results if you run with transient rotor stator? |
|
January 12, 2017, 06:38 |
|
#5 |
Member
Sanyo
Join Date: Apr 2009
Location: India
Posts: 62
Rep Power: 17 |
Yes. Same results with transient rotor stator. I guess volume fraction is calculated using superficial velocity that's why there is such odd behavior. Is there any way to calculate it based on superficial velocity in stationary frame(there is no such standard variable though)?
Following is ccl: FLOW: Flow Analysis 1 SOLUTION UNITS: Angle Units = [rad] Length Units = [m] 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: ROTATING II Coord Frame = Coord 0 Domain Type = Fluid Location = Rotating BOUNDARY: Domain Interface 1 Side 1 Boundary Type = INTERFACE Location = Interface_2 BOUNDARY CONDITIONS: MASS AND MOMENTUM: Option = Conservative Interface Flux END TURBULENCE: Option = Conservative Interface Flux END END END BOUNDARY: INLET Boundary Type = INLET Frame Type = Rotating Location = Inlet BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END MASS AND MOMENTUM: Normal Speed = 10 [m s^-1] Option = Normal Speed END TURBULENCE: Option = Medium Intensity and Eddy Viscosity Ratio END END FLUID: Air BOUNDARY CONDITIONS: VOLUME FRACTION: Option = Value Volume Fraction = 0 END END END FLUID: Liquid BOUNDARY CONDITIONS: VOLUME FRACTION: Option = Value Volume Fraction = 1 END END END END BOUNDARY: ROTATING II Default Boundary Type = WALL Frame Type = Rotating Location = Primitive 2D F,Primitive 2D G BOUNDARY CONDITIONS: MASS AND MOMENTUM: Option = No Slip Wall END WALL ROUGHNESS: Option = Smooth Wall END END END BOUNDARY: Wall Nozzles Boundary Type = WALL Frame Type = Rotating Location = Wall Inlet BOUNDARY CONDITIONS: MASS AND MOMENTUM: Option = No Slip Wall END WALL ROUGHNESS: Option = Smooth Wall END END END DOMAIN MODELS: BUOYANCY MODEL: Option = Non Buoyant END DOMAIN MOTION: Angular Velocity = 4000 [rev min^-1] Option = Rotating AXIS DEFINITION: Option = Coordinate Axis Rotation Axis = Coord 0.2 END END MESH DEFORMATION: Option = None END REFERENCE PRESSURE: Reference Pressure = 1 [atm] END END FLUID DEFINITION: Air Material = Air at 25 C Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID DEFINITION: Liquid Material = Water Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID MODELS: COMBUSTION MODEL: Option = None END HEAT TRANSFER MODEL: Fluid Temperature = 25 [C] Homogeneous Model = On Option = Isothermal END THERMAL RADIATION MODEL: Option = None END TURBULENCE MODEL: Option = k epsilon END TURBULENT WALL FUNCTIONS: Option = Scalable END END FLUID PAIR: Air | Liquid Surface Tension Coefficient = 0.073 [N m^-1] INTERPHASE TRANSFER MODEL: Interface Length Scale = 1. [mm] Option = Mixture Model END MASS TRANSFER: Option = None END SURFACE TENSION MODEL: Option = None END END INITIALISATION: Frame Type = Rotating Option = Automatic FLUID: Air INITIAL CONDITIONS: VOLUME FRACTION: Option = Automatic with Value Volume Fraction = 1 END END END FLUID: Liquid INITIAL CONDITIONS: VOLUME FRACTION: Option = Automatic with Value Volume Fraction = 0 END END END INITIAL CONDITIONS: Velocity Type = Cartesian CARTESIAN VELOCITY COMPONENTS: Option = Automatic END STATIC PRESSURE: Option = Automatic END TURBULENCE INITIAL CONDITIONS: Option = Medium Intensity and Eddy Viscosity Ratio END END END MULTIPHASE MODELS: Homogeneous Model = On FREE SURFACE MODEL: Option = Standard END END END DOMAIN: Stationary Coord Frame = Coord 0 Domain Type = Fluid Location = Stationary BOUNDARY: Domain Interface 1 Side 2 Boundary Type = INTERFACE Location = Interface BOUNDARY CONDITIONS: MASS AND MOMENTUM: Option = Conservative Interface Flux END TURBULENCE: Option = Conservative Interface Flux END END END BOUNDARY: Opening Boundary Type = OPENING Location = Opening BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END MASS AND MOMENTUM: Option = Opening Pressure and Direction Relative Pressure = 0 [bar] END TURBULENCE: Option = Medium Intensity and Eddy Viscosity Ratio END END FLUID: Air BOUNDARY CONDITIONS: VOLUME FRACTION: Option = Value Volume Fraction = 1 END END END FLUID: Liquid BOUNDARY CONDITIONS: VOLUME FRACTION: Option = Value Volume Fraction = 0 END END END END BOUNDARY: Stationary Default Boundary Type = WALL Location = Primitive 2D D,Primitive 2D E BOUNDARY CONDITIONS: MASS AND MOMENTUM: Option = No Slip Wall END WALL ROUGHNESS: Option = Smooth Wall END END END DOMAIN MODELS: BUOYANCY MODEL: Option = Non Buoyant END DOMAIN MOTION: Option = Stationary END MESH DEFORMATION: Option = None END REFERENCE PRESSURE: Reference Pressure = 1 [atm] END END FLUID DEFINITION: Air Material = Air at 25 C Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID DEFINITION: Liquid Material = Water Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID MODELS: COMBUSTION MODEL: Option = None END HEAT TRANSFER MODEL: Fluid Temperature = 25 [C] Homogeneous Model = On Option = Isothermal END THERMAL RADIATION MODEL: Option = None END TURBULENCE MODEL: Option = k epsilon END TURBULENT WALL FUNCTIONS: Option = Scalable END END FLUID PAIR: Air | Liquid Surface Tension Coefficient = 0.073 [N m^-1] INTERPHASE TRANSFER MODEL: Interface Length Scale = 1. [mm] Option = Mixture Model END MASS TRANSFER: Option = None END SURFACE TENSION MODEL: Option = None END END INITIALISATION: Option = Automatic FLUID: Air INITIAL CONDITIONS: VOLUME FRACTION: Option = Automatic with Value Volume Fraction = 1 END END END FLUID: Liquid INITIAL CONDITIONS: VOLUME FRACTION: Option = Automatic with Value Volume Fraction = 0 END END END INITIAL CONDITIONS: Velocity Type = Cartesian CARTESIAN VELOCITY COMPONENTS: Option = Automatic END STATIC PRESSURE: Option = Automatic END TURBULENCE INITIAL CONDITIONS: Option = Medium Intensity and Eddy Viscosity Ratio END END END MULTIPHASE MODELS: Homogeneous Model = On FREE SURFACE MODEL: Option = Standard END END END DOMAIN INTERFACE: Domain Interface 1 Boundary List1 = Domain Interface 1 Side 1 Boundary List2 = Domain Interface 1 Side 2 Interface Type = Fluid Fluid INTERFACE MODELS: Option = General Connection FRAME CHANGE: Option = Frozen Rotor 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: BACKUP RESULTS: Backup Results 1 File Compression Level = Default Option = Standard OUTPUT FREQUENCY: Iteration Interval = 50 Option = Iteration Interval END END MONITOR OBJECTS: MONITOR BALANCES: Option = Full END MONITOR FORCES: Option = Full END MONITOR PARTICLES: Option = Full END MONITOR RESIDUALS: Option = Full END MONITOR TOTALS: Option = Full END END RESULTS: File Compression Level = Default Option = Standard END END SOLVER CONTROL: Turbulence Numerics = First Order ADVECTION SCHEME: Option = High Resolution END CONVERGENCE CONTROL: Length Scale Option = Conservative Maximum Number of Iterations = 500 Minimum Number of Iterations = 500 Timescale Control = Auto Timescale Timescale Factor = 1 END CONVERGENCE CRITERIA: Residual Target = 0.000001 Residual Type = RMS END DYNAMIC MODEL CONTROL: Global Dynamic Model Control = Yes END END END |
|
January 12, 2017, 16:34 |
|
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,828
Rep Power: 144 |
I can see why frozen rotor would cause this, but transient rotor stator should handle it correctly. Can you post an image of the velocity vectors from the transient rotor stator simulation?
How long did you run the transient rotor stator simulation for? |
|
January 13, 2017, 07:15 |
|
#7 |
Member
Sanyo
Join Date: Apr 2009
Location: India
Posts: 62
Rep Power: 17 |
Attached are images from transient run. I have run it for 2 sec with 0.001s timestep. Even if I run for more time or lower timestep, I doubt that results will change.
Is there any solution? |
|
January 14, 2017, 02:50 |
|
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,828
Rep Power: 144 |
I think your time step size is far too big. Please repeat the TRS simulation with at least 100 time steps per rev at 4000 rpm.
|
|
January 17, 2017, 06:36 |
|
#9 |
Member
Sanyo
Join Date: Apr 2009
Location: India
Posts: 62
Rep Power: 17 |
Thanks Glenn,
It worked like a charm! Now the volume fraction is continuous at interface. But how to achieve these results in steady state? It will not be always feasible to carry out transient run with such small timestep especially with large models. There must be some way to do it using frozen rotor, right? |
|
January 18, 2017, 03:37 |
|
#10 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,828
Rep Power: 144 |
I am on holidays at the moment so I cannot look anything up.
But try the other GGI frame change models. Especially the Fourier Transform one. |
|
January 19, 2017, 08:06 |
|
#11 |
Member
Sanyo
Join Date: Apr 2009
Location: India
Posts: 62
Rep Power: 17 |
Extremely Sorry to disturb you.
I will try other models. Thanks for your help. |
|
January 19, 2017, 17:55 |
|
#12 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,828
Rep Power: 144 |
No need to apologise. I am the twit who is doing this stuff on his holidays. Just shows what sort of a CFD tragic I am.
|
|
January 21, 2017, 09:23 |
Thank you very much for your help
|
#13 |
Member
Sanyo
Join Date: Apr 2009
Location: India
Posts: 62
Rep Power: 17 |
I think you are the lighthouse of CFD for people like me. Really appreciate your help every time. Thanks for taking such pain for CFD community.
|
|
February 7, 2017, 06:06 |
|
#14 |
Member
Sanyo
Join Date: Apr 2009
Location: India
Posts: 62
Rep Power: 17 |
Hello Glenn,
Sorry to disturb. But I couldn't get the results in steady state. FFT is used in transient case. Could you help me out please? |
|
February 7, 2017, 17:19 |
|
#15 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,828
Rep Power: 144 |
This is not an area I can help you much with, hopefully some of the other members of the forum with more experience in rotating machinery can help you with implementing it.
All I can suggest is to do the relevant tutorial examples available on the ANSYS customer page. That shows how to run most of the models in CFX. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Wind turbine simulation | Saturn | CFX | 60 | July 17, 2024 05:45 |
My radial inflow turbine | Abo Anas | CFX | 27 | May 11, 2018 01:44 |
Overflow Error in Multiphase Modelling with Two Continuous Fluids | ashtonJ | CFX | 6 | August 11, 2014 14:32 |
CFX13 Post Periodic interface | EtaEta | CFX | 7 | December 8, 2011 17:15 |
RPM in Wind Turbine | Pankaj | CFX | 9 | November 23, 2009 04:05 |