Wrong flow in ratating domain problem

Sanyo · August 10, 2015, 05:25

Dear All,

Greetings. I am trying to simulate a solid-liquid decanter along with air. Decanter is an equipment which uses centrifugal force to separate solid & liquid phase. It is a rotating drum. Inside rotating drum there is rotating screw. Direction of rotation & RPM for both is identical. There is a small gap of 0.25-1 mm in drum & screw. On left side of drum there is a weir controlled liquid outlet while at right side elevated solid outlet. Both outlet are open to atmosphere. Screw rotation is such that it will push the solids towards solid outlet. In addition, there is dominant air volume which needs to be considered. I have modeled air & water as continuous phase & solid particles as discrete phase (not the DPM). Rotation of drum & screw is modeled using rotating domain & frozen rotor interface (There is stationary inlet pipe before drum).

In reality, solids are collected from solid outlet while liquid passes to liquid outlet thru small gap between drum & screw. Weir at outlet controls the liquid level. However in simulation everything is passing thru solid outlet only due to conveying motion of screw. We have tried refining mesh in the gap, used stage & transient rotor approach, changed flow rates & RPM; but no use. Now its quite a time we are struggling with this problem & its frustrating now. Is there any way to solve this problem?

Another problem with this simulation is mass balance is not achieved. Sometimes there is difference of 0.1% but sometimes the mass going out of the system is much more than the mass coming into the system. But I guess this might be because of dead air volume inside equipment which is causing accumulation of the mass.

Thanks in advance.

Regards,

Sanyo

ghorrocks · August 10, 2015, 07:02

Please show some images of what you are modelling, your mesh and your CCL.

Sanyo · August 11, 2015, 07:33

LIBRARY:
CEL:
EXPRESSIONS:
AreaIn = area()@INLET
UpVFAir = 1-UpVFWater
UpVFWater = step((Radius -rw)/1[m])
Vin = vol flow /AreaIn
flow = 15
rw = 0.12 [m]
vol flow = (flow /3600) [m^3 s^-1]
END
END
COORDINATE FRAME DEFINITIONS:
COORDINATE FRAME: Coord 1
Axis 3 Point = 0.0[m],0.0[m],1.0[m]
Coord Frame Type = Cartesian
Option = Axis Points
Origin Point = 0.0[m],0.0[m],0.0[m]
Plane 13 Point = 1.0[m],0.0[m],0.0[m]
Reference Coord Frame = Coord 0
END
END
MATERIAL: Air at 25 C
Material Description = Air at 25 C and 1 atm (dry)
Material Group = Air Data, Constant Property Gases
Option = Pure Substance
Thermodynamic State = Gas
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 1.185 [kg m^-3]
Molar Mass = 28.96 [kg kmol^-1]
Option = Value
END

DYNAMIC VISCOSITY:
Dynamic Viscosity = 1.831E-05 [kg m^-1 s^-1]
Option = Value
END

MATERIAL: FLUID SOLIDS
Material Description = Water (liquid)
Material Group = Water Data,Constant Property Liquids
Option = Pure Substance
Thermodynamic State = Liquid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 2200 [kg m^-3]
Molar Mass = 18.02 [kg kmol^-1]
Option = Value
END

DYNAMIC VISCOSITY:
Dynamic Viscosity = 8.899E-4 [kg m^-1 s^-1]
Option = Value
END

MATERIAL: Water
Material Description = Water (liquid)
Material Group = Water Data,Constant Property Liquids
Option = Pure Substance
Thermodynamic State = Liquid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 1150 [kg m^-3]
Molar Mass = 18.02 [kg kmol^-1]
Option = Value
END

DYNAMIC VISCOSITY:
Dynamic Viscosity = 0.0015 [Pa s]
Option = Value
END

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 = Auto Detected Volume 28,HEX,Auto Detected Volume 27
BOUNDARY: Air Opening
Boundary Type = OPENING
Frame Type = Stationary
Location = AIR OPENING
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Opening Pressure and Direction
Relative Pressure = 0 [Pa]
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
FLUID: Solids
BOUNDARY CONDITIONS:
VOLUME FRACTION:
Option = Value
Volume Fraction = 0
END
END
END
END
BOUNDARY: Domain Interface 1 Side 2
Boundary Type = INTERFACE
Location = INTERFACE INLET
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Domain Interface 2 Side 1
Boundary Type = INTERFACE
Location = INTERFACE DISTRIBUTOR 01_2,INTERFACE DISTRIBUTOR \
02_2,INTERFACE DISTRIBUTOR 03_2,INTERFACE DISTRIBUTOR 04_2
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Domain Interface 2 Side 2
Boundary Type = INTERFACE
Location = INTERFACE DISTRIBUTOR 01,INTERFACE DISTRIBUTOR 02,INTERFACE \
DISTRIBUTOR 03,INTERFACE DISTRIBUTOR 04
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: OUTLET LIQUID
Boundary Type = OUTLET
Frame Type = Rotating
Location = OUTLET LIQUID
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Static Pressure
Relative Pressure = 0 [Pa]
END
END
END
BOUNDARY: OUTLET SOLID
Boundary Type = OUTLET
Frame Type = Rotating
Location = OUTLET SOLID
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Static Pressure
Relative Pressure = 0 [Pa]
END
END
END
BOUNDARY: WALL DISTRIBUTER
Boundary Type = WALL
Frame Type = Rotating
Location = DISTRIBUTOR
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: WALL DRUM
Boundary Type = WALL
Frame Type = Rotating
Location = DRUM,WALL HEX DRUM
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: WALL OUTLETS
Boundary Type = WALL
Frame Type = Rotating
Location = WALL LIQUID OUT,WALL SOLID OUT,WALL OTHER
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: WALL SCREW
Boundary Type = WALL
Frame Type = Rotating
Location = SCREW,WALL HEX SCREW
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: WALL SHAFT
Boundary Type = WALL
Frame Type = Rotating
Location = SHAFT
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 = 2000 [rev min^-1]
Option = Rotating
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.1
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 DEFINITION: Solids
Material = FLUID SOLIDS
Option = Material Library
MORPHOLOGY:
Mean Diameter = 50 [micron]
Option = Dispersed Solid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
FLUID: Solids
KINETIC THEORY MODEL:
Option = None
END
SOLID BULK VISCOSITY:
Option = None
END
SOLID PRESSURE MODEL:
Option = None
END
SOLID SHEAR VISCOSITY:
Option = None
END
END
HEAT TRANSFER MODEL:
Homogeneous Model = On
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = SST
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
FLUID PAIR: Air | Liquid
INTERPHASE TRANSFER MODEL:
Option = Free Surface
END
MASS TRANSFER:
Option = None
END
SURFACE TENSION MODEL:
Option = None
END
END
FLUID PAIR: Air | Solids
INTERPHASE TRANSFER MODEL:
Option = Particle Model
END
MASS TRANSFER:
Option = None
END
SURFACE TENSION MODEL:
Option = None
END
END
FLUID PAIR: Liquid | Solids
INTERPHASE TRANSFER MODEL:
Option = Particle 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 = UpVFAir
END
END
END
FLUID: Liquid
INITIAL CONDITIONS:
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = UpVFWater
END
END
END
FLUID: Solids
INITIAL CONDITIONS:
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 0
END
END
END
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = 0 [bar]
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 I
Coord Frame = Coord 0
Domain Type = Fluid
Location = STATIONARY VOL
BOUNDARY: Domain Interface 1 Side 1 2
Boundary Type = INTERFACE
Location = INTERFACE INLET_2
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: INLET
Boundary Type = INLET
Location = INLET
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Normal Speed = Vin
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 = 0.9451
END
END
END
FLUID: Solids
BOUNDARY CONDITIONS:
VOLUME FRACTION:
Option = Value
Volume Fraction = 0.0549
END
END
END
END
BOUNDARY: WALL INLET
Boundary Type = WALL
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:
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 DEFINITION: Solids
Material = FLUID SOLIDS
Option = Material Library
MORPHOLOGY:
Mean Diameter = 50 [micron]
Option = Dispersed Solid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
FLUID: Solids
KINETIC THEORY MODEL:
Option = None
END
SOLID BULK VISCOSITY:
Option = None
END
SOLID PRESSURE MODEL:
Option = None
END
SOLID SHEAR VISCOSITY:
Option = None
END
END
HEAT TRANSFER MODEL:
Homogeneous Model = On
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = SST
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
FLUID PAIR: Air | Liquid
INTERPHASE TRANSFER MODEL:
Option = Free Surface
END
MASS TRANSFER:
Option = None
END
SURFACE TENSION MODEL:
Option = None
END
END
FLUID PAIR: Air | Solids
INTERPHASE TRANSFER MODEL:
Option = Particle Model
END
MASS TRANSFER:
Option = None
END
SURFACE TENSION MODEL:
Option = None
END
END
FLUID PAIR: Liquid | Solids
INTERPHASE TRANSFER MODEL:
Option = Particle 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 = 0
END
END
END
FLUID: Liquid
INITIAL CONDITIONS:
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 1
END
END
END
FLUID: Solids
INITIAL CONDITIONS:
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 0
END
END
END
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = -4.5 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = 0 [bar]
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 2
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
DOMAIN INTERFACE: Domain Interface 2
Boundary List1 = Domain Interface 2 Side 1
Boundary List2 = Domain Interface 2 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:
BACKUP RESULTS: Backup Results 1
File Compression Level = Default
Option = Standard
OUTPUT FREQUENCY:
Iteration Interval = 50
Option = Iteration Interval
END
END
RESULTS:
File Compression Level = Default
Option = Standard
END
END
SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Blend Factor = 0.75
Option = Specified Blend Factor
END
CONVERGENCE CONTROL:
Length Scale = 1 [m]
Length Scale Option = Specified Length Scale
Maximum Number of Iterations = 2000
Minimum Number of Iterations = 1000
Timescale Control = Auto Timescale
Timescale Factor = 1.0
END
CONVERGENCE CRITERIA:
Residual Target = 0.00001
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = Yes
END

ghorrocks · August 11, 2015, 07:45

What stops the solids from flowing through the 1mm gap? They look like 50um particles and a 1mm gap so they would fit through.

Does the solids form a packed bed or agglomerate? CFX does not have models for this.

What stops the liquid flowing out the solid outlet? Or does the screw push the solids above the fluid level, so they are pretty dry?

Sanyo · August 11, 2015, 11:56

Solid particles agglomerate and screw pushes particles above water level. We intend to follow SPH (solid particle harmonics) method in later stage of project for particle modelling. But for now liquid phenomenon is important.

Are we modeling rotations in wrong way? Is there any other method to model rotation? Or any other method to model the problem?

ghorrocks · August 11, 2015, 20:06

Well, there's your problem. CFX has no agglomeration model, and no mechanism by which you can push the particles out of the water. So it appears CFX lacks two key bits of physics you need to model this device. So I don't think you can model your device with CFX - at least without developing a particle agglomeration model and a method of pushing particles out of the water.

Sanyo · August 12, 2015, 03:13

Thanks for reply. I agree that it needs special treatment for particles. But at this moment, we are concerned about the water behavior. It should pass thru 1mm gap & leave the domain from liquid outlet which is at left side. But simulation shows liquid passing thru solid outlet (right side outlet). What could be the reason of this opposite behavior?

ghorrocks · August 12, 2015, 06:47

Please show images of your mesh and the flow results you are getting.

Sanyo · August 12, 2015, 08:11

Centreplane shows the liquid volume fraction accumulation.
When i try streamlines using velocity in stn frame, the streamlines are ending abruptly. i tried to increase the limits but not useful.

ghorrocks · August 12, 2015, 20:28

This device lies horizontally, doesn't it? And gravity keeps the liquid at the bottom of the screw? The final image shows that liquid is right the way around the device. This appears to be a fundamental problem in the way you are modelling it.

Sanyo · August 13, 2015, 06:44

The device do lie horizontally. But the decanter separates the phases using centrifugal force. G force in decanter goes well beyond 1000-2000 times more than gravitational force making gravity insignificant.

CFX doesn't allow to solve rotating domain with gravity direction not aligned with rotation axis in steady state. I have to solve it as transient simulation.

I think RFR approach is not suitable for this kind of problems. If I define the wall velocity instead of rotating domain, will it solve the problem? I know that I have to go for mesh deformation option but will it help to capture the physics? How wall velocity option treats the fluid?

ghorrocks · August 13, 2015, 07:00

I see - so yes, in this case gravity is not important and can be ignored. So then I can see the solids will form a mud and the liquid will get centrifuged out and trickle along the outside wall. But what moves the solids towards the solids outlet?

Why do you think RFR is not suitable? It appears the only practical way of doing it to me.

I think your problem is that you have not included important physical models, and nothing to do with RFR. I have already said CFX has no agglomeration model and no method of pushing solids out of the liquid - these seem like fundamental effects to me. But I do not understand the operating principle of this device yet so I may well be wrong.

Sanyo · August 13, 2015, 12:24

Solids are pushed out of device by screw movement. Yes we are not modeling the agglomeration. But if I do not model solid for the moment & only model air+water, in that case I should get the correct fluid behavior, right?? But in that case also, I am getting same behavior. Will it help by modeling the rotating domain differently say just near the screw & drum by few millimeters? In that case rest of the domain can be kept stationary.

ghorrocks · August 13, 2015, 19:20

Is the outer wall stationary and the screw moving inside? Or does it all move together?

Sanyo · August 14, 2015, 01:44

The outerwall, screw, and distributor rotates at same speed & direction. Only inlet pipe is stationary.

ghorrocks · August 14, 2015, 09:27

Then what makes the solids move up to the solids outlet? They have to go against the centripetal force to get there (they need to go uphill) so they are not going to get there unless something pushes them. What is pushing the solids uphill?

Sanyo · August 14, 2015, 11:04

Probably this video can clear the concept.

https://www.youtube.com/watch?v=FhS5vN4r5LA

ghorrocks · August 15, 2015, 07:20

Looking at a few of the videos on the topic they say there is a speed differential between the scroll/screw and the shell. I cannot see how the solids would move without a speed differential between the screw and the shell.

It appears you have modelled the screw and the shell as having the same speed. This is a fundamental problem in your model, isn't it?

Anyway, back to your original question:
Why is the liquid going out the solids outlet? This would suggest the resistance in going through the gap is too large, or you have not run the simulation long enough. Can you show a cross section of your mesh through the gap region?

Why not achieve mass balance? You might need to run a tighter convergence. But first determine whether it is important to get mass balance more accurate. If it is not required then don't bother to get it.

August 10, 2015, 05:25	Wrong flow in ratating domain problem	#1
Sanyo Member Sanyo Join Date: Apr 2009 Location: India Posts: 62 Rep Power: 17	Dear All, Greetings. I am trying to simulate a solid-liquid decanter along with air. Decanter is an equipment which uses centrifugal force to separate solid & liquid phase. It is a rotating drum. Inside rotating drum there is rotating screw. Direction of rotation & RPM for both is identical. There is a small gap of 0.25-1 mm in drum & screw. On left side of drum there is a weir controlled liquid outlet while at right side elevated solid outlet. Both outlet are open to atmosphere. Screw rotation is such that it will push the solids towards solid outlet. In addition, there is dominant air volume which needs to be considered. I have modeled air & water as continuous phase & solid particles as discrete phase (not the DPM). Rotation of drum & screw is modeled using rotating domain & frozen rotor interface (There is stationary inlet pipe before drum). In reality, solids are collected from solid outlet while liquid passes to liquid outlet thru small gap between drum & screw. Weir at outlet controls the liquid level. However in simulation everything is passing thru solid outlet only due to conveying motion of screw. We have tried refining mesh in the gap, used stage & transient rotor approach, changed flow rates & RPM; but no use. Now its quite a time we are struggling with this problem & its frustrating now. Is there any way to solve this problem? Another problem with this simulation is mass balance is not achieved. Sometimes there is difference of 0.1% but sometimes the mass going out of the system is much more than the mass coming into the system. But I guess this might be because of dead air volume inside equipment which is causing accumulation of the mass. Thanks in advance. Regards, Sanyo

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
mass flow rate not conserved in turbomachine, interface defined wrong?	wildli	FLUENT	3	September 15, 2022 13:19
Modeling the flow domain in Icepak	saisanthoshm88	ANSYS	1	December 12, 2011 01:20
[DesignModeler] Flow Domain of DesignModeler	swiss_zhang	ANSYS Meshing & Geometry	0	June 9, 2011 08:13
Modeling the flow domain in Icepak	saisanthoshm88	Main CFD Forum	0	April 11, 2011 09:31
problem in modeling flow over a 3d airfoil	guess	Main CFD Forum	8	March 20, 2010 14:54

August 10, 2015, 07:02		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Please show some images of what you are modelling, your mesh and your CCL.

August 11, 2015, 07:45		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	What stops the solids from flowing through the 1mm gap? They look like 50um particles and a 1mm gap so they would fit through. Does the solids form a packed bed or agglomerate? CFX does not have models for this. What stops the liquid flowing out the solid outlet? Or does the screw push the solids above the fluid level, so they are pretty dry?

August 11, 2015, 11:56		#5
Sanyo Member Sanyo Join Date: Apr 2009 Location: India Posts: 62 Rep Power: 17	Solid particles agglomerate and screw pushes particles above water level. We intend to follow SPH (solid particle harmonics) method in later stage of project for particle modelling. But for now liquid phenomenon is important. Are we modeling rotations in wrong way? Is there any other method to model rotation? Or any other method to model the problem?

August 11, 2015, 20:06		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Well, there's your problem. CFX has no agglomeration model, and no mechanism by which you can push the particles out of the water. So it appears CFX lacks two key bits of physics you need to model this device. So I don't think you can model your device with CFX - at least without developing a particle agglomeration model and a method of pushing particles out of the water.

August 12, 2015, 03:13		#7
Sanyo Member Sanyo Join Date: Apr 2009 Location: India Posts: 62 Rep Power: 17	Thanks for reply. I agree that it needs special treatment for particles. But at this moment, we are concerned about the water behavior. It should pass thru 1mm gap & leave the domain from liquid outlet which is at left side. But simulation shows liquid passing thru solid outlet (right side outlet). What could be the reason of this opposite behavior?

August 12, 2015, 06:47		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Please show images of your mesh and the flow results you are getting.

August 12, 2015, 20:28		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	This device lies horizontally, doesn't it? And gravity keeps the liquid at the bottom of the screw? The final image shows that liquid is right the way around the device. This appears to be a fundamental problem in the way you are modelling it.

August 13, 2015, 06:44		#11
Sanyo Member Sanyo Join Date: Apr 2009 Location: India Posts: 62 Rep Power: 17	The device do lie horizontally. But the decanter separates the phases using centrifugal force. G force in decanter goes well beyond 1000-2000 times more than gravitational force making gravity insignificant. CFX doesn't allow to solve rotating domain with gravity direction not aligned with rotation axis in steady state. I have to solve it as transient simulation. I think RFR approach is not suitable for this kind of problems. If I define the wall velocity instead of rotating domain, will it solve the problem? I know that I have to go for mesh deformation option but will it help to capture the physics? How wall velocity option treats the fluid?

August 13, 2015, 07:00		#12
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	I see - so yes, in this case gravity is not important and can be ignored. So then I can see the solids will form a mud and the liquid will get centrifuged out and trickle along the outside wall. But what moves the solids towards the solids outlet? Why do you think RFR is not suitable? It appears the only practical way of doing it to me. I think your problem is that you have not included important physical models, and nothing to do with RFR. I have already said CFX has no agglomeration model and no method of pushing solids out of the liquid - these seem like fundamental effects to me. But I do not understand the operating principle of this device yet so I may well be wrong.

August 13, 2015, 12:24		#13
Sanyo Member Sanyo Join Date: Apr 2009 Location: India Posts: 62 Rep Power: 17	Solids are pushed out of device by screw movement. Yes we are not modeling the agglomeration. But if I do not model solid for the moment & only model air+water, in that case I should get the correct fluid behavior, right?? But in that case also, I am getting same behavior. Will it help by modeling the rotating domain differently say just near the screw & drum by few millimeters? In that case rest of the domain can be kept stationary.

August 13, 2015, 19:20		#14
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Is the outer wall stationary and the screw moving inside? Or does it all move together?

August 14, 2015, 01:44		#15
Sanyo Member Sanyo Join Date: Apr 2009 Location: India Posts: 62 Rep Power: 17	The outerwall, screw, and distributor rotates at same speed & direction. Only inlet pipe is stationary.

August 14, 2015, 09:27		#16
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Then what makes the solids move up to the solids outlet? They have to go against the centripetal force to get there (they need to go uphill) so they are not going to get there unless something pushes them. What is pushing the solids uphill?

August 14, 2015, 11:04		#17
Sanyo Member Sanyo Join Date: Apr 2009 Location: India Posts: 62 Rep Power: 17	Probably this video can clear the concept. https://www.youtube.com/watch?v=FhS5vN4r5LA

August 15, 2015, 07:20		#18
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Looking at a few of the videos on the topic they say there is a speed differential between the scroll/screw and the shell. I cannot see how the solids would move without a speed differential between the screw and the shell. It appears you have modelled the screw and the shell as having the same speed. This is a fundamental problem in your model, isn't it? Anyway, back to your original question: Why is the liquid going out the solids outlet? This would suggest the resistance in going through the gap is too large, or you have not run the simulation long enough. Can you show a cross section of your mesh through the gap region? Why not achieve mass balance? You might need to run a tighter convergence. But first determine whether it is important to get mass balance more accurate. If it is not required then don't bother to get it.