[Shaun Waters]

Hi all,

I am modelling an Archimedes Screw Turbine with CFX. I currently have three domains, one inlet and outlet domain which are both stationary. The third domain contains the turbine.

I created the turbine in Solidworks, and used Boolean Subtract on the turbine to create the turbine shaped hole in this domain.

I am only using water as the fluid, and have set buoyancy. I have tried using a steady state solution using the single frame of reference method by creating a rotating domain. I have also tried using the moving mesh method, by creating a subdomain and causing the mesh to rotate about the stationary domain.

For both, of these, I have very low torque values. For my set up, I have set a mass flow rate at the inlet and have a static pressure at the outlet. The simulation is in a tidal range situation, so has a net head of 5.25m. My turbine is set in a pipe like structure in a barrage wall. I've attached an image which explains it much better.

My Questions are:
1. Why am I getting such low values of torque? I am currently using torque_y()@Turbine (The axis of rotations is the y axis)
2. Is there a problem with my pressure calculations? I am using the formula: Pstatic = density*g*depth of fluid. As there is 5.25m of head at the inlet (lagoon) Pstatic = 51.5KPa, which I have set as the reference pressure. For the Static Pressure at the outlet, I have used the same formula, using the lower head value for the sea.

Thank you for any help,
Shaun

[ghorrocks]

I would not expect much torque out of a rotor like that. It looks horribly inefficient. Do you have quality data to compare against, or are you just guessing what you think the torque should be?

[Shaun Waters]

I have some comparable data which where the values are small. My model is a variation of the data I have, but I don't believe the different aspects I have included (fully submerged instead of partially) would affect the values this significantly.

What I don't understand is, when using the CFX Post calculator tab/Function calculator, when I select Torque and Location "turbine" these are the values I get. The axis of rotation is the Yaxis, but this value is by far the smallest?

torque_y()@Turbine
0.0391385 [N m]
torque_x()@Turbine
-15.2094 [N m]
torque_z()@Turbine
5.13368 [N m]

Thank for your help,
Shaun

[ghorrocks]

I would imagine this sort of thing would have massively different results comparing fully submerged to partially submerged. It usually makes a big difference in other areas (eg pump priming) Why do you say it will not make a difference?

I would have a careful look at the flow field you simulated to look for weirdness. Also have a look at the FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

[singer1812]

Are you putting any resistance (or inertia) in to the spin? Or are you prescribing the spin rate on the turbine?

[Opaque]

Have you checked the axis of rotation used by CFD-Post is the same used by the ANSYS CFX Solver ?

Go to the Turbo tab, and verify the axis of rotation in CFD-Post.

[Shaun Waters]

I'm not putting any resistance/inertia on the spin. I have given it a rotation rate.

I've checked the axis of rotation in Post as well. It is the same. I'm currently going through the Wiki for inaccuracy. Making the mesh better is my next step. I do not know how to use ICEM, so I am still using regular ansys meshing.

Thanks for the help so far,
Shaun

[singer1812]

Ok. Thinking off the cuff here, with you fixing the rotation rate and driving it at that, doesnt that add work into your system and lower/alter the torque that the screw would see from the flow, or impart to the flow?

Assume you spun (imparted rotation) to the screw at the exact right rate that the flow would normally drive the screw at on its own. I would anticipate that you would get zero torque reading.

So, if your torque value is very low, and you are driving the screw at a rate that experimental data suggests, then perhaps it is matching data?

The above ideas is provided without careful ferreting out of system forces, and I would confirm with a free body if I had the time, but you might check it out.

[ghorrocks]

And just checking: Have you modelled this as a rotating frame of reference or as a rigid body?

[Shaun Waters]

I am modelling it as a rotating frame of reference. The middle domain is set as rotating, with the other two (inlet and outlet) set as stationary. Frozen rotor interfaces connect the domains. The turbine is modeled as a wall inside the rotating domain and the enclosure it is in is set as a counter rotating wall.

I have now scaled it up to the size I am investigating. Approximately 7m in diameter and 10m in length. The sizes of torque I am getting are approximately 3.5e+6 with 150RPM, which when converted into power makes it approximately 55,000KW.
Power (kW) = Torque (N.m) x Speed (RPM) / 9.5488

The turbine I am comparing it to is a bulb turbine producing between 16MW and 20MW, and I am predicting this would be much, much lower.

My inlet and outlet conditions are correct, with flow rate information for the inlet and pressure at the outlet based on the hydrostatic pressure caused by 4m of water above the turbine outlet.

I have tried reducing the size of the mesh. I initially halved the mesh size, re-ran and halved it again. The change between the 2 and 3rd run was small.

I have used a physical timescale, based on the amount of time the fluid would take to flow through the turbine and it is converging at 1e-5.

Is there something I am forgetting with my setup? The turbine boundary condition is set as a no slip, smooth wall.

[ghorrocks]

Are you sure the frozen rotor approach is applicable here? I would need to think about that. If you want to be sure run one with transient rotor stator and see if it makes a difference.

[Shaun Waters]

I have modified the setup to a transient analysis instead of steady state, with transient rotor stator interfaces between the rotating domains and stationary domains, and the monitor points being recorded so far are even larger than when it was using frozen rotor and steady state simulation.

Currently, Torque = 2.1E+8.

[ghorrocks]

Something is seriously wrong here. Are you sure the surface you are getting the torque over is the full rotor? You are not just getting one side? Or you missed a bit?

[Shaun Waters]

I agree, I just can't see what is wrong. I have the whole turbine as a named selection = Turbine.

I am using the monitor point: "torque_z()@Turbine" The Z axis is the axis of rotation.

[ghorrocks]

You better check the turbine axis is along the Z axis, ie axis vector (0,0,1). Also check the torque function is giving torques about this same axis.

[Shaun Waters]

I believe the turbine axis is along the Z axis. I've added a new Coordinate 1 located at the central shaft of the turbine to check and modified the torque monitor point to:

torque_z_Coord 1()@Turbine. This picks up the same value as before.

I've refined the mesh even more to stop there being any dramatic size difference between domains. There are now over 11 million elements. There is adequate inflation at both the walls of the enclosure and around the turbine itself. The geometry is 7m in diameter and with the long inlet/outlet sections, it is 80m in length. This means the mesh sizes are still fairly large in comparison, could this be part of the issue? Although, I don't think my computer could handle many more nodes/elements.

[ghorrocks]

There is adequate inflation...

Unless you have actually checked whether it is adequate, then how can you say this? Have you done a sensitivity analysis?

Inadequate mesh can cause errors, but not as big as you are getting. I still think there is a fundamental error in your simulation. Can you post your CCL?

[Shaun Waters]

I have checked with CFX Post, looking at the pressure and velocity change around the inflation layers, as well as looking at the Y+ values. There are no sudden changes.

LIBRARY:
CEL:
EXPRESSIONS:
RPM = (2 * pi * 50) / 60 [rad/s]
VolFlow = massFlow()@inlet / areaAve(Density)@inlet
dPtot = massFlowAve(Total Pressure in Stn Frame)@Inlet - \
massFlowAve(Total Pressure in Stn Frame)@Outlet
trq = torque_z_Coord 1()@Turbine
volFlow = massFlow()@Inlet / areaAve(Density)@Inlet
END
END
COORDINATE FRAME DEFINITIONS:
COORDINATE FRAME: Coord 1
Centroid Type = Absolute
Invert Normal Axis Direction = Off
Location = F34.24
Option = Point and Normal
Origin = 1.83854e-007 [m], -2.27102e-007 [m], 30.1 [m]
Point on Axis 3 = 1.83854e-007 [m], -2.27102e-007 [m], 29.1 [m]
Point on Plane 13 = 1 [m], 0 [m], 0 [m]
Reference Coord Frame = Coord 0
END
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 = 997.0 [kg m^-3]
Molar Mass = 18.02 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 4181.7 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0.0 [J/kg]
Reference Specific Entropy = 0.0 [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 8.899E-4 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 0.6069 [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
THERMAL EXPANSIVITY:
Option = Value
Thermal Expansivity = 2.57E-04 [K^-1]
END
END
END
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: Z1
Coord Frame = Coord 0
Domain Type = Fluid
Location = B72,B46
BOUNDARY: Inlet
Boundary Type = INLET
Location = F47.46
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Mass Flow Rate = 297000 [kg s^-1]
Mass Flow Rate Area = As Specified
Option = Mass Flow Rate
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: Outlet
Boundary Type = OPENING
Location = F73.72
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 = 39240 [Pa]
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: Z12 Side 1
Boundary Type = INTERFACE
Location = F48.46
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Z1Wall
Boundary Type = WALL
Location = F75.72,F49.46
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Z23 Side 2
Boundary Type = INTERFACE
Location = F74.72
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Temperature = 10 [C]
Gravity X Component = 0 [m s^-2]
Gravity Y Component = 0 [m s^-2]
Gravity Z Component = -g
Option = Buoyant
BUOYANCY REFERENCE LOCATION:
Option = Automatic
END
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 0 [Pa]
END
END
FLUID DEFINITION: water
Material = Water
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Fluid Temperature = 10 [C]
Option = Isothermal
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = SST
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
END
DOMAIN: Z2
Coord Frame = Coord 0
Domain Type = Fluid
Location = B24
BOUNDARY: Turbine
Boundary Type = WALL
Frame Type = Rotating
Location = F28.24,F29.24,F30.24,F31.24,F32.24,F33.24,F34.24,F 35.24
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Z12 Side 2
Boundary Type = INTERFACE
Location = F27.24
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Z23 Side 1
Boundary Type = INTERFACE
Location = F26.24
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Z2Wall
Boundary Type = WALL
Frame Type = Rotating
Location = F25.24
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
WALL VELOCITY:
Option = Counter Rotating Wall
END
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Temperature = 10 [C]
Gravity X Component = 0 [m s^-2]
Gravity Y Component = 0 [m s^-2]
Gravity Z Component = -g
Option = Buoyant
BUOYANCY REFERENCE LOCATION:
Option = Automatic
END
END
DOMAIN MOTION:
Angular Velocity = -50 [rev min^-1]
Option = Rotating
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 1.3
END
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 0 [Pa]
END
END
FLUID DEFINITION: water
Material = Water
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Fluid Temperature = 10 [C]
Option = Isothermal
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = SST
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
END
DOMAIN INTERFACE: Z12
Boundary List1 = Z12 Side 1
Boundary List2 = Z12 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: Z23
Boundary List1 = Z23 Side 1
Boundary List2 = Z23 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:
MONITOR OBJECTS:
MONITOR BALANCES:
Option = Full
END
MONITOR FORCES:
Option = Full
END
MONITOR PARTICLES:
Option = Full
END
MONITOR POINT: Eff
Coord Frame = Coord 0
Expression Value = (torque_z_Coord 1()@Turbine * RPM) / (volFlow * \
dPtot)
Option = Expression
END
MONITOR POINT: Power
Coord Frame = Coord 0
Expression Value = trq*RPM
Option = Expression
END
MONITOR POINT: TrqC0
Coord Frame = Coord 0
Expression Value = torque_z()@Turbine
Option = Expression
END
MONITOR POINT: TrqC1
Coord Frame = Coord 1
Expression Value = torque_z()@Turbine
Option = Expression
END
MONITOR POINT: trq2
Coord Frame = Coord 1
Expression Value = torque_z_Coord 1()@Turbine
Option = Expression
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:
Maximum Number of Iterations = 500
Minimum Number of Iterations = 1
Physical Timescale = 10.9944 [s]
Timescale Control = Physical Timescale
END
CONVERGENCE CRITERIA:
Residual Target = 1e-5
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
END
END
COMMAND FILE:
Version = 16.1
Results Version = 16.1
END
SIMULATION CONTROL:
EXECUTION CONTROL:
EXECUTABLE SELECTION:
Double Precision = No
END
INTERPOLATOR STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
END
PARALLEL HOST LIBRARY:
HOST DEFINITION: ngd030000012
Host Architecture String = winnt-amd64
Installation Root = C:\Program Files\ANSYS Inc\v%v\CFX
END
END
PARTITIONER STEP CONTROL:
Multidomain Option = Automatic
Runtime Priority = Standard
EXECUTABLE SELECTION:
Use Large Problem Partitioner = Off
END
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARTITION SMOOTHING:
Maximum Partition Smoothing Sweeps = 100
Option = Smooth
END
PARTITIONING TYPE:
MeTiS Type = k-way
Option = MeTiS
Partition Size Rule = Automatic
END
END
RUN DEFINITION:
Run Mode = Full
Solver Input File = Fluid Flow CFX.def
Solver Results File = C:/Users/waterss/Desktop/Swansea Bay CFX/swansea \
bay v4_pending/dp0_CFX_6_Solution_6/Fluid Flow CFX_002.res
END
SOLVER STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1
END
PARALLEL ENVIRONMENT:
Number of Processes = 1
Start Method = Serial
END
END
END
END

Thanks for your help. I, and other students I have asked, are out of ideas of what could be wrong.

The 270,000kg/s mass flow rate is converted from 297m^3/s flow rate, which is what the turbine I am comparing it to used.

[ghorrocks]

Comments:

* Pedantic comment first - just enter the rotation speed as 50 [rpm]. No need for you to do the conversion.
* More pedantry: Why get volume flow from mass flow and density? Why not just calculate it directly?
* You have the outlet at 39kPa and zero reference pressure. You should have defined 39kPa as your reference pressure and zero pressure at the outlet.
* Why have you got gravity defined for this model?
* Back to pedantry: You define the rotation speed in your CEL but you redefine it in your rotating frame of reference. You should define it once in CEL and use the variable everywhere. Multiple definitions of the same variable will lead to mistakes.
* Talking about mistakes, you have two volflow variables: VolFlow and volFlow. They are defined as the same quantity. Delete one of them.

I have more comments after you have responded to these comments.

[Shaun Waters]

1 - I have changed the RPM input as suggested.
2 - Modified volume flow calculation
3 - Changed outlet pressure to 0 and reference pressure to 39kPa. With pressure, at the inlet I have the 297m^3/s volume flow rate and, 6.5m of water above the inlet. At the outlet the water level is less, with only 4m of water above the outlet. Should I be incorporating both of these pressure values somehow, or do I not need to include the 6.5m of water head at the inlet because I am using the volume flow rate at the inlet instead?
4 - I included gravity as part of the buoyancy, I originally tried to put gravity in the downwards direction to simulate real conditions, but had to put it in line with the axis of rotation as it is steady state. I have now turned buoyancy off until the issue with high torque is sorted.
5 - RPM is now referenced only once. 50RPM.
6 - There is now only one volFlow variable.

I've reposted my new CEL:

LIBRARY:
CEL:
EXPRESSIONS:
RPM = 50 [rev min^-1]
dPtot = massFlowAve(Total Pressure in Stn Frame)@Inlet - \
massFlowAve(Total Pressure in Stn Frame)@Outlet
trq = torque_z_Coord 1()@Turbine
volFlow = 297 [m^3 / s]
END
END
COORDINATE FRAME DEFINITIONS:
COORDINATE FRAME: Coord 1
Centroid Type = Absolute
Invert Normal Axis Direction = Off
Location = F34.24
Option = Point and Normal
Origin = 2.45915e-008 [m], 2.25138e-007 [m], 30.1 [m]
Point on Axis 3 = 2.45915e-008 [m], 2.25138e-007 [m], 29.1 [m]
Point on Plane 13 = 1 [m], 0 [m], 0 [m]
Reference Coord Frame = Coord 0
END
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 = 997.0 [kg m^-3]
Molar Mass = 18.02 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 4181.7 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0.0 [J/kg]
Reference Specific Entropy = 0.0 [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 8.899E-4 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 0.6069 [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
THERMAL EXPANSIVITY:
Option = Value
Thermal Expansivity = 2.57E-04 [K^-1]
END
END
END
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: Z1
Coord Frame = Coord 0
Domain Type = Fluid
Location = B72,B46
BOUNDARY: Inlet
Boundary Type = INLET
Location = F47.46
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Mass Flow Rate = 297000 [kg s^-1]
Mass Flow Rate Area = As Specified
Option = Mass Flow Rate
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: Outlet
Boundary Type = OPENING
Location = F73.72
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
END
BOUNDARY: Z12 Side 1
Boundary Type = INTERFACE
Location = F48.46
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Z1Wall
Boundary Type = WALL
Location = F75.72,F49.46
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Z23 Side 2
Boundary Type = INTERFACE
Location = F74.72
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
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 = 39240 [Pa]
END
END
FLUID DEFINITION: water
Material = Water
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Fluid Temperature = 10 [C]
Option = Isothermal
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = SST
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
END
DOMAIN: Z2
Coord Frame = Coord 0
Domain Type = Fluid
Location = B24
BOUNDARY: Turbine
Boundary Type = WALL
Frame Type = Rotating
Location = F28.24,F29.24,F30.24,F31.24,F32.24,F33.24,F34.24,F 35.24
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Z12 Side 2
Boundary Type = INTERFACE
Location = F27.24
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Z23 Side 1
Boundary Type = INTERFACE
Location = F26.24
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Z2Wall
Boundary Type = WALL
Frame Type = Rotating
Location = F25.24
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
WALL VELOCITY:
Option = Counter Rotating Wall
END
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Alternate Rotation Model = On
Angular Velocity = RPM
Option = Rotating
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 1.3
END
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 39240 [Pa]
END
END
FLUID DEFINITION: water
Material = Water
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Fluid Temperature = 10 [C]
Option = Isothermal
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = SST
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
END
DOMAIN INTERFACE: Z12
Boundary List1 = Z12 Side 1
Boundary List2 = Z12 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: Z23
Boundary List1 = Z23 Side 1
Boundary List2 = Z23 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:
MONITOR OBJECTS:
MONITOR BALANCES:
Option = Full
END
MONITOR FORCES:
Option = Full
END
MONITOR PARTICLES:
Option = Full
END
MONITOR POINT: Eff
Coord Frame = Coord 0
Expression Value = (trq * RPM) / (volFlow * dPtot)
Option = Expression
END
MONITOR POINT: Power
Coord Frame = Coord 0
Expression Value = trq*RPM
Option = Expression
END
MONITOR POINT: TrqC0
Coord Frame = Coord 0
Expression Value = torque_z()@Turbine
Option = Expression
END
MONITOR POINT: TrqC1
Coord Frame = Coord 1
Expression Value = torque_z()@Turbine
Option = Expression
END
MONITOR POINT: trq2
Coord Frame = Coord 0
Expression Value = trq
Option = Expression
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:
Maximum Number of Iterations = 500
Minimum Number of Iterations = 1
Physical Timescale = 11.8184 [s]
Timescale Control = Physical Timescale
END
CONVERGENCE CRITERIA:
Residual Target = 1e-5
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
END
END
COMMAND FILE:
Version = 16.1
Results Version = 16.1
END
SIMULATION CONTROL:
EXECUTION CONTROL:
EXECUTABLE SELECTION:
Double Precision = Yes
END
INTERPOLATOR STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
END
PARALLEL HOST LIBRARY:
HOST DEFINITION: ngd030000012
Host Architecture String = winnt-amd64
Installation Root = C:\Program Files\ANSYS Inc\v%v\CFX
END
END
PARTITIONER STEP CONTROL:
Multidomain Option = Automatic
Runtime Priority = Standard
EXECUTABLE SELECTION:
Use Large Problem Partitioner = Off
END
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARTITION SMOOTHING:
Maximum Partition Smoothing Sweeps = 100
Option = Smooth
END
PARTITIONING TYPE:
MeTiS Type = k-way
Option = MeTiS
Partition Size Rule = Automatic
END
END
RUN DEFINITION:
Run Mode = Full
Solver Input File = Fluid Flow CFX.def
Solver Results File = C:/Users/waterss/Desktop/Swansea Bay CFX/swansea \
bay v4_pending/dp0_CFX_6_Solution_6/Fluid Flow CFX_001.res
END
SOLVER STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1
END
PARALLEL ENVIRONMENT:
Number of Processes = 1
Start Method = Serial
END
END
END
END

It is now not converging as quickly and P-Mass is failing on pretty much every other iteration like this:

================================================== ====================
OUTER LOOP ITERATION = 22 CPU SECONDS = 7.707E+03
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom | 1.11 | 4.9E-04 | 4.9E-02 | 2.1E-01 ok|
| V-Mom | 1.01 | 4.8E-04 | 6.3E-02 | 2.0E-01 ok|
| W-Mom | 1.00 | 6.4E-04 | 5.5E-02 | 2.8E-01 ok|
| P-Mass | 1.14 | 5.4E-05 | 4.6E-03 | 9.3 1.2E+00 F |
+----------------------+------+---------+---------+------------------+
| K-TurbKE | 0.72 | 1.8E-03 | 1.8E-01 | 5.6 9.0E-02 OK|
| O-TurbFreq | 1.20 | 3.0E-03 | 6.6E-01 | 11.9 3.1E-04 OK|
+----------------------+------+---------+---------+------------------+

Torque values are still very high with the value currently at 1.7E+7 and it’s close to reaching a steady state value, only changing minutely between each iteration.

Thank you for the help so far.