|
[Sponsors] |
June 19, 2015, 11:45 |
Low torque values on Screw Turbine
|
#1 |
New Member
Shaun Waters
Join Date: Mar 2015
Posts: 19
Rep Power: 11 |
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 |
|
June 20, 2015, 07:47 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144 |
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?
|
|
June 20, 2015, 10:56 |
|
#3 |
New Member
Shaun Waters
Join Date: Mar 2015
Posts: 19
Rep Power: 11 |
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 |
|
June 21, 2015, 07:34 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144 |
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 |
|
June 22, 2015, 12:17 |
|
#5 |
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 21 |
Are you putting any resistance (or inertia) in to the spin? Or are you prescribing the spin rate on the turbine?
|
|
June 22, 2015, 15:05 |
|
#6 |
Senior Member
Join Date: Jun 2009
Posts: 1,875
Rep Power: 33 |
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. |
|
June 24, 2015, 12:40 |
|
#7 |
New Member
Shaun Waters
Join Date: Mar 2015
Posts: 19
Rep Power: 11 |
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 |
|
June 24, 2015, 13:32 |
|
#8 |
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 21 |
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. |
|
June 24, 2015, 20:44 |
|
#9 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144 |
And just checking: Have you modelled this as a rotating frame of reference or as a rigid body?
|
|
July 15, 2015, 12:44 |
|
#10 |
New Member
Shaun Waters
Join Date: Mar 2015
Posts: 19
Rep Power: 11 |
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. |
|
July 15, 2015, 20:32 |
|
#11 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144 |
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.
|
|
July 16, 2015, 11:47 |
|
#12 |
New Member
Shaun Waters
Join Date: Mar 2015
Posts: 19
Rep Power: 11 |
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. |
|
July 16, 2015, 19:53 |
|
#13 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144 |
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?
|
|
July 17, 2015, 06:03 |
|
#14 |
New Member
Shaun Waters
Join Date: Mar 2015
Posts: 19
Rep Power: 11 |
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. |
|
July 17, 2015, 07:29 |
|
#15 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144 |
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.
|
|
July 17, 2015, 12:14 |
|
#16 |
New Member
Shaun Waters
Join Date: Mar 2015
Posts: 19
Rep Power: 11 |
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. |
|
July 17, 2015, 18:58 |
|
#17 | |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144 |
Quote:
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? |
||
July 18, 2015, 17:09 |
|
#18 |
New Member
Shaun Waters
Join Date: Mar 2015
Posts: 19
Rep Power: 11 |
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. |
|
July 19, 2015, 08:06 |
|
#19 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144 |
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. |
|
July 19, 2015, 16:53 |
|
#20 |
New Member
Shaun Waters
Join Date: Mar 2015
Posts: 19
Rep Power: 11 |
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. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Wind turbine torque calculation is less than expected | AhmedMaklid | FLUENT | 1 | February 20, 2015 15:56 |
Low values of y Plus | kingmaker | OpenFOAM Running, Solving & CFD | 0 | September 23, 2013 09:00 |
Time step for Low pressure turbine simulation | Far | FLUENT | 17 | April 1, 2013 06:20 |
Low values of Lift force | vmlxb6 | CFX | 1 | February 2, 2011 06:13 |
How to calculate Torque for francis turbine | manish | CFX | 4 | March 15, 2007 03:57 |