Basic Nozzle-Expander Design
 

Hi all,
I am proceeding towards design of a nozzle-expander system. Please help me in understanding the output and correct geometry if needed. I have uploaded images showing my input in Vista-RTD, input in CFX and final results of velocity profile.

Expander design
1. I input required parameters as shown in Vista-RTD for the expander and created the Expander geometry in BladeGen. I have included input of each step from Vista-RTD.

Nozzle design
2. I used the nozzle assumption on Pic 1 from Vista-RTD to create a nozzle in BladeGen.

3. I used the inlet velocity triangle on Pic 4 to match the RELATIVE INLET FLOW ANGLE (W2) = 40.66 degrees required by expander to match the nozzle ABSOLUTE FLOW ANGLE.

CFX Input

4.I brought in CFX-MESH for both expander and nozzle and show my input in Pic 6. I input same inlet pressure and temperature as in Vista-RTD and same outlet mass flowrate (0.23 kg/s divided by 13 blade passages = 0.0176 kg/s) as in Vista-RTD.
I used conditions at inlet of expander to be same as inlet of nozzle for the time being since I didn't analyze the nozzle separately (I hope this doesn't affect the flow angle problem I am witnessing in the results!)

CFX-Post

5.I have attached the velocity profile I obtain in Pic 7. As I interpret it I can see separation and possibly the inlet flow angle to the expander is not correct?.

Question-
6. Please help understand the interpretation from the velocity profile I obtained how to correct the geometry or any input I have mistaken.

Thank you all for your previous help to familiarize myself with the programs and now I need help to understand results and interprete to create a proper geometry.

Karmavatar

Anybody please to help me on this topic.
Mr. Glenn Horrocks if you could help me please.
Thank you,

But what are you trying to do? Looks like a blade geometry with lots of big separations to me so it does not appear to be operating well.

Glenn,
Yes, there are lot of separations. But I am not able to understand how to correct it.
I matched nozzle absolute velocity direction to rotor relative velocity direction and I have see big separation.
Please give me some direction what to check and look for to correct this.
Thank you,
Karmavatar

I have no experience in rotating machinery design. Looks like you need to get some textbooks on rotating machinery design.

Thanks Glenn.

Anybody who is working on either turbine or compressor blade geometry and simulation, I would appreicate if you could give me a direction on this.
Thank you,
Karmavatar

hI karmavatar
I have some difficulties in creating a nozzle in Ansys ,I found you had made it . Did you create the nozzle in the VISTA RTD or you design it in the Bladegen ?
Thank you

Hello,
Please help with my questions.
How to correct blade geometry by looking at results.
Blade geometry was created for certain input by Bladegen.
But, CFD results don't match with inputs.

Thanks in advance.

How to fix a blade design - look in a turbomechinery design textbook.

Inaccurate results - This is an FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Hi, I've got expierences about turbomachinery. Could you upload your CCL from Solver? Then it will be easier to help you :) And also put here more images, for example view from preprocessor to see how you set up boundary conditions.

Thank you tomson199 for replying.
I will upload CCL solver in next few days.

I have background in turbomachinery and have extensive course work using books like Dixon, Wilson, Aungier etc. and for CFD like Anderson and understand the equations, terminology and the language. I understand inverse solver and equations for creating geometry like BladeGen. I understand pros and cons of different types of meshing in CFD.
Except I haven't been able to go through the CFD software portion of it, successfully yet.. not even once.... due to lack of a guide or guidance.


I simply want to know and understand if it is traditional or typical method or usual practice to look at output characteristics (flow separations, pressure, entropy etc.) of the impeller/diffuser etc. and then go back manually to edit the blade profile. Is this iterative process typically done by trial and error?.

As Bladegen created the geometry using those inputs, I was expecting CFD outputs to be close (not exact) to those inputs, and that I would need to make minimal changes to the blade profile (for next iterations). But, the results are so off. I will check my inputs to CFX again.

Thank you very much for extending help.

Hello Thomas,
Please find below CCL details. I will post pictures if required.
Thank you,


+--------------------------------------------------------------------+
| |
| CFX Command Language for Run |
| |
+--------------------------------------------------------------------+

LIBRARY:
MATERIAL: Air Ideal Gas
Material Description = Air Ideal Gas (constant Cp)
Material Group = Air Data, Calorically Perfect Ideal Gases
Option = Pure Substance
Thermodynamic State = Gas
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Molar Mass = 28.96 [kg kmol^-1]
Option = Ideal Gas
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 1.0044E+03 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0. [J/kg]
Reference Specific Entropy = 0. [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 1.831E-05 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 2.61E-2 [W m^-1 K^-1]
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 0.01 [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
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: Expander
Coord Frame = Coord 0
Domain Type = Fluid
Location = PassageBody1
BOUNDARY: Expander Blade
Boundary Type = WALL
Frame Type = Rotating
Location = Blade1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Expander Hub
Boundary Type = WALL
Coord Frame = Coord 0
Frame Type = Rotating
Location = Hub1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Expander Outlet
Boundary Type = OUTLET
Frame Type = Stationary
Location = Outflow1
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Mass Flow Rate = 0.216154 [kg s^-1]
Option = Mass Flow Rate
END
END
END
BOUNDARY: Expander Shroud
Boundary Type = WALL
Coord Frame = Coord 0
Frame Type = Rotating
Location = Shroud1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
WALL VELOCITY:
Option = Counter Rotating Wall
END
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Expander to Expander Periodic 1 Side 1
Boundary Type = INTERFACE
Location = PeriodicA1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Expander to Expander Periodic 1 Side 2
Boundary Type = INTERFACE
Location = PeriodicB1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Expander to Nozzle Interface Side 2
Boundary Type = INTERFACE
Location = Inflow1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
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:
Alternate Rotation Model = true
Angular Velocity = 30000 [rev min^-1]
Option = Rotating
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.3
END
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 1 [atm]
END
END
FLUID DEFINITION: Air Ideal Gas
Material = Air Ideal Gas
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Option = Total Energy
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k epsilon
END
TURBULENT WALL FUNCTIONS:
High Speed Model = Off
Option = Scalable
END
END
END
DOMAIN: Nozzle
Coord Frame = Coord 0
Domain Type = Fluid
Location = PassageBody1 2
BOUNDARY: Expander to Nozzle Interface Side 1
Boundary Type = INTERFACE
Location = Outflow1 2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Nozzle Blade
Boundary Type = WALL
Location = Blade1 2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Nozzle Hub
Boundary Type = WALL
Location = Hub1 2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Nozzle Inlet
Boundary Type = INLET
Location = Inflow1 2
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
HEAT TRANSFER:
Option = Total Temperature
Total Temperature = 390 [K]
END
MASS AND MOMENTUM:
Option = Total Pressure
Relative Pressure = 1580 [kPa]
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: Nozzle Shroud
Boundary Type = WALL
Location = Shroud1 2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Nozzle to Nozzle Periodic 1 Side 1
Boundary Type = INTERFACE
Location = PeriodicA1 2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Nozzle to Nozzle Periodic 1 Side 2
Boundary Type = INTERFACE
Location = PeriodicB1 2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
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 = 1 [atm]
END
END
FLUID DEFINITION: Air Ideal Gas
Material = Air Ideal Gas
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Option = Total Energy
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k epsilon
END
TURBULENT WALL FUNCTIONS:
High Speed Model = Off
Option = Scalable
END
END
END
DOMAIN INTERFACE: Expander to Expander Periodic 1
Boundary List1 = Expander to Expander Periodic 1 Side 1
Boundary List2 = Expander to Expander Periodic 1 Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = Rotational Periodicity
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.3
END
END
MESH CONNECTION:
Option = Automatic
END
END
DOMAIN INTERFACE: Expander to Nozzle Interface
Boundary List1 = Expander to Nozzle Interface Side 1
Boundary List2 = Expander to Nozzle Interface 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 = Value
Pitch Ratio = 1
END
END
MESH CONNECTION:
Option = GGI
END
END
DOMAIN INTERFACE: Nozzle to Nozzle Periodic 1
Boundary List1 = Nozzle to Nozzle Periodic 1 Side 1
Boundary List2 = Nozzle to Nozzle Periodic 1 Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = Rotational Periodicity
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.3
END
END
MESH CONNECTION:
Option = Automatic
END
END
OUTPUT CONTROL:
MONITOR OBJECTS:
EFFICIENCY OUTPUT:
Inflow Boundary = Nozzle Inlet
Option = Output To Solver Monitor
Outflow Boundary = Expander Outlet
END
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 = 100
Minimum Number of Iterations = 1
Timescale Control = Auto Timescale
Timescale Factor = 1.0
END
CONVERGENCE CRITERIA:
Residual Target = 1.E-4
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
END
END
COMMAND FILE:
Version = 13.0
Results Version = 13.0
END
SIMULATION CONTROL:
EXECUTION CONTROL:
EXECUTABLE SELECTION:
Double Precision = Off
END
INTERPOLATOR STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
END
PARALLEL HOST LIBRARY:
HOST DEFINITION:
Host Architecture String = winnt
Installation Root = D:\Program Files\ANSYS Inc\v%v\CFX
END
END
PARTITIONER STEP CONTROL:
Multidomain Option = Independent Partitioning
Runtime Priority = Standard
EXECUTABLE SELECTION:
Use Large Problem Partitioner = Off
END
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARTITIONING TYPE:
MeTiS Type = k-way
Option = MeTiS
Partition Size Rule = Automatic
END
END
RUN DEFINITION:
Run Mode = Full
Solver Input File = CFX.def
END
SOLVER STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARALLEL ENVIRONMENT:
Number of Processes = 1
Start Method = Serial
END
END
END
END

Screenshots 1 through 5

Screenshots 6 through 10

Screenshots 11 through 15

Hi karmavatar.
In the first look I think that you did mistake in this turbine design. Are you compare your desing with hand made calculations? Because you used a cp=1712 J/kgK and gas constant R=317 J/kgK and then you use in CFX air as ideal gas when those parameters are different. Secondly why you applied expansion ratio 9? This is too big, because you cannot expand gas above 2,58 pressure ratio if you don't use convergent-divergent nozzle. The last think is pitch ratio. You have 9 blades of nozzle and 13 blades of expander, and you cannot apply this values. In the one side it should be 360/13 and the second side you should use 360/9.

Hey,
I do not fully understand your questions. Are you asking why there are big flow separations in the plot? To see more details accurately, you need to see the relative Mach contours along near the hub and midspan and near the shroud, at least 3 sections.

The rotor inlet (2) velocity triangle cartoon implies a CW rotation, but the nozzle cartoon itself shows a CCW rotation of the rotor. The nozzle outlet angle should be aligned with V2 (rotor absolute inlet flow), not with W2 (rotor relative inlet flow). By the combination of blade velocity U2, the relative inlet velocity W2 is found to be aligned with the rotor incidence angle. Every your velocity triangle does not match with those pictures. Because of the wrong design, in the CFX velocity contours you can see the wrong direction of velocity vector at the rotor inlet. The correct design should show the flow vector from top to bottom at the rotor inlet. Please compare yours with what I attached here (found from web).

Why do your rotor parts look apart in the velocity contour plot, BTW?

What you are dealing with is called the radial-inflow turbine which we can easily see in turbochargers.

Thank you Thomas, Thank you Turbo

Turbo has identified a fundamental problem with velocity diagram with my Bladegen. What I need is a CCW rotating Radial Turbine, for which velocity diagrams should be as in attached picture, but Bladegen velocity diagram is opposite, although the 3D geometry of the expander wheel appear correct. I am trying to figure out how to correct this velocity triangle (from forums and Bladegen help files), but Turbo if you know already, please help.

I also understood that "The nozzle outlet angle should be aligned with V2 (rotor absolute inlet flow), not with W2 (rotor relative inlet flow)".

Thank you

Why don't you go back to the starting line? Your meanline design (Vista whatever) was totally wrong.

Please suggest software to create impeller geometry other than Ansys.
I have seen demo of Axstream and looking for similar software names.
Thank you

I've never used the Vista whatever programs in the workbench, but guess you used it in a wrong way probably. I do not think they are totally collapsed to give you the false velocity triangles. Read the manual if any.