CFX-Intro 14.5 WS06 AxialFanStage [PDF]

Zitiervorschau

Workshop 06 Axial Fan Stage (MFR) 14.5 Release

Introduction to ANSYS CFX 1

© 2012 ANSYS, Inc.

December 17, 2012

Release 14.5

Introduction • Workshop Description: – This Workshop deals with an Axial Fan stage operating at 2880 rpm. The working fluid is Air Ideal Gas and flow is assumed to be steady.

Shroud

Outlet m’ = 0.3kg/s

Stator Blade (20) w = 2880 rev/min

– Due to rotational periodicity a single blade passage will be modeled.

• Learning Aims: – Working outside Workbench – Working with rotating domains – Basic setup using multiple frames

Inlet pt = 1.0 bar Tt = 288 K

Rotor Blades (30) Hub

of reference – Turbo-specific post-processing Introduction 2

© 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation

Summary Release 14.5

Multiple Frames of Reference • Axial, radial & mixed turbo machines, mixing vessels

• Diverse component installations – Gaps, tip clearance, … • Available models: – Stage: stationary calculation, circumferential averaging – Frozen Rotor: stationary calculation, frozen blade position – Transient Rotor Stator: transient calculation, rotating interface mapping, rotor-stator interaction – 3 Transient Blade Row methods: • Time Transform - Inlet Disturbance, Stage TRS • Fourier Transform - Inlet Disturbance, Stage TRS & Blade Flutter Introduction 3

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Pre-processing Goals • Using Stand-Alone CFX Mode(outside of

• • • • • •

Workbench) Launch CFX-Pre from CFX-Launcher Define stationary and rotating domain Define boundary conditions Define rotor stator interface Set up monitor points using simple expressions Define turbomachinery specific solver parameters

• Launch CFD-Post • Rotate, zoom and pan the view • Initialize turbo postprocessing • Define turbo surface • Use turbo coordinates for contour plots.

• Launch the CFX Solver Manager

Introduction 4

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Start a CFX-Pre • Start CFX-Launcher

– Start > All Programs > ANSYS 14.5 > Fluid Dynamics > CFX 14.5

• Start CFX-Pre from CFX-Launcher

• Choose “New Case”

• General Introduction 5

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Import Mesh • Select File > Import > Mesh • Change Files of Type: CFX Mesh (*.gtm *.cfx)

1

• Browse to workshop_input_files\WS_06_ \AxialFanStage

• Select Rotor.gtm • Click on “Open”

3

• Next Import the Stator.gtm

2 6

© 2012 ANSYS, Inc.

December 17, 2012

4

Release 14.5

Imported meshes

7

© 2012 ANSYS, Inc.

December 17, 2012

Release 14.5

Define Expressions • Create expressions that will be used later to define the speed of rotation and the physical timescale for convergence control

• Right-click on Expressions > Insert > Expression – Name: myRotationSpeed – Value: 2880 [rev min^-1] • Define physical timescale for solver control – Name: myPhysicalTimescale – Value: 1 [rad]/myRotationspeed – Dependency on rotation speed Introduction 8

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Domain: Stator (S1) • Select (Basic Settings): – “Create Domain”: S1 – Location: Passage 2 – Material: Air Ideal Gas – Reference Pressure: 1[bar] – Domain Motion: Stationary

Introduction 9

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Domain: Stator (S1) • Select (Fluid Models): – Heat Transfer: Total Energy – Turbulence: Shear Stress Transport – Click “OK”

Introduction 10

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Domain: Rotor (R1) • Select (Basic Settings): – “Create Domain”: R1 – Location: Passage – Material: Air Ideal Gas – Reference Pressure: 1[bar] – Domain Motion: Rotating – Angular Velocity: myRotationSpeed • Use expression symbol to enter expression! • Right-click in box and select expression – Rotation Axis: Global Z

Introduction 11

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Domain: Rotor (R1) • Select (Fluid Models): – Heat Transfer: Total Energy – Turbulence: Shear Stress Transport – Click “OK” Note: By default Constant Domain Physics is active (Case Options > General Options > Settings) and so these options should already be set. Introduction 12

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Boundary: Inlet (in R1) • Select: – Right-click on Domain R1 > Insert > Boundary – Name: R1 Inlet – Boundary Type: Inlet – Location: INFLOW – Frame Type: Stationary

Introduction 13

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Boundary: Inlet (in R1) • Select: – Mass And Momentum – Option: Stat. Frame Tot. Press. – Relative Pressure: 0 [Pa] – Flow Direction: Normal to Boundary Condition – Turbulence: Medium – Stat. Frame Total Temperature: 288 [K] – Click “OK” Introduction 14

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Boundary: Blade and Hub (in R1) • Select: – Right-click on Domain R1 > Insert > Boundary – Name: R1 Blade – Boundary Type: Wall – Location: BLADE – Frame Type: Rotating Boundary Details tab: – Mass And Momentum: No Slip Wall – Wall Roughness: Smooth Wall – Heat Transfer: Adiabatic

– Click “OK”

• Similarly define new Wall Boundary “R1 Hub” – Location: HUB Introduction 15

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Boundary: Shroud (in R1) • Select:

– Right-click on Domain R1 > Insert > Boundary – Name: R1 Shroud – Boundary Type: Wall – Location: SHROUD – Frame Type: Rotating – Click on the Boundary Details tab • Check the box for Wall Velocity • Set the Option to Counter Rotating Wall (Counter Rotating in rotating system = stationary in global system) – Click “OK” Introduction 16

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Boundary: Outlet (in S1) • Select: – Right-click on Domain S1 > Insert > Boundary – Name: S1 Outlet – Boundary Type: Outlet – Location: OUTFLOW 2

Introduction 17

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Boundary: Outlet (in S1) • Select: – Mass Flow Rate: 0.3 [kg s^-1] – Click “OK”

Introduction 18

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Create Wall Boundaries in S1 • Create additional Wall boundaries: – S1 Hub: Location: HUB 2 – S1 Shroud: Location: SHROUD 2 – S1 Blade: Location: BLADE 2 • Set Boundary Conditions to: – Mass And Momentum: No Slip Wall – Heat Transfer: Adiabatic

Introduction 19

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Periodic Interfaces • Periodic Interface are defined to connect the two sides of each domain

Introduction 20

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Periodic Interface: Rotor Domain • Select: – Domain Interface – Name: R1 Periodic – Interface Type = Fluid Fluid – Domain (Filter): R1 (for both sides) – Region List: • PER1 (Side 1) • PER2 (Side 2) – Interface Model: Rotational Periodicity – Rotation Axis: Global Z – Click “OK”

– NOTE: Each side of the interface is a boundary in the domain! Introduction 21

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Periodic Interface: Stator Domain • Select: – Domain Interface – Name: S1 Periodic – Interface Type= Fluid Fluid – Domain (Filter): S1 (for both sides) – Region List: • PER1 2 (Side 1) • PER2 2(Side 2) – Interface Model: Rotational Periodicity – Rotation Axis: Global Z – Click “OK” Introduction 22

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Stage Interface: Rotor to Stator • Select: – Domain Interface – Name: R1 to S1 – Domain (Filter): • R1 (Side 1) • S1 (Side 2) – Region List: • OUTFLOW (Side 1) • INFLOW 2 (Side 2) – Frame Change/Mixing Model: Stage – Downstream Velocity Constraint: Stage Average Velocity Introduction 23

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Check boundaries/interfaces defined • Check the outline tree for the boundaries and interfaces defined!

Introduction 24

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Solver Control • Double-click Solver Control • Advection Scheme: High Resolution

• Turbulence Numerics: First Order • Max Iterations: 200 • Physical Timescale: myPhysicalTimescale – Click on expression symbol – Right-click in box and select expression

• Residual Type: MAX • Residual Target: 0.001 Introduction 25

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Output Control Switch on Efficiency Output • Double-click on Output Control

• Select Monitor Tab > Monitor Objects

– Tick Efficiency Output – Efficiency Type : Compression – Value: Total to Total – NOTE: The efficiency calculates both the Isentropic and Polytropic efficiencies

26

© 2012 ANSYS, Inc.

December 17, 2012

Release 14.5

Output Control • Define expressions for monitoring during the run. • Pdiff gives the pressure rise developed by the fan.

Attention: The monitor name must differ from the expression name!

Introduction 27

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Output Control • Create the following expressions to calculate Power consumed by the fan

• Define number of rotor blades expression

– Name: nRotor – Value: 30 • Define power expression

– Name: power – Value: (torque_z()@R1 Blade +

torque_z()@R1 Hub)*myRotationSpeed/1 [rad] *nRotor

• Define Monitor Point for Power

– Name: Power – Expression Value: power 28

© 2012 ANSYS, Inc.

December 17, 2012

Release 14.5

Obtaining a solution • Launch CFX-Pre from CFX-Launcher • Define stationary and rotating domain • Define boundary conditions • Define rotor stator interface • Set up monitor points using simple expressions • Define turbomachinery specific solver parameters

• Launch CFD-Post • Rotate, zoom and pan the view • Initialize turbo postprocessing • Define turbo surface • Use turbo coordinates for contour plots.

• Launch the CFX Solver Manager • Check solution process Introduction 29

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Write the definition file • Right-click on Simulation Control and select Start Solver > Define Run • Save the definition (def) file when prompted

• The CFX-Solver Manager will open automatically

Introduction 30

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Run the CFX-Solver • The Solver Input File (definition file) for the run will already be specified • If possible, set up a local parallel run

• Click on Start Run

Introduction 31

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Monitor (Power) • The monitors for power and pressure difference will automatically appear in a window labelled User Points • The pressure rise developed by the fan is about 1155 Pa • The power consumed is about 6452 W

Introduction 32

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Monitor (Efficiency) • To view the Efficiency Output you will need a new monitor windows • Select Workspace > New Monitor • Right-click in the window and select Monitor Properties • Click on the Plot Lines tab and expand EFFICIENCY in the tree • Check the boxes for both the Isentropic and the Polytropic Compression • For both the value is about 87.5%

Introduction 33

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

Post-processing Goals • Launch CFX-Pre from CFX-Launcher • Define stationary and rotating domain • Define boundary conditions • Define rotor stator interface • Set up monitor points using simple expressions • Define turbomachinery specific solver parameters

• Launch CFD-Post • Rotate, zoom and pan the view • Initialize turbo post-processing • Define turbo surface • Use turbo coordinates for contour plots.

• Launch the CFX Solver Manager • Check solution process

Introduction 34

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

CFD-Post • Launch CFD-Post from CFXLauncher • Load results: – File  Load Results

Introduction 35

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

CFD-Post • Enter Turbo-Post • Auto-initialize turbo components • Based on naming conventions – Blade – Hub – Shroud – Inlet – Outlet

Introduction 36

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

CFD-Post • After initialization, turbospecific locations are available in CFD-Post – Turbo Surface – Turbo Line • For details, please refer to Appendix A Turbo

Introduction 37

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

CFD-Post • Define turbo surface – Constant Span = 0.5

Introduction 38

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

CFD-Post • Define Contour Plots for

– Mach Number – Total Pressure – Total Pressure in Stn Frame Note that, when there are rotating frames, some extra variables are created, e.g. Total Pressure in Stn Frame, Velocity in Stn Frame. These are referred to the stationary rather than the rotating frame and so are useful for visualization. Introduction 39

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

CFD-Post • Change transformation – Blade-to-Blade (ThetaM’)

• For details, please refer to Appendix A Turbo

Introduction 40

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

CFD-Post • Generate Vectors on Turbo-surface • In Blade-to-Blade-view

Introduction 41

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5

CFD Post • Quantitative Postprocessing

– Evaluating Fan stage performance using – – – – –

42

‘Gas Compressor Performance Macro’ Go to Tools > Macro calculator Select Macro: Gas Compressor Performance Specify Inputs as shown in picture Click on ‘Calculate’ Click on ‘View Report’

© 2012 ANSYS, Inc.

December 17, 2012

Release 14.5

Summary • This workshop has shown a basic setup using multiple frames of reference • An interface dealing with the frame change has been defined (frozen rotor) • Post-processing in turbo-specific coordinate system has been defined • Transformation of coordinates for visualisation has been set

Introduction 43

© 2012 ANSYS, Inc.

Setup December 17, 2012

Solving

Postprocessing

Summary Release 14.5