CFX-Intro 14.5 WS07 Centrifugal-Pump [PDF]

Zitiervorschau

Workshop 07 Cavitating Centrifugal Pump 14. 5 Release

Introduction to ANSYS CFX © 2012 ANSYS, Inc.

December 17, 2012

1

Release 14.5

Introduction Workshop Description: The problem consists of a five-blade centrifugal pump operating at 2160 rpm. The working fluid is water and flow is assumed to be steady and incompressible. Due to rotational periodicity a single-blade passage will be modeled. The initial flow-field will be solved without cavitation. It will be turned on later.

Learning Aims: This workshop introduces several new skills: • Working with rotating domains • Modeling cavitation in ANSYS CFX

Learning Objectives: To model cavitation in a centrifugal pump, which involves the use of a rotation domain and the cavitation model. Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 2

Summary Release 14.5

Workbench 1. Start Workbench and save the project as centrifugalpump.wbpj 2. Drag a CFX system into the Project Schematic from the Component Systems toolbox 3. Start CFX-Pre by double clicking Setup

4. When CFX-Pre opens import the mesh by right-clicking on Mesh and selecting Import Mesh > ICEM CFD 5. Browse to pump.cfx5 (workshop_input_files\WS_07_Cavitating Pump) 6. Keep Mesh units in m 7. Click Open

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 3

Summary Release 14.5

Creating Working Fluids Modifying the material properties:

1. Expand Materials in the Outline tree 2. Double-click Water 3. On the Material Properties tab change Density to 1000 [kg/m3] 4. Expand Transport Properties and change Dynamic Viscosity to 0.001 [kg m^-1 s^-1] 5. Click OK

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 4

Summary Release 14.5

Setting up the Fluid Domain 1.

Double-click on Default Domain

2.

Under Fluid and Particle Definitions, delete Fluid 1 and then create a new Fluid named Water Liquid

3.

Set Material to Water

4.

Create another new Fluid named Water Vapour

5.

Next to the Material drop-down list, click the “…” icon, then the Import Library Data icon (on the right of the form), and select Water Vapour at 25 C under the Water Data object

• 6.

Click OK

Back in the Material panel, select Water Vapour at 25 C

•

Click OK

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 5

Summary Release 14.5

Setting up the Fluid Domain 7.

Set the Reference Pressure to 0 [Pa]

8.

Set Domain Motion to Rotating

9.

Set Angular Velocity to 2160 [rev min^-1]

10. Switch on Alternate Rotation Model. The Alternate Rotation Model is used to avoid “False swirl” which could occur when a significant amount of the fluid is flowing in the axial direction. 11. Make sure Rotation Axis under Axis Definition is set to Global Z 11. Switch to the Fluid Models tab and set the following: 12. Turn on Homogeneous Model in the Multiphase section 13. Under Heat Transfer set the Option to Isothermal, with a Temperature of 25 C 14. Set Turbulence Option to Shear Stress Transport 15. Click OK

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 6

Summary Release 14.5

Inlet Boundary Condition 1. Insert a boundary condition named Inlet 2. On the Basic Settings tab, set Boundary Type to Inlet 3. Set Location to INLET

4. Set Frame Type to Stationary 5. Switch to the Boundary Details tab 6. Specify Mass and Momentum with a Normal Speed of 7.0455 [m/s] 7. Switch to the Fluid Values tab 8. For Water Liquid, set the Volume Fraction to a Value of 1 9. For Water Vapour, set the Volume Fraction to a Value of 0 10. Click OK

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 7

Summary Release 14.5

Outlet Boundary Condition 1. Inset a boundary condition named Outlet 2. On the Basic Settings tab, set Boundary Type to Opening 3. Set Location to OUT

4. Set Frame Type to Stationary 5. Switch to the Boundary Details tab 6. Specify Mass and Momentum using Entrainment, and enter a Relative Pressure of 600,000 [Pa] 7. Enable the Pressure Option and set it to Opening Pressure 8. Set Turbulence Option to Zero Gradient 9. Switch to the Fluid Values tab 10. For Water Liquid, set the Volume Fraction to a Value of 1 11. For Water Vapour, set the Volume Fraction to a Value of 0 12. Click OK Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 8

Summary Release 14.5

Periodic Interface 1. Click

to create an Interface, and name it Periodic

2. On the Basic Settings tab set the Interface Type to Fluid Fluid 3. For Interface Side 1 set the Region List to DOMAIN INTERFACE 1 SIDE 1 and DOMAIN INTERFACE 2 SIDE 1 (use the “…” icon and the Ctrl key) 4. For Interface Side 2, set the Region List to DOMAIN INTERFACE 1 SIDE 2 and DOMAIN INTERFACE 2 SIDE 2 5. Set the Interface Models option to Rotational Periodicity 6. Under Axis Definition, select Global Z 7. Switch to the tab labelled Mesh Connection and set Option to 1:1 8. Click OK Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 9

Summary Release 14.5

Wall Boundary Conditions 1.

Insert a boundary condition named Stationary

2.

Set it to be a Wall, using the STATIONARY location

3.

On the Boundary Details tab, enable a Wall Velocity and set it to Counter Rotating Wall By default, all walls in a rotating domain rotate with the rotating reference frame. Since this wall is stationary in the absolute frame it must be counter rotating in the rotating frame.

4.

Click OK

5.

In the Outline Tree right-click on the Default Domain Default boundary and Rename it to Moving

•

The default behavior for the Moving boundary condition is to move with the rotating domain. So there is nothing that needs to be set

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 10

Summary Release 14.5

Initialization 1.

Click

to initialize the solution

2.

On the Fluid Settings form, set Water Liquid Volume Fraction to Automatic with Value, and set the Volume Fraction to 1

3.

Set Water Vapour Volume Fraction to Automatic with Value, and set the Volume Fraction to 0

4.

Click OK

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 11

Summary Release 14.5

Solver Control 1.

Double click Solver Control in the Outline tree

2.

Set Timescale Control to Physical timescale A commonly used timescale in turbomachinery is 1/omega, where omega is the rotation rate in radians per second. You can use an expression to determine a timestep from this. In this case, 2/omega will be used to achieve faster convergence.

3.

Enter the following expression in the Physical Timescale box: 1/(pi*2160 [min^-1])

4.

Set Residual Target to 1e-5

5.

On the Advanced Options tab turn on Multiphase Control. Then turn on Volume Fraction Coupling and set the Option to Coupled. This will speed up convergence

6.

Click OK

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 12

Summary Release 14.5

Output Control 1.

Double-click on Output Control in the Outline tree

2.

On the Monitor tab turn on Monitor Objects

3.

Under Monitor Points and Expressions, create a new object and call it InletPTotalAbs

4.

Set Option to Expression

5.

Enter the following expression: massFlowAve(Total Pressure in Stn Frame )@Inlet

6.

Create a new object called InletPStatic and set Option to Expression

7.

Enter the following expression: areaAve(Pressure )@Inlet

8.

Click OK

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 13

Summary Release 14.5

Solver 1.

Close CFX-Pre and switch to the Workbench Project Schematic window

2.

Save the project

3.

Now double-click on Solution in the Project Schematic to start the CFXSolver Manager

4.

When the CFX-Solver Manager opens click Start Run

This run takes about 9 minutes. To save time you can stop the run after a few iterations (in the Project Schematic right-click on the Solution cell and choose Interrupt Solution) and continue with an existing results file

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 14

Summary Release 14.5

Solver If running to completion, then when the solution has finished close the CFXSolver Manager and return to the Project Schematic window. Save the project. OR

If you have stopped the run early, save the project. Drag and drop the provided results file, CFX_001.res, into the Project Schematic

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 15

Summary Release 14.5

Post-processing 1.

View the results in CFD-Post by double-clicking Results cell in the component system, in the Project Schematic, that contains the completed solution.

2.

Insert a Contour by clicking

3.

For the Location click , , expand Regions and then select BLADE

4.

Set Variable to Absolute Pressure from the extended list

5.

Set Range to Global

6.

On the Render tab switch off Lighting and Show contour Lines

7.

Click Apply

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 16

Summary Release 14.5

Post-processing 8.

Create a contour on the HUB location, using the variable Absolute Pressure over the Local Range. Turn off Lighting and Show Contour Lines.

9.

Create a contour on the SHROUD location, using the variable Absolute Pressure coloured by Local Range. Turn off Lighting and Show Contour Lines. The minimum pressure is above the saturation pressure of 2650 Pa for water here. In the next step the outlet pressure will be reduced so as to induce cavitation.

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 17

Summary Release 14.5

Adding another Analysis 1.

Close CFD-Post and return to the Project Schematic

2.

Click the arrow next to the A cell and select Duplicate

•

A copy of the first CFX system is created

3.

Change the name of the new system to Cavitation

4.

Use the arrow next to the A cell to Rename it to No Cavitation

5.

Save the Project

6.

Double-click Setup for the Cavitation simulation to open CFX-Pre

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 18

Summary Release 14.5

Physics Modifications 1.

Edit the Default Domain

2.

On the Fluid Pair Models tab set Mass Transfer to Cavitation

3.

Set Option to Rayleigh Plesset. Leave the Mean Diameter (mean nucleation site diameter) set to 2e-6 [m]. This is a reasonable value.

4.

Turn on Saturation Pressure

5.

Set a Saturation Pressure of 2650 [Pa]

6.

Click OK

7.

Edit the Outlet Boundary Condition

8.

On the Boundary Details tab, set the Relative Pressure to 300,000 [Pa]

9.

Click OK

Most cavitation solutions should be performed by turning cavitation on and then successively lowering the system pressure over several runs to induce cavitation gradually. To speed up this workshop a sudden change in pressure is introduced. Note that this approach may not be suitable for modelling some industrial cases. Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 19

Summary Release 14.5

Physics Modifications 1.

Edit Solver Control

2.

Set the Max. Iterations to 150

3.

Set the Residual Target to 1e-4

4.

Click OK

5.

Close CFX-Pre and save the project

6.

In the Project Schematic drag cell A3 on to cell B3 or B2 on to C3

• 7.

Double-click Solution for the Cavitation system

•

8.

The non-cavitating solution will be used as the initial guess for the cavitating solution

In the CFX-Solver Manager note that the initial conditions have been provided by the Project Schematic

Click Start Run Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 20

Summary Release 14.5

Cavitation Solution There is a significant spike in residuals, in part due to the outlet pressure difference, but also due to the fact that the absolute pressure is low enough to induce cavitation. 1.

This run takes about 12 minutes. Either allow the run to complete, close the CFXSolver Manager and return to the Project Schematic or stop the run after a few iterations.

2.

Save the project

3.

If you ran the simulation to completion, double-click Results for the Cavitation project to open CFD-Post. If you stopped the run early then drag and drop CFX_002.res, provided, into the schematic and open those results in CFD-Post. Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 21

Summary Release 14.5

Post-processing 1.

If it is not enabled, turn on visibility for the Wireframe and turn off visibility for any User Locations and Plots

2.

Create an XY Plane at Z = 0.01 [m]

3.

Colour it by Absolute Pressure ( Range

•

). Use a Global

The minimum absolute pressure is equal to the saturation pressure specified earlier. This suggests that some cavitation has occurred

4.

Change the Colour Variable to Water Vapour.Volume Fraction

5.

Change the Colour Map to Blue to White

Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 22

Summary Release 14.5

Post-processing 1.

Turn off visibility for Plane 1

2.

Create a Volume using the Isovolume method

3.

Set the Variable to Water Vapour.Volume Fraction

4.

Set Mode to Above Value, and enter a value of 0.5

5.

To view 360 degrees of the model, double-click Default Transform

6.

Uncheck Instancing Info from Domain

7.

Set Number of Graphical Instances to 5

8.

Make sure that Apply Rotation is checked

9.

Under Axis Definition set Method to Principal Axis and select the Z axis

10. Under Instance Definition set Number of Passages to 5

11. Click OK Introduction © 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 23

Summary Release 14.5

Summary The main area of cavitation exists between the suction side of the blade and the shroud in this geometry. A secondary area of cavitation is just behind the leading edge of the blade on the pressure side.

Further steps to try: 1.

Calculate torque on the BLADE using the function calculator (hint, use the extended region list to find the BLADE and use Global Z axis)

2.

Plot velocity vectors on Plane 1, using the variable Water Liquid.Velocity in Stn. Frame

3.

Calculate the mass flow through the pump (hint: use the function calculator to evaluate massFlow at the Outlet region)

4.

Using a similar method to step 2, calculate the drop in Total Pressure from Inlet to Outlet

5.

Plot Streamlines, starting from the Inlet location Introduction

© 2012 ANSYS, Inc.

December 17, 2012

No cavitation

Cavitation 24

Summary Release 14.5