CFX Intro 14.5 WS13 Turbo Pre Post [PDF]

Zitiervorschau

Workshop 13 Axial Fan simulation using Turbo Pre and Post 14. 5 Release

Introduction to ANSYS CFX © 2012 ANSYS, Inc.

December 17, 2012

1

Release 14.5

Introduction A simple workshop follows to demonstrate how to use the Turbomachinery mode in CFX-Pre and CFD-Post. This workshop models an Axial fan. The model consists of a single rotating domain for the fan blade with stationary domains upstream and downstream of the blade.

The full axial fan contains ten blades. Due to rotational periodicity a single blade passage will be modeled. Frozen Rotor interfaces are used to connect the rotating and stationary domains. © 2012 ANSYS, Inc.

December 17, 2012

2

Release 14.5

Turbo-Pre 1. Open Workbench (Start > Programs > ANSYS 14.5 > ANSYS Workbench)

2. Drag CFX into the project schematic 3. Start CFX-Pre by double clicking Setup

4. Select Tools > Turbo Mode

© 2012 ANSYS, Inc.

December 17, 2012

3

Release 14.5

Basic Settings The Turbo mode uses a setup wizard to walk you through CFX-Pre. The first step is the Basic Settings panel: 1. Set the Machine Type to Fan 2. Select Z as the Rotation Axis • Notice that the rotational axis is displayed in the Viewer 3. Select Analysis Type as Steady State 4. Click Next >

© 2012 ANSYS, Inc.

December 17, 2012

4

Release 14.5

Component Definition The Component Definition panel is used to import meshes, select the rotation speed for each component and set the tip clearance (if any).

For this Axial Fan Tutorial there are 3 components to be defined Start by defining the 1st stationary component: 1.

Right-click in the Component Definition white space, and select Add Component…

2.

Select the Type as Stationary and set the Name to S1

3.

Select the Mesh File as fan.gtm (workshop_input_files\WS_13_TurboPrePost)

4.

Expand the Available Volumes frame and select the Volumes as INBlock Main

5.

Expand the Region Information frame and compare with the picture on the next page and make the necessary changes

© 2012 ANSYS, Inc.

December 17, 2012

5

Release 14.5

Component Definition The Region Information is used by CFXPre to identify mesh regions of interest. CFX-Pre will try to automatically identify these regions, but manual input may be required depending on how the regions are named in the mesh file. CFX-Pre will automatically create boundary conditions and domain interfaces using these regions, so checking the Region Information at this stage will save time later. • The mesh file contains all three components, but only one of those components is to be included in S1 • Default values can be used for all other options

• Do Not click the Next Button © 2012 ANSYS, Inc.

December 17, 2012

6

Release 14.5

Component Definition Now define the 2nd component which is rotating:

1. Right-click in the Component Definition white space, and select New Component… 2. Select Rotating and set the Name as R1 3. Set the Rotating Value to –3000 [rev min^-1] • The rotation direction is shown in the Viewer 4. Do not select a mesh file. The mesh has already been imported in the previous step.

Under Available Volumes select “Passage” 5. Expand the Wall Configuration frame. Set Tip Clearance at Shroud to YES and Tip Clearance at Hub to NO • This sets boundary conditions for a fan with a rotating hub and a counterrotating shroud surface © 2012 ANSYS, Inc.

December 17, 2012

7

Release 14.5

Component Definition 6. Expand the Region Information frame and compare with the picture below and make the necessary changes

• This sets boundary conditions for a fan with a rotating hub and a counter-rotating shroud surface • Do Not click the Next Button. © 2012 ANSYS, Inc.

December 17, 2012

8

Release 14.5

Component Definition Now define the 3rd component which is stationary: 1. Create a new stationary component named S2 2. Under Available Volumes select OUTBlock Main 3. Expand the Passages and Alignment frame • The number of Passages in 360 and the number of Passages To Model is determined automatically • You can change the automatic values or apply a Theta Offset by clicking the Edit button, but this is not necessary for this case, so click cancel

4. Expand the Region Information frame and compare with the picture next page and make the necessary changes © 2012 ANSYS, Inc.

December 17, 2012

9

Release 14.5

Component Definition

5. Click Next > to proceed

© 2012 ANSYS, Inc.

December 17, 2012

10

Release 14.5

Physics Definition All Physics settings, including Fluid Type, Inlet & Outlet boundary conditions, Interface types, and Solver Parameters are set in one panel. 1. The default Fluid and Model Data are appropriate for this simulation 2. Select Boundary Template as P-Total Inlet Mass Flow Outlet • The Boundary Template provides quick setup of the most common turbomachinery boundary combinations

3. Set P-Total to 0 [atm] 4. Set Flow Direction to Cylindrical Components with direction set to 1,0,0

5. Set Mass Flow to Per Component and then enter a Mass Flow Rate of 0.04 [kg s^-1] © 2012 ANSYS, Inc.

December 17, 2012

11

Release 14.5

Physics Definition – Cont’d… 6. Change the Interface Default Type to Frozen Rotor 7. Expand the Solver Parameters frame 8. Set the Convergence Control to Physical Timescale with a value of 0.02 [s] (select the expression icon to allow this to be entered) • This sets the timescale to roughly 6/ω, where ω is the machine rotational speed in [rad/s]. Typically, the timescale for rotating machinery is specified somewhere between 0.1/ω and 10/ω.

9. Click Next > to proceed

© 2012 ANSYS, Inc.

December 17, 2012

12

Release 14.5

Interface Definition Interfaces are automatically created using the Region Information from the Component Definition panel. 1. Select each interface to verify it has been created correctly • There are two Frozen Rotor interfaces, three Periodic interfaces and an interface near the blade tip to connect dissimilar meshes together • The interfaces have been correctly created 2. Click Next > to continue © 2012 ANSYS, Inc.

December 17, 2012

13

Release 14.5

Boundary Definition Boundary conditions are also automatically created using the Region Information from the Component Definition panel and information from the Physics Definition panel. 1. Select each boundary condition to verify the settings are appropriate 2. Select Next > to continue

© 2012 ANSYS, Inc.

December 17, 2012

14

Release 14.5

Final Operations The Final Operations panel allows you to Enter General Mode. Enter General Mode is useful if you want to use other CFX-Pre features (profile boundaries, CEL etc) but still complete most of the set up using the Turbomachinery mode.

1. Click Finish

© 2012 ANSYS, Inc.

December 17, 2012

15

Release 14.5

Solver and CFD-Post 1. Switch to the Projects window

2. Select File > Save 3. Enter the File name as turbo_demo.wbpj and click Save 4. Now double-click on Solution in the Project Schematic to start the Solver Manager

5. When the Solver Manager opens, click Start Run © 2012 ANSYS, Inc.

December 17, 2012

16

Release 14.5

Turbo-Post In CFD-Post the following features will be demonstrated: •

Auto Initialize of Turbo Components

•

Modifying Turbo regions

•

Displaying Hubs and Blades using the 3D view

•

Create vector and contour plots using the Blade to Blade View

•

Create vector and contour plots using the Meridional View

•

Use of Turbo Charts and Macros

•

Table creation and viewing using the Table Viewer

© 2012 ANSYS, Inc.

December 17, 2012

17

Release 14.5

Turbo-Post GUI 1. Switch to the Projects window 2. View the results in CFD-Post by double clicking Results in the Project Schematic 3. In CFD-Post, click on the Turbo tab 4. Click Initialise All Components • For each component CFD-Post detects which regions correspond to the Hub, Shroud, Blade, Inlet, Outlet and Periodic regions. CFD-Post uses this information to make turbo plots and charts. You can manually assign these regions, or check the auto-assigned regions by editing each of the component object from the Turbo tree (Component 1 (S1), Component 2 (R1) and Component 3 (S2))

5. Select the Three Views toggle • You can toggle between a Single View and Three Views. The three views shown are a 3D view, a Blade to Blade View and a Meridional View © 2012 ANSYS, Inc.

December 17, 2012

18

Release 14.5

3D View 6. Edit the 3D View object from the Turbo tree • The Details of 3D View are shown

7. Select All Domains 8. Under Parts to Draw, select Hub and Blade 9. Toggle Show Faces on

10. Under Instancing, • • •

set Domain to R1, set # of Copies to 3 and then click Apply Now set Domain to S1, set # of Copies to 3 and click Apply Finally set Domain to S2, set # of Copies to 3 and click Apply

The 3D View now shows 3 copies of the Hub and Blade in each of the 3 components © 2012 ANSYS, Inc.

December 17, 2012

19

Release 14.5

Blade-to-Blade View Now create a Blade to Blade Vector Plot: 1. Edit the Blade-to-Blade object from the Turbo tree 2. Change Plot Type to Vector 3. Set Sampling to Equally Spaced and # of Points to 400

4. Click Apply • A Vector Plot is shown in the Blade-to-Blade View 5. Change Sampling from Equally Spaced to Vertex and click Apply • The Vector Plot now shows vectors starting from each mesh node © 2012 ANSYS, Inc.

December 17, 2012

20

Release 14.5

Blade-to-Blade View 6. In Details of Blade-to-Blade Plot, change the Plot Type to Contour and select the Variable as Total Pressure in Stn Frame, then click Apply. 7. Create a Stream plot of Velocity in the same way • Change the number of points to 100 8. Double-click on 3D View in the Turbo tree 9. Enable the Show Blade-to-Blade plot toggle and click Apply to show the blade-to-blade Stream plot in the 3D View © 2012 ANSYS, Inc.

December 17, 2012

21

Release 14.5

Meridional View 1. Edit the Meridional object from the Turbo tree 2. Generate a Contour plot of Pressure using a Local Range • A Contour plot is shown in the Meridional View 3. Now enable the Show Sample Mesh toggle (near the bottom of Details of Meridional Plot ) • A mesh is now shown on the Contour plot • This illustrates the resolution used in creating the meridional data

© 2012 ANSYS, Inc.

December 17, 2012

22

Release 14.5

Turbo-Post

© 2012 ANSYS, Inc.

December 17, 2012

23

Release 14.5

Turbo Charts & Macros Turbo Charts and Macros are also available: 1. Double-click on the Inlet to Outlet object under Turbo Charts in the Turbo tree 2. Increase the number of Samples/Comp. to 20

3. Examine some of the other Turbo Charts

© 2012 ANSYS, Inc.

December 17, 2012

24

Release 14.5

Tables The Table Viewer allows you to create a table that can be exported in .html, .csv, or .txt formats. You can also save a state file for a table for later use. Next you will create a table and export it to an html file

1. Select the Table Viewer tab from the bottom of the Viewer window 2. Select the New Table icon and accept the default name

from the Table Viewer toolbar

3. In cell A1 type: Mass Averaged Inlet Total Pressure 4. In cell B1, type: =massFlowAve(Total Pressure)@S1 Inlet • Alternatively you can use the Table Viewer toolbar to select Insert: Function > CFD-Post > massFlowAve, then Insert: Variable > Total Pressure, etc to build the expression © 2012 ANSYS, Inc.

December 17, 2012

25

Release 14.5

Tables 5. In cell A2 type: Mass Averaged Outlet Total Pressure 6. In cell B2, enter the equation: =massFlowAve(Total Pressure )@S2 Outlet

7. In cell A3 type: Omega 8. In cell B3, select Insert: Expression > omega or type: =omega © 2012 ANSYS, Inc.

December 17, 2012

26

Release 14.5

Tables 9. In cell A4 type: Filename 10. In cell B4, select Insert: Annotation > File Name > Name 11. Click the Save Table icon from the Table Viewer toolbar 12. Save the file as axial_table.html 13. Open this file in a web browser

© 2012 ANSYS, Inc.

December 17, 2012

27

Release 14.5

Turbo Reports CFX Post includes automatic report generation based on templates. A number of Turbo-specific templates are available: 1. From the main menu select File > Report > Report Templates…

2. Select Fan Report and click Load 3. Once the report has been generated, click on the Report Viewer tab 4. Browse through the report to see what has been included © 2012 ANSYS, Inc.

December 17, 2012

28

Release 14.5

Turbo Report You can add you own Figures, Tables, Charts and Comments to the report. Next you will add a figure to the end of the report showing a Vector plot at 50% span in the blade passage. 1. Click the Comment icon

from the main toolbar

2. Enter User Plots the for Name 3. Type the following in to the Comment Viewer :

© 2012 ANSYS, Inc.

December 17, 2012

29

Release 14.5

Turbo Report 4. Switch to the Report Viewer, and Refresh the report • The Refresh button is in the Report Viewer toolbar • The new comment will appear at the end of the report

© 2012 ANSYS, Inc.

December 17, 2012

30

Release 14.5

Turbo Report Now create a Velocity plot at 50% span:

1. Switch to Turbo tab 2. Double-click Blade-to-Blade from the Turbo tree

3. Set Span to 0.5 4. Set Plot Type to Vector and Variable to Velocity 5. Click Apply

© 2012 ANSYS, Inc.

December 17, 2012

31

Release 14.5

Turbo Report Now add this plot to you report: 1. Click the Figure icon from the main toolbar or RightClick in the viewer window and select “Copy to New Figure…”

2. Set the Name to Vector Midspan and click OK 3. Scroll to the bottom of the Outline tree • The Figure appears at the end of the Report 4. Switch to the Report Viewer tab and Refresh the report to see the changes © 2012 ANSYS, Inc.

December 17, 2012

32

Release 14.5

Turbo Plot Once the report is complete you can publish it to an html file 1. Click the Publish icon from the Report Viewer toolbar 2. Click OK to write the HTML file • The file and figures can be distributed as necessary

© 2012 ANSYS, Inc.

December 17, 2012

33

Release 14.5

CFD-Post You may want to try the following on your own, time permitting 1. Create various figures, tables, comments and charts that you might typically want to see in your analysis

2. Try enabling the Generate CFX-Viewer Files… toggle when publishing your report • Image in the report can then be rotated, zoomed and panned. The CFX Viewer must be installed on the machine viewing the report; this is freely available from the Customer Portal and does not require a license (so your customers can view your figures in 3D) © 2012 ANSYS, Inc.

December 17, 2012

34

Release 14.5