1. Workshop 10 Turbo Pre and Post
Introduction to CFX
Pardad Petrodanesh.Co
Lecturer: Ehsan Saadati

2. 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.

3. Turbo-Pre
Open Workbench (Start > Programs > ANSYS 12.0 > ANSYS Workbench)
Drag CFX into the project schematic
Start CFX-Pre by double clicking Setup
Select Tools > Turbo Mode

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

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). Start by defining the first stationary component:
Right-click in the Component Definition white space, and select Add Component…
Select the Type as Stationary and set the Name to S1
Select the Mesh File as fan.gtm
Expand the Available Volumes frame and select the Volumes as INBlock Main
Expand the Region Information frame and compare with the picture on the next page and make the necessary changes

6. Component Definition
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
The Region Information is used by CFX-Pre 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.

7. Now define the rotating component:
Component Definition
Now define the rotating component:
Right-click in the Component Definition white space, and select New Component…
Select Rotating and set the Name as R1
Set the Rotating Value to –3000 [rev min^-1]
The rotation direction is shown in the Viewer
Do not select a mesh file. The mesh has already been imported in the previous step. Under Available Volumes select Passage
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 counter-rotating shroud surface

8. Component Definition
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

9. Component Definition Now define the second stationary component:
Create a new stationary component named S2
Under Available Volumes select OUTBlock Main
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
Expand the Region Information frame and compare with the picture next page and make the necessary changes

10. Component Definition
Click Next > to proceed

11. Physics Definition
All Physics settings, including Fluid Type, Simulation Type, Inlet and Outlet boundary conditions, Interface types, and Solver Parameters are set in one panel.
The default Fluid, Simulation Type and Model Data are appropriate for this simulation
Select Boundary Template as P-Total Inlet Mass Flow Outlet
The Boundary Template provides quick setup of the most common turbomachinery boundary combinations
Set P-Total to 0 [atm]
Set Mass Flow to Per Component and then enter a Mass Flow Rate of 0.04 [kg s^-1]
Set Flow Direction to Cylindrical Components with direction set to 1,0,0

12. Physics Definition Change the Interface Default Type to Frozen Rotor
Expand the Solver Parameters frame
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.
Click Next > to proceed

13. Interface Definition
Interfaces are automatically created using the Region Information from the Component Definition panel.
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
Click Next > to continue

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

15. 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.
Click Finish

16. Solver and CFD-Post Switch to the Projects window
Select File > Save
Enter the File name as turbo_demo.wbpj and click Save
Now double-click on Solution in the Project Schematic to start the Solver Manager
When the Solver Manager opens, click Start Run

17. 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

18. Turbo-Post GUI Switch to the Projects window
View the results in CFD-Post by double clicking Results in the Project Schematic
In CFD-Post, click on the Turbo tab
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))
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

19. 3D View Edit the 3D View object from the Turbo tree Select All Domains
The Details of 3D View are shown
Select All Domains
Under Parts to Draw, select Hub and Blade
Toggle Show Faces on
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

20. Blade-to-Blade View Now create a Blade to Blade Vector Plot:
Edit the Blade-to-Blade object from the Turbo tree
Change Plot Type to Vector
Set Sampling to Equally Spaced and # of Points to 400
Click Apply
A Vector Plot is shown in the Blade-to-Blade View
Change Sampling from Equally Spaced to Vertex and click Apply
The Vector Plot now shows vectors starting from each mesh node

21. Blade-to-Blade View
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
Create a Stream plot of Velocity in the same way
Change the number of points to 100
Double-click on 3D View in the Turbo tree
Enable the Show Blade-to-Blade plot toggle and click Apply to show the blade-to-blade Stream plot in the 3D View

22. Meridional View Edit the Meridional object from the Turbo tree
Generate a Contour plot of Pressure using a Local Range
A Contour plot is shown in the Meridional View
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

23. Turbo-Post

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

25. 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.
Select the Table Viewer tab from the bottom of the Viewer window
Select the New Table icon from the Table Viewer toolbar and accept the default name
In cell A1 type: Mass Averaged Inlet Total Pressure
In cell B1, type the equation: =massFlowAve(Total 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

26. Tables In cell A2 type: Mass Averaged Outlet Total Pressure
In cell B2, enter the equation: =massFlowAve(Total Pressure Outlet
In cell A3 type: Omega
In cell B3, select Insert: Expression > omega or type: =omega

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

28. Turbo Reports
CFX Post includes automatic report generation based on templates. A number of Turbo-specific templates are available:
From the main menu select File > Report > Report Templates…
Select Fan Report and click Load
Once the report has been generated, click on the Report Viewer tab
Browse through the report to see what has been included

29. Turbo Report Click the Comment icon from the main toolbar
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.
Click the Comment icon from the main toolbar
Enter User Plots the for Name
Type the following in to the Comment Viewer :

30. Turbo Report 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

31. Turbo Report Switch to Turbo tab
Now create a Velocity plot at 50% span:
Switch to Turbo tab
Double-click Blade-to-Blade from the Turbo tree
Set Span to 0.5
Set Plot Type to Vector and Variable to Velocity
Click Apply

32. Turbo Report Click the Figure icon from the main toolbar
Now add this plot to you report:
Click the Figure icon from the main toolbar
Set the Name to Vector Midspan and click OK
Scroll to the bottom of the Outline tree
The Figure appears at the end of the Report
Switch to the Report Viewer tab and Refresh the report to see the changes

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

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