1. In the Basic Settings panel, configure the following setting(s):

   Setting	Value
   Machine Type	Axial Turbine
   Analysis Type > Type	Steady State

2. Click Next.

1. Right-click in the blank area and select Add Component from the shortcut menu.

2. Create a new component of type Stationary, named S1.

3. Configure the following setting(s):

   Setting	Value
   Mesh > File	stator.gtm [ a ]
   Click Browse   to open the Import Mesh dialog box. You may have to select the CFX Mesh (*gtm *cfx) option under Files of type.

4. Create a new component of type Rotating, named R1.

5. Configure the following setting(s):

   Setting	Value
   Component Type > Value	523.6 [radian s^-1]
   Mesh > File	rotor.grd [ a ]
   Click Browse   to open the Import Mesh dialog box. You may have to select the CFX-TASCflow (*grd) option under Files of type. Ensure that Options > Mesh Units is set to m.

   ---

   Note:  The components must be ordered as above (stator then rotor) in order for the interface to be created correctly. The order of the two components can be changed by right-clicking on S1 and selecting Move Component Up.

   ---

   When a component is defined, Turbo Mode will automatically select a list of regions that correspond to certain boundary types. This information should be reviewed in the Region Information section to ensure that all is correct. This information will be used to help set up boundary conditions and interfaces. The upper case turbo regions that are selected (for example, HUB) correspond to the region names in the CFX-TASCflow grd file. CFX-TASCflow turbomachinery meshes use these names consistently.

6. Click Passages and Alignment > Edit.

7. Configure the following setting(s):

   Setting	Value
   Passage and Alignment > Passages/Mesh > Passages per Mesh	2
   Passage and Alignment > Passages to Model	2
   Passage and Alignment > Passages in 360	113

8. Click Passages and Alignment > Done.

9. Configure the following setting(s):

   Setting	Value
   Wall Configuration	(Selected)
   Wall Configuration > Tip Clearance at Shroud	Yes [ a ]
   Wall Configuration > Tip Clearance at Hub	No [ a ]
   These settings configure the slip conditions on the walls such that the shroud is counter-rotating with respect to the rotor, but the hub is not.

10. Click Next.

1. In the Physics Definition panel, configure the following setting(s):

   Setting	Value
   Fluid	Air Ideal Gas
   Model Data > Reference Pressure	0.25 [atm]
   Model Data > Heat Transfer	Total Energy
   Model Data > Turbulence	k-Epsilon
   Inflow/Outflow Boundary Templates > P-Total Inlet Mass Flow Outlet	(Selected)
   Inflow/Outflow Boundary Templates > Inflow > P-Total	0 [atm]
   Inflow/Outflow Boundary Templates > Inflow > T-Total	340 [K]
   Inflow/Outflow Boundary Templates > Inflow > Flow Direction	Normal to Boundary
   Inflow/Outflow Boundary Templates > Outflow > Mass Flow	Per Component
   Inflow/Outflow Boundary Templates > Outflow > Mass Flow Rate	0.06 [kg s^-1]
   Interface > Default Type	Frozen Rotor
   Solver Parameters	(Selected)
   Solver Parameters > Advection Scheme	High Resolution
   Solver Parameters > Convergence Control	Physical Timescale
   Solver Parameters > Physical Timescale	0.002 [s] [ a ]
   This time scale is approximately equal to 1 / , which is often appropriate for rotating machinery applications.

2. Click Next.

1. Review the various interfaces but do not change them.

2. Click Next.

1. Review the various boundary definitions but do not change them.

2. Click Next.

1. Set Operation to Enter General Mode.

2. Click Finish.

1. Click Define Run  .

2. Configure the following setting(s):

   Setting	Value
   File name	AxialIni.def [ a ]
   You do not need to set the full path unless you are saving the solver file somewhere other than the working directory.

3. Click Save.

   CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.

4. If using stand-alone mode, quit CFX-Pre, saving the simulation (.cfx) file at your discretion.

1. Click Start Run on the Define Run dialog box.

   CFX-Solver runs and attempts to obtain a solution. At the end of the run, a dialog box is displayed stating that the simulation has ended.

2. Select Post-Process Results.

3. If using stand-alone mode, select Shut down CFX-Solver Manager.

4. Click OK.

1. Set Run Mode to a parallel mode suitable for your environment; for example, Intel MPI Local Parallel.

2. If required, click Add Process   to increase the maximum number of processes.

   Ideally, the number of processes should not exceed the number of available processor cores. The number of processes used will be the number of partitions for the mesh.

3. Click Start Run.

4. Select the check box next to Post-Process Results when the completion message appears at the end of the run.

5. If using stand-alone mode, select the check box next to Shut down CFX-Solver Manager.

6. Click OK.

1. Set Run Mode to a parallel mode suitable for your environment; for example, Intel MPI Distributed Parallel.

   One partition should already be assigned to the host that you are logged into.

2. Click Insert Host   to specify a new parallel host.

3. In Select Parallel Hosts, select another host name (this should be a machine that you can log into using the same user name).

4. Click Add, and then Close.

   The names of the two selected machines should be listed in the Host Name column of the Define Run dialog box.

5. Click Start Run.

6. Select the check box next to Post-Process Results when the completion message appears at the end of the run.

7. If using stand-alone mode, select the check box next to Shut down CFX-Solver Manager.

8. Click OK.

1. Follow one of the next two procedures as appropriate:

   Procedure 1: If Simulation Control > Execution Control does not appear in the outline tree view:

   1. Click Define Run  .

   2. Configure the following setting(s):

      Setting	Value
      File name	AxialIni_Cor.def

   3. Click Save.

   CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.

   Procedure 2: If Simulation Control > Execution Control appears in the outline tree view:

   1. Click Execution Control  .

   2. Configure the following setting(s):

      Tab	Setting	Value
      Run Definition	Input File Settings > Solver Input File	AxialIni_Cor.def

   3. Click OK.

   4. Click Define Run  .

   CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.

2. If using stand-alone mode, quit CFX-Pre, saving the simulation (.cfx) file at your discretion.

1. Ensure that the Define Run dialog box is displayed.

2. Select Run Mode > Intel MPI Local Parallel and click Start Run.

3. In CFX-Solver Manager, select Workspace > New Monitor in the main menu and click OK to accept the default name.

4. Configure the following setting(s):

   Tab	Setting	Value
   Plot Lines	Flow > Boundary > R1 Outlet > P-Mass Boundary Flow on R1 Outlet (R1)	(Selected)

5. Click OK.

6. When the dialog box is displayed stating that the simulation has ended, click OK.

   ---

   Note:  The resulting plot of the P-Mass Boundary Flow on R1 Outlet (R1) vs. Accumulated Time Step converges to –0.06 on the Y axis. The exit corrected mass flow rate entered (0.3745 kg s^-1) for this run yields the same physical mass flow as used in the previous steady-state setup; this is expected. The value is negative because the flow is leaving the domain.

   ---

1. Select Tools > Turbo Mode.

   Basic Settings is displayed.

2. Configure the following setting(s):

   Setting	Value
   Analysis Type > Type	Transient
   Analysis Type > Total Time	2.124e-4 [s]
   Analysis Type > Time Steps	2.124e-5 [s] [ a ]
   This time step size will be used until the total time is reached, giving 10 time steps, each 2.124e-5 s.

3. Click Next.

   Component Definition is displayed.

4. Click Next.

   Physics Definition is displayed.

5. Configure the following setting(s):

   Setting	Value
   Fluid	Air Ideal Gas
   Interface > Default Type	Transient Rotor Stator

   ---

   Note:  A Transient Rotor-Stator calculation often runs long enough for the blades to pass through more than one pitch. In these cases, it may be useful to look at variable data averaged over the time interval required to complete 1 pitch. You can then compare data for each pitch rotation to see if a "steady state" has been achieved, or if the flow is still developing.

   ---

6. Click Next.

   A warning message is displayed.

7. Click Yes.

   Interface Definition is displayed.

8. Click Next.

   Boundary Definition is displayed.

9. Click Next.

   Final Operations is displayed.

10. Ensure that Operation is set to Enter General Mode.

11. Click Finish.

1. Click Output Control  .

2. Click the Trn Results tab.

3. In the Transient Results tree view, click Add new item  , set Name to Transient Results 1, and click OK.

4. Configure the following setting(s):

   Setting	Value
   Option	Selected Variables
   Output Variables List	Pressure, Velocity, Velocity in Stn Frame [ a ]
   Output Frequency > Option	Time Interval
   Output Frequency > Time Interval	2.124e-5 [s]
   Use the Ctrl key to select more than one variable.

5. Click OK.

1. Click Execution Control  .

2. Configure the following setting(s):

   Tab	Setting	Value
   Run Definition	Input File Settings > Solver Input File	Axial.def [ a ]
   You do not need to set the full path unless you are saving the solver file somewhere other than the working directory.

3. Confirm that the rest of the execution control settings are set appropriately.

4. Click OK.

1. Click Define Run  .

   A warning will appear, due to a lack of initial values.

   Initial values are required, but will be supplied later using a results file.

2. Click Yes.

3. If using stand-alone mode, quit CFX-Pre, saving the simulation (.cfx) file at your discretion.

1. Under the Initial Values tab, select Initial Values Specification.

2. Under Initial Values Specification > Initial Values, select Initial Values 1.

3. Under Initial Values Specification > Initial Values > Initial Values 1 Settings > File Name, click Browse  .

4. Select AxialIni_001.res from your working directory.

5. Click Open.

6. Under Initial Values Specification > Use Mesh From, select Solver Input File.

7. Click Start Run.

   CFX-Solver runs and attempts to obtain a solution. At the end of the run, a dialog box is displayed stating that the simulation has ended.

8. Select Post-Process Results.

9. If using stand-alone mode, select Shut down CFX-Solver Manager.

10. Click OK, then continue this tutorial from Monitoring the Run.

1. Click the Turbo tab.

   The Turbo Initialization dialog box is displayed and asks you whether you want to auto-initialize all components.

   ---

   Note:  If you do not see the Turbo Initialization dialog box, or as an alternative to using that dialog box, you can initialize all components by clicking the Initialize All Components button, which is visible initially by default, or after double-clicking the Initialization object in the Turbo tree view.

   ---

2. Click Yes.

   Both components (domains) are initialized based on the automatically selected turbo regions. When the process is complete, a green turbine icon appears next to each component entry in the list. Also, the viewer displays a green background mesh for each initialized component, visible when a component is selected.

3. Double-click Component 1 (S1) and review the automatically-selected turbo regions and other data in the details view.

4. Double-click Component 2 (R1) and review the automatically-selected turbo regions and other data in the details view (including the Passages per Component setting on the Instancing tab, which should have a value of 2).

1. In the Turbo tree view, double-click Blade-to-Blade.

2. Click Apply.

   A surface of constant span appears, colored by pressure.

1. In the Turbo tree view, double-click Initialization.

2. Click Three Views.

   Left view is 3D View, top right is Blade-to-Blade and bottom right is Meridional view.

3. Click Single View.

1. Select Insert > Location > Turbo Surface, and accept the default name.

2. Set Method to Constant Span and Value to 0.5.

3. Under the Color tab, set Mode to Variable, Variable to Pressure, Range to User Specified, Min to -10000 [Pa], and Max to -7000 [Pa].

4. Click Apply.

1. In the Turbo tree view, double-click the 3D View object.

2. In the Graphical Instancing section of the form, set # of Copies to 6 for R1.

3. Click Apply.

4. In the Graphical Instancing section of the form, set # of Copies to 6 for S1.

5. Click Apply.

6. Return to the Outline tab and ensure that the turbo surface is visible again.

1. Click Timestep Selector  .

2. Select time value 0.

3. Click Apply to load the time step. The rotor blades move to their starting positions. These positions are exactly 1 pitch from the blade positions that were previously displayed, so the blades will appear to be in the same positions.

4. Turn off the visibility of Wireframe.

5. Position the geometry as shown below, ready for the animation. During the animation the rotor blades will move to the right. Make sure you have at least two rotor blades out of view to the left side of the viewer. They will come into view during the animation.

   

6. Click Animation  .

   The Animation dialog box appears.

7. Set Type to Keyframe Animation.

8. Click New   to create KeyFrameNo1.

9. Select KeyframeNo1, then set # of Frames to 9, then press Enter while in the # of Frames box.

   ---

   Tip:  Be sure to press Enter and confirm that the new number appears in the list before continuing.

   ---

10. Use the Timestep Selector to load the final time step.

11. In the Animation dialog box, click New   to create KeyframeNo2.

12. Click More Animation Options   to expand the Animation dialog box.

13. Click Options and set Transient Case to TimeValue Interpolation. Click OK.

    The animation now contains a total of 11 frames (9 intermediate frames plus the two Keyframes), one for each of the available time values.

14. In the expanded Animation dialog box, select Save Movie.

15. Set Format to MPEG1.

16. Click Browse  , next to the Save Movie box and then set the file name to an appropriate file name.

17. If frame 1 is not loaded (shown in the F: text box at the bottom of the Animation dialog box), click To Beginning   to load it.

    Wait for CFD-Post to finish loading the objects for this frame before proceeding.

18. Click Play the animation  .

    • It takes a while for the animation to be completed.

    • To view the movie file, you will need to use a media player that supports the MPEG format.

    You will be able to see from the animation, and from the plots created previously, that the flow is not continuous across the interface. This is because a pitch change occurs. The relatively coarse mesh and the small number of time steps used in the transient simulation also contribute to this. The movie was created with a narrow pressure range compared to the global range, which exaggerates the differences across the interface.

1. Click File > Report > Report Templates.

2. In the Report Templates dialog box, select Turbine Report, then click Load.

   The report will be generated automatically.

3. Click the Report Viewer tab (located below the viewer window).

   A report appears.

1. Select Insert > Location > Turbo Surface.

2. Set the Name to R1 MidSpan and click OK.

3. Under the Geometry tab, set Domains to R1.

4. Ensure that Method is set to Constant Span and Value is set to 0.5 to create a surface at the mid-span of the rotor.

5. Click Apply.

1. Select Insert > Location > Turbo Surface.

2. Set the Name to S1 MidSpan and click OK.

3. Under the Geometry tab, set Domains to S1.

4. Ensure that Method is set to Constant Span and Value is set to 0.5 to create a surface at the mid-span of the rotor.

5. Click Apply.

1. Click File > Export > Export.

   The Export dialog box appears.

2. Set File to R1 MidSpan.csv.

3. Set Type to Geometry Only.

4. Set Locations to R1 MidSpan.

5. Click Save.

6. Repeat steps 1-5 for the stator surface naming the file S1 MidSpan.csv.

1. Select Insert > User Locations > User Surface.

   The Insert User Surface dialog box appears.

2. Set the Name to R1 MidSpan.

3. Click Browse  .

4. Select R1 MidSpan.csv from your working directory.

5. Click Open.

6. Select Visibility so you can see the surface in the graphics viewer.

7. Click OK.

8. Repeat steps 1-7, naming the user surface "S1 MidSpan" and selecting S1 MidSpan.csv from your working directory.

   You can now see the two surfaces you created in CFD-Post in the CFX-Pre viewer.

1. Select Insert > Coordinate Frame and accept the default name.

2. Configure the following setting(s):

   Setting	Value
   Option	Axis points
   Frame Motion	(selected)
   Frame Motion > Option	Rotating
   Frame Motion > Angular Velocity	523.6 [radian s^-1]

3. Click OK.

1. Click Output Control  .

2. Click the Monitor tab.

3. In the Monitor Surfaces group box, click Add new item  , set Name to S1 MonitorSurface, and click OK.

4. Configure the following setting(s):

   Setting	Value
   Output Variables List	Pressure, Velocity
   Output Location List	S1 MidSpan
   Output Frequency > Option	Every Timestep

5. Click Apply.

1. In the Monitor Surfaces group box, click Add new item  , set Name to R1 MonitorSurface, and click OK.

2. Configure the following setting(s):

   Setting	Value
   Coordinate Frame	Coord 1 [ a ]
   Output Variables List	Pressure, Velocity
   Output Location List	R1 MidSpan
   Output Frequency > Option	Every Timestep
   By specifying the rotating coordinate frame, the monitor surface will rotate at the same speed as the blades, allowing for simpler post-processing.

3. Click OK.

1. Click Output Control  .

2. Click the Results tab.

3. Set Option to None.

4. Click OK.

1. Right-click Analysis Type in the Outline tree view and select Edit.

2. Set Time Steps > Timesteps to 2.124e-6 [s].

   Reducing the timestep size by a factor of 10 will make the simulation run for 100 timesteps. This allows more time to view the Monitor Surface in CFD-Post.

3. Click OK.

1. Right-click Execution Control in the Outline tree view and select Edit.

2. Set Input File Settings > Solver Input File to AxialMonitoring.def.

   This ensures that you do not overwrite any previously created .def file.

3. Click OK.

1. Click Define Run  .

   A warning will appear, due to a lack of initial values.

   Initial values are required, but will be supplied later using a results file.

2. Click Yes.

3. If using stand-alone mode, quit CFX-Pre, saving the simulation (.cfx) file at your discretion.

1. Ensure that Solver Input File is set to AxialMonitoring.def.

2. Under the Initial Values tab, select Initial Values Specification.

3. Under Initial Values Specification > Initial Values, select Initial Values 1.

4. Under Initial Values Specification > Initial Values > Initial Values 1 Settings > File Name, click Browse  .

5. Select AxialIni_001.res from your working directory.

6. Click Open.

7. Under Initial Values Specification > Use Mesh From, select Solver Input File.

8. Click Start Run.

   CFX-Solver runs and attempts to obtain a solution.

9. After the run has started, select Tools > Monitor Run with CFD-Post.

   CFD-Post opens and loads the solution data.

1. Select Insert > Text and accept the default name.

2. Select Embed Auto Annotation.

3. Set Type to Timestep.

4. Click Apply.

The Monitor Surface you defined in CFX-Pre has been pre-loaded into CFD-Post. You can view it in the Outline tab under Other Locations.

Select Other Locations > R1 MonitorSurface to unhide it.

1. Double-click R1 MonitorSurface.

2. Under the Color tab set the Mode to Variable.

3. Set the Variable to Pressure.

4. Set the Range to Local.

5. Click Apply.

1. Select Monitor > Start Auto Update.

   The contour now shows data and will regularly update to the data associated with the latest timestep generated by the solver. Notice how the rotor and Monitor Surface rotate together.

   Object creation is prohibited in CFD-Post during Auto Update. You can look in CFX-Solver Manager to see if a timestep is almost complete.

2. Select Monitor > Stop Auto Update.

   This stops the Auto Update and you can once again create and edit objects.

1. Select Insert > Vector and accept the default name.

2. Under the Geometry tab, set the Locations to S1 MonitorSurface.

3. Under the Color tab , set the Range to Local.

4. Click Apply.

1. Wait until another timestep has completed and then select Monitor > Update Once.

   This will load the most recently written solution data (most recent timestep in this case).

2. Select Monitor > Start Auto Update again.

   You can watch the solution progress up until the run is finished.

3. In CFX-Solver Manager, you can stop the run by selecting Workspace > Stop Current Run at any time.