### 2.8.2. Setting up the Turbomachinery Simulation

You will use CFX-Pre in Turbo mode to set up physics and boundary conditions. In this case, you will specify the same rotational rate and mass flow as specified in Vista CPD.

1. Double-click the Setup cell in the CFX system to open CFX-Pre.

2. Select Tools > Turbo Mode.

   The Basic Settings panel is displayed.

3. Accept the default settings in the Basic Settings panel by clicking Next.

4. In the Component Definition panel, select R1.

5. Set Component Type > Value to `1450 [rev min^-1]`.

6. Click Next.

7. In the Physics Definition panel, configure the following options:

   Setting | Value
   --- | ---
   Fluid | Water
   Model Data > Turbulence | Shear Stress Transport
   Inflow/Outflow Boundary Templates | P-Total Inlet Mass Flow Outlet
   Inflow > P-Total | 0 [atm]
   Inflow > Flow Direction | Cylindrical Components
   Outflow > Mass Flow | Per Machine
   Outflow > Mass Flow Rate | 77.8 [kg s^-1]

8. Click Next.

9. In the Interface Definition panel, note that periodic interfaces have been set up, then click Next.

10. In the Boundary Definition panel, modify the R1 Hub boundary:

    1. Select R1 Hub

    2. Click the Multi-select from extended list icon.

       This opens the Selection Dialog dialog box.

    3. In the Selection Dialog dialog box, hold the Ctrl key and click each of `HUB DOWNSTREAM` and `OUTBlock HUB` to remove them from the selection, so that only `Passage HUB` and `INBlock HUB` are selected.

    4. Click OK in the Selection Dialog dialog box.

11. Add a new boundary:

    1. Right-click Boundaries in the tree view and select Add Boundary....

    2. Set the boundary name to `R1 Hub Outlet` and click OK.

    3. Select the R1 Hub Outlet boundary and configure the following settings:

       Setting | Value
       --- | ---
       R1 Hub Outlet > Boundary Type | Wall
       R1 Hub Outlet > Location | HUB DOWNSTREAM,OUTBlock HUB [a]
       Wall Influence On Flow > Option | Counter Rotating Wall
       [a] Use the Multi-select from extended list icon to select multiple locations.

12. Modify the R1 Shroud boundary by setting Wall Influence On Flow > Option to `Counter Rotating Wall`.

13. Click Next.

    Final Operations is displayed.

14. Ensure that Operation is set to `Enter General Mode`.

15. Click Finish.

16. In the Outline tree view, edit `R1 Outlet`.

17. In the details view, configure the following settings:

    Tab | Setting | Value
    --- | --- | ---
    Boundary Details | Mass And Momentum > Mass Flow Outlet Constraint | (Selected)
    Mass And Momentum > Mass Flow Outlet Constraint > Option | Pressure Shape Constrained
    Mass And Momentum > Mass Flow Outlet Constraint > Pres. Profile Shape | 0.0 [Pa]
    Mass And Momentum > Mass Flow Outlet Constraint > Pres. Profile Blend | 0.95

18. Click OK.

19. Select File > Close CFX-Pre to return to the Project Schematic view.

20. Double-click the Solution cell in the CFX system to launch CFX-Solver Manager.

21. In the Define Run dialog box, click Start Run to begin the CFD calculation.

    The residual monitors show the progress of the calculation.

22. After the solution has been generated, click OK to dismiss the completion message, then select File > Close CFX-Solver Manager to return to the Project Schematic view.

Release 18.2 - © ANSYS, Inc. All rights reserved.