Step 6: Boundary Conditions

Boundary Conditions

1.   Change wall-2 type to interior.

Boundary Conditions wall-2

  The zones wall-2 and wall-3 are the interfaces between the three fluid zones. They need to be changed to type interior, as discussed earlier. The resulting interior faces are those that have fluid cells on both sides but do not require any boundary conditions to be set.

(a)   Select interior from the Type drop-down list.

  A Question dialog box will open, asking if you want to change the type from wall to interior.

i.   Click Yes to open the interior dialog box.

   ANSYS FLUENT will fuse wall-2 and wall-2-shadow together to form interior-2.

ii.   Click OK to retain the default Zone Name.

(b)   Similarly, change wall-3 to an interior zone named interior-3.

2.   Identify the rotating fluid zone (i.e., the zone containing the blades) by displaying the mesh for each zone.

Boundary Conditions Display Mesh...

  It is unclear when you read the mesh which fluid zone corresponds to which interior zone. While the interior zones can be selected individually in the Mesh Display dialog box, the fluid zones cannot. Commands in the text interface, however, can be used to make this association.

(a)   Deselect all the surfaces by clicking the button to the right of the Surfaces selection list.

(b)   Click the Outline button to select only the outline surfaces of the domain.

(c)   Click Display.

  Only the domain boundaries and interior walls will be displayed.

(d)   Type the commands, in the console, as shown.

Hint:   You may need to press the <Enter> key to get the $>$ prompt.

> display

/display> zone-mesh

()
zone id/name(1) [()] 13

zone id/name(2) [()] <Enter>

  The resulting display (Figure  10.3) shows that zone fluid-13 corresponds to the rotating region.

(e)   Close the Mesh Display dialog box.

Figure 10.3: Mesh in fluid-13

3.   Set the boundary conditions (see Figure  10.1) for the flow inlet ( pressure-inlet-5).

Boundary Conditions pressure-inlet-5 Edit...

(a)   Enter 200 Pa for Gauge Total Pressure.

(b)   Select Intensity and Hydraulic Diameter from the Specification Method drop-down list.

(c)   Enter 5 % for Turbulent Intensity.

(d)   Enter 0.05 m for Hydraulic Diameter.

(e)   Click OK to close the Pressure Inlet dialog box.

Note:   All pressures that you specify in ANSYS FLUENT are gauge pressures, relative to the operating pressure specified in the Operating Conditions dialog box. By default, the operating pressure is 101325 Pa.

For details, see this section in the separate User's Guide.

4.   Set the backflow turbulence parameters for the flow outlet ( pressure-outlet-9) to the same values used for pressure-inlet-5.

Note:   The backflow values are used only if reversed flow occurs at the outlet, but it is a good idea to use reasonable values, even if you do not expect any backflow to occur.

5.   Define the velocity of the wall zone representing the blades ( wall-7) relative to the moving fluid zone.

Boundary Conditions wall-7 Edit...

  With fluid-13 set to a rotating reference frame, wall-7 becomes a moving wall.

(a)   Select Moving Wall in the Wall Motion list.

  The Wall dialog box will expand to show the wall motion parameters.

(b)   Retain the default selection of Relative to Adjacent Cell Zone and select Rotational in the Motion group box.

(c)   Retain the default value of 0 rad/s for (relative) Speed.

(d)   Click OK to close the Wall dialog box.

  The Rotation-Axis Origin should be located at $x$ = 0 m and $y$ = 0 m. With these settings, the blades will move at the same speed as the surrounding fluid.