Step 6: Boundary Conditions

Boundary Conditions

1.   Set the following conditions at the flow inlet ( velocity-inlet-2).

Boundary Conditions velocity-inlet-2 Edit...

(a)   Select Components from the Velocity Specification Method drop-down list.

(b)   Enter 1.146 m/s for Axial-Velocity.

(c)   Select Intensity and Hydraulic Diameter from the Specification Method drop-down list in the Turbulence group box.

(d)   Enter 2.6% for Turbulent Intensity.

(e)   Enter 8.86 cm for Hydraulic Diameter.

(f)   Click OK to close the Velocity Inlet dialog box.

2.   Set the following conditions at the flow outlet ( pressure-outlet-3).

Boundary Conditions pressure-outlet-3 Edit...

(a)   Retain the default selection of Normal to Boundary from the Backflow Direction Specification Method drop-down list.

(b)   Select Intensity and Viscosity Ratio from the Specification Method drop-down list in the Turbulence group box.

(c)   Enter 5% for Backflow Turbulent Intensity.

(d)   Retain the default value of 10 for Backflow Turbulent Viscosity Ratio.

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

Note:    ANSYS FLUENT will use the backflow conditions only if the fluid is flowing into the computational domain through the outlet. Since backflow might occur at some point during the solution procedure, you should set reasonable backflow conditions to prevent convergence from being adversely affected.

3.   Accept the default settings for the disk walls ( wall-6).

Boundary Conditions wall-6 Edit...

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

Note:   For a rotating reference frame, ANSYS FLUENT assumes by default that all walls rotate at the speed of the moving reference frame, and hence are moving with respect to the stationary (absolute) reference frame. To specify a non-rotating wall, you must specify a rotational speed of 0 in the absolute frame.