Click here for the FLUENT 6.3.26 version.
We will be working within ANSYS Workbench. To launch FLUENT, double click on the Setup cell from the Project view. Make sure the Double Precision option is selected. This will use 64 bits (rather than 32) per floating point number, decreasing round-off errors.
Once Fluent has opened, select Problem Setup > General > Display...
Make sure all 5 items under Surfaces are selected. Then click Display. Remember that we can zoom in using the middle mouse button. Zoom in and admire the mesh. How many divisions are there in the radial direction?
Recall that you can look at specific components of the mesh by choosing the entities you wish to view under Surfaces (click to select and click again to deselect a specific boundary). Click Display again when you have selected your boundaries. Use this feature and make sure that the boundary labels correspond to the correct geometric entities.
Click Edit... and choose k-epsilon (2eqn). Notice that the window expands and additional options are displayed on choosing the k-epsilon turbulence model. Under Near-Wall Treatment, pick Enhanced Wall Treatment. This option uses a blended function to go between a two-layer model and standard wall functions. If the mesh near the wall is fine enough, the two-layer model is used. Otherwise, standard wall functions are used. You could alternately use Standard Wall Functions; this will work well when 30 < y+ < 100. Refer to the turbulence chapter in the FLUENT user manual.
Problem Setup > Materials
Next, let's look at the centerline. Since we are solving an axisymmetric problem, we will set the centerline as the axis; this will impose symmetry at this boundary. Set centerline to axis boundary type, using the drop down menu. Click Yes and OK to confirm.
Choose inlet and click on Edit..... This boundary is set to velocity-inlet type by default which is right in our case. Change the Velocity Specification Method to Magnitude, Normal to Boundary. Enter
1 m/sfor Velocity Magnitude. This indicates that the fluid is coming in normal to the inlet at the rate of 1 meter per second. Select Intensity and Hydraulic Diameter next to the Turbulence Specification Method. Then enter
1% for Turbulence Intensity and
0.2m for Hydraulic Diameter. Click OK to set the boundary conditions for the inlet.
The (absolute) pressure at the outlet is 1 atm. Since the operating pressure is set to 1 atm, the outlet gauge pressure = outlet absolute pressure - operating pressure = 0. Choose outlet under Zone. The Type of this boundary is pressure-outlet. Click on Edit. The default value of the Gauge Pressure is 0. Click Cancel to leave the defaults in place.
Let's setup the reference values, which will be used later on while while viewing non-dimensional results (this setting doesn't affect the numerical solution).