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.
Problem Setup > General > Solver
Choose Axisymmetric under 2D Space. As in the laminar pipe flow tutorial, we'll use the defaults of Pressure-Based Type, Steady Flow and Absolute Velocity Formulation.
Problem Setup > Models > Energy...
The energy equation can be turned off since this is an incompressible flow and we are not interested in the temperature. Make sure Energy - Off appears.
Problem Setup > Models > Viscous - Laminar
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
Double click on air and change Density to
1.0 kg/m^3 and Viscosity to
2e-5 kg/(m*s). These are the values in the Problem Specification and are picked to give us a Reynolds number of 10,000. We'll take both as constant.
Click Change/Create and close the window.
Problem Setup > Boundary conditions > Operating Conditions...
Recall that for all flows, Fluent uses the gauge pressure internally. Any time an absolute pressure is needed, it is generated by adding the operating pressure to the gauge pressure. We'll use the default value of 1 atm (101,325 Pa) as the Operating Pressure.
Click Cancel to leave the default in place.
We'll now set up the boundary conditions at the wall, centerline, inlet and outlet.
Problem Setup > Boundary conditions
We don't need to set any parameters for the pipewall zone. Fluent will automatically detect that this location should be set as a wall based on its name. Verify this by selecting that zone and looking at its type in the drop-down menu.
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 correct in our case. Change the Velocity Specification Method to Magnitude, Normal to Boundary. Enter
1 m/s for 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.
Note: Backflow in the Pressure Outlet menu refers to flow entering through an outlet boundary. This is not likely to happen in this case. So, we don't have to set the backflow parameters.
This completes the boundary condition specification.
Let's set up the reference values, which will be used later while viewing non-dimensional results (this setting doesn't affect the numerical solution).
Problem Setup > Reference Values
Select Compute from > inlet.