Sign-up for free online course on ANSYS simulations!...
We ask FLUENT to solve the axisymmetric form of the governing equations. When you do this, the solver switches to cylindrical polar coordinates. So from here on, you should interpret the horizontal coordinate as axial and the vertical coordinate as radial.
General > Solver > 2D Space > Axisymmetric
The energy equation is turned off by default. Turn on the energy equation. Note that in most cases, you'll have to double-click on an item to select it.
Models > Energy - Off > Edit...
Turn on the Energy Equation and click OK.
By default, FLUENT will assume the flow is laminar. Let's tell it that our flow is turbulent rather than laminar and that we want to use the k-epsilon turbulence model to simulate our turbulent flow. This means FLUENT will solve for mean (i.e. Reynolds-averaged) quantities at every point in the domain. It will add the k and epsilon equations to the governing equations to calculate the effect of the turbulent fluctuations on the mean, as discussed in the Pre-Analysis step.
...
This is what you should currently see under Models.
Now let's set the "material properties" i.e. properties of air that appear in our boundary value problem.
...
Cp (Specific Heat) (j/kg-k): 1005
Thermal Conductivity (w/m-k): 0.0266
Viscosity (kg/m-s): 1.787e-5
Molecular Weight (kg/kgmol): 28.97
...
https://confluence.cornell.edu/download/attachments/111221574/material%20properties.png
Click Change/Create and Close the Create/Edit Materials window.
...
Enter 98338.2 under Operating Pressure and click OK.
Next we will specify the boundary condition for the centerline.
...
Change the Type to axis and click OK. FLUENT will set the flow gradients at this boundary in accordance with the axisymmetric assumption.
Now let's specify the boundary condition at the walls. By default, FLUENT correctly picks the Wall boundary type for these boundaries. It will impose the no-slip condition for velocity at these boundaries. Additionally, for the heated wall section, we need to specify the heat flux into the flow.
...
A new Wall window will open. Click on Thermal tab and enter 5210.85 next to Heat Flux (w/m2) and click OK.
...
https://confluence.cornell.edu/download/attachments/111221574/heated%20wall.png
As discussed in the Pre-Analysis step, we need to set:
...
Select:
Boundary Conditions > inlet
Note that the boundary Type is automatically set to velocity-inlet. FLUENT has an automatic mechanism to pick a boundary type according to the name you give and settings that you have selected previously (this could be dangerous if FLUENT selects the wrong boundary type and a lackadaisical user doesn't change it.). In this case, it gets it right.
...
Use the default values for Turbulent Intensity (5%) and Turbulent Viscosity Ratio (10). These are plausible guess values for the turbulence level at the inlet. FLUENT will calculate k and epsilon at the inlet from these values and use them as boundary conditions for the k and epsilon equations. The results should not be sensitive to these inputs since most of the turbulence is generated in the boundary layers (ideally, you should check the sensitivity of your calculation to this setting).
Now click on Thermal tab and enter 298.15K for Temperature. Click OK to close the window.
Finally, set up the outlet boundary condition:
Boundary Conditions > Outlet
FLUENT selects the pressure-outlet boundary type and its guess turns out to be right.
...
Enter -1112.3 for Gauge Pressure and click Ok. (From experiment, measured outlet pressure is 97225.9 Pa. Corresponding gauge pressure = 97225.9 Pa - operating pressure = -1112.3 Pa)
...
https://confluence.cornell.edu/download/attachments/111221574/outlet%20pressure.png 
Now FLUENT knows all necessary elements of our beloved BVP (domain, governing equations and boundary conditions). In the Solution step, we'll prod the beast to obtain an approximate numerical solution to our BVP.
...