Physics Setup

In the Workbench window, this is what you should see currently in the Project Schematic space.

Double click on Setup which will bring up the FLUENT Launcher. Click OK to select the default options in the FLUENT Launcher. Twiddle your thumbs a bit while the FLUENT interface comes up. This is where we'll specify the governing equations and boundary conditions for our boundary-value problem. On the left-hand side of the FLUENT interface, we see various items listed under Problem Setup. We will work from top to bottom of the Problem Setup items to setup the physics of our boundary-value problem. On the right hand side, we have the Graphics pane and, below that, the Command pane.

Display Mesh

 Let's first display the mesh that was created in the previous step. 

...

Translation: The model can be translated in any direction by holding down the Left Mouse Button and then moving the mouse in the desired direction.

Zoom In: Hold down the Middle Mouse Button and drag a box from the Upper Left Hand Corner to the Lower Right Hand Corner over the area you want to zoom in on.

Zoom Out: Hold down the Middle Mouse Button and drag a box anywhere from the Lower Right Hand Corner to the Upper Left Hand Corner.

Use these operations to zoom in and interrogate our mesh.

You should have all the surfaces shown in the above snapshot.  Clicking on a surface name in the Mesh Display menu will toggle between select and unselect. Clicking Display will show all the currently selected surface entities in the graphics pane. Unselect all surfaces and then select each one in turn to see which part of the domain or boundary the particular surface entity corresponds to (you will need to zoom in/out and translate the model as you do this). For instance, the surface labeled heated_section should correspond to the part of the wall where heating occurs.

...

We ask FLUENT to solve the axisymmetric form of the governing equations.
General > Solver > 2D Space > Axisymmetric

 
The energy equation is turned off by default. Turn on the energy equation.
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 powerpoint presentation.

Models > Viscous - Laminar > Edit...

Under Model, select k-epsilon (2 eqn). Since we'll use the default settings for the k-epsilon turbulence model, click OK.

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.

...

Since variations in absolute pressure are small in our pipe, we'll use a constant absolute pressure in the ideal gas law as discussed in the powerpoint presentation. This is called the "Incompressible ideal gas" model in FLUENT (it's non-standard nomenclature).  Change the Density (kg/m3) from constant to incompressible-ideal-gas. The constant absolute pressure to be used in the ideal gas equation is specified later as Operating Pressure.

...

https://confluence.cornell.edu/download/attachments/111221574/material%20properties.png

Click Change/Create and Close the Create/Edit Materials window.

...

Boundary Conditions > Operating Conditions...

Enter 98338.2 under Operating Pressure and click OK.

Next we will specify the boundary condition for the centerline.

Boundary Conditions > axis

Change the Type to axis and click OK. FLUENT will set the flow gradients at this boundary in accordance with the axisymmetric assumption.

...

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

...

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.

Click Edit... to set up the correct inlet parameters. The Velocity Inlet window pops up. Enter 30.06 next to Velocity Magnitude (m/s). Under Turbulence, select the specification method to be K and Epsilon. For Turbulent Kinetic Energy (m2/s2), enter value 0.09. For Turbulent Dissipation Rate (m2/s3), enter value 16. Note that k and epsilon are not measured and are rough guess values. 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). 

...

https://confluence.cornell.edu/download/attachments/111221574/velocity%20inlet_sm.png

 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. 

Click Edit... to specify the gauge pressure at the outlet. 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)

...