In the * Workbench* window, this is what you should see currently in the

Double click on * Setup,* which will bring up the

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 * Setup*. We will work from top to bottom of the

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

**Setup > General > Mesh > Display...**

The long, skinny rectangle displayed in the graphics window corresponds to our solution domain. Some of the operations available in the graphics window to interrogate the geometry and mesh are:

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

Zoom Out: Hold down the * Middle Mouse Button* and drag a box anywhere from the

Use these operations to zoom in and interrogate the 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 that surface entity corresponds to (you will need to zoom in/out and translate the model as you do this). For instance, the surface labeled

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

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) values of velocity, pressure, and temperature. It will add the *k* and *epsilon* equations to the set of governing equations to calculate the effect of the turbulent fluctuations on the mean, as discussed in the Pre-Analysis step.

**Models > Viscous - Laminar > Edit...**

Under ** Model**, select

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.

**Materials > Fluid air > Create/Edit...**

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 Pre-Analysis step. This is called the "incompressible ideal gas" model in Fluent (it's non-standard nomenclature). Change the * Density (kg/m3)* from

The other properties are also functions of temperature. However, we'll use constant values equal to the average values over the temperature range obtained in the experiment. Enter the following constant values:

**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 **

Click ** Change/Create** and

Fluent uses gauge pressure internally to minimize round-off errors stemming from small differences of big numbers. Anytime an absolute pressure is needed, it is generated by adding the so-called "operating pressure" to the gauge pressure:

absolute pressure = gauge pressure + "operating pressure"

This "operating pressure" is also used in the "incompressible ideal gas" model as mentioned above. We will specify the "operating pressure" as equal to the measured ambient pressure since the absolute pressure in the pipe varies only slightly from this (you do get significant variations in gauge pressures though).

**(double-click) Boundary Conditions > Operating Conditions...**

Enter **98338.2** under ** Operating Pressure** and click

Next, we will specify the boundary condition for the centerline.

**Boundary Conditions > axis**

Change the ** Type** to axis and click

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.

**Boundary Conditions > heated_section > Edit...**

A new Wall window will open. Click on the * Thermal* tab and enter 5210.85 next to

As discussed in the Pre-Analysis step, we need to set:

- Velocity and temperature (plus k and epsilon for the turbulence model equations) at the inlet
- Pressure at the outlet

For subsonic flow, the flow adjusts to the pressure at the outlet (consider this as a signal you are sending the flow about what it needs to do inside the pipe).

Select:

**Boundary Conditions > inlet**

Note that the boundary ** Type** is automatically set to

Click ** Edit...** to set up the correct inlet parameters. The

Use the default values for * Turbulent Intensity *(5%) and

Now click on the * Thermal* tab and enter

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

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.