Let's get Fluent to solve our nonlinear BVP. It will introduce discretization and linearization errors in the process, as discussed in the Pre-Analysis step. We'll check the level of numerical errors later in the Verification & Validation step. There are lots of knobs in the *Solution* menu that you can twiddle to improve your numerical solution to the BVP. We'll not mess with most of these since the default settings yield an adequate numerical solution for our problem. We could get a slight improvement in accuracy by fiddling various knobs which we'll refrain from doing here.

**Solution > Methods**

The Fluent solver converts our BVP to a set of algebraic equations through a process called discretization. We'll use second-order discretization for which the error is of the order of the *square* of the mesh spacing. This is more accurate (albeit less stable) than first-order discretization, where the error is of the order of the mesh spacing. Choose *Second-Order Upwind* for all equations as shown below. Set *Pressure-Velocity Coupling *to *SIMPLE* if it is not by default.

To set the convergence criterion identified in the flowchart above, select:

**Solution > Monitors > Residual**

We see that we need to provide a convergence criterion for each PDE that is being solved. The solver will stop iterating when mass, momentum, energy, k, and epsilon imbalances (called residuals) fall below the convergence tolerance. We'll use a residual tolerance of 10^{-6} for all six PDE's being solved. Fluent will consider the iterations to have converged when all six residuals have fallen below this tolerance. Set the residuals tolerance as shown in the figure below. Make sure to scroll down and set the tolerance for *k* and *epsilon* equations also.

Also, make sure the ** Plot** box is checked as shown above. This will help you monitor how/whether the solution is proceeding to convergence as the iterations are carried out. Click

Next, we set the initial guess indicated in the flowchart. The initial guess can be entered using:

**Solution > Initialization**

We need to provide Fluent with an initial guess for the flow variables (velocity, pressure, etc.) to start the iterations. For this example, we know the conditions at the inlet of the pipe (except for pressure, which is set to zero gauge by default). Initialize the entire flowfield to the specified values at the inlet: First, select ** Standard Initialization**, then under

To prevent the computer from iterating indefinitely, we need to set an iterations limit.

**Solution > Run Calculation **

Enter 500 for ** Number of Iterations** and click

Save project and exit Fluent:

**File > Save Project **

**File > Close Fluent**