Numerical Solution

FLUENT incorporates advanced algorithms for numerically solving our nonlinear BVP. 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.

Let's now investigate how we can achieve a numerical solution in FLUENT. One must keep in mind that the governing equations we are attempting to find an approximate solution to are nonlinear. This means that in order for a CFD program, such as FLUENT to solve it, it must go through an iterative process. This process is briefly described in the flow-chart below.

 
From the flow chart, we see that we need to provide FLUENT with an initial guess for the flow variables (velocity, pressure etc.) to start the iterations. We'll also specify the convergence criterion to let the beast know when to consider the iterative process to have converged to a solution.

Solution > 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.

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

Solution > Monitors > Residuals - Print, Plot > Edit...

We see that we need to provide a convergence criterion for each PDE that is being solved. We'll use a residual tolerance of 10^-6 for all six PDE's being solved. FLUENT will consider the iterations 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 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 OK.

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

Solution > Solution Initialization

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 Compute from, select Inlet and click Initialize.

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 Calculate. You will see a window message saying Calculating the solution... Wait for FLUENT to finish the calculation. Our solution converges in about 350 - 400  iterations. You should see a residual plot on screen as the computation is being performed. It should look something like this:

Save project and exit FLUENT:

File > Save Project 

File > Close Fluent

Go to Step 6: Numerical Results

Go to all FLUENT Learning Modules