Panel |
---|

Problem Specification |

Info | ||
---|---|---|

| ||

Click here for the FLUENT 12 version. |

## Step 5: Solution

We'll use second-order discretization for the momentum equation, as in the laminar pipe flow tutorial, and also for the turbulence kinetic energy equation which is part of the *k-epsilon* turbulence model.

**Main Menu > Solve > Controls > Solution...**

Change ** Discretization** for

**,**

*Momentum*

*Turbulence***and**

*Kinetic Energy***equations to**

*Turbulence Dissipation Rate***(if you do not see all of the equations scroll down to see them)**

*Second Order Upwind*newwindow | ||||
---|---|---|---|---|

| ||||

https://confluence.cornell.edu/download/attachments/90737468/03solution_controls_sm.jpg?version=1 |

The order of discretization that we just set refers to the convective terms in the equations; the discretization of the viscous terms is always second-order accurate in FLUENT. Second-order discretization generally yields better accuracy while first-order discretization yields more robust convergence. If the second-order scheme doesn't converge, you can try starting the iterations with the first-order scheme and switching to the second-order scheme after some iterations. |

#### Set Convergence Criteria

Recall that FLUENT reports a residual for each governing equation being solved. The residual is a measure of how well the current solution satisfies the discrete form of each governing equation. We'll iterate the solution until the residual for each equation falls below 1e-6.

**Main Menu > Solve > Monitors > Residual...**

Notice that ** Convergence Criterion** has to be set for the

*k*and

*epsilon*equations in addition to the three equations in the last tutorial. Set the

**to be 1e-06 for all five equations being solved.**

*Convergence Criterion*Select ** Print** and

**under**

*Plot***. This will print as well plot the residuals as they are calculated which you will use to monitor convergence.**

*Options*Click ** OK**.

#### Set Initial Guess

We'll use an initial guess that is constant over the entire flow domain and equal to the values at the inlet:

**Main Menu > Solve > Initialize > Initialize...**

In the *Solution Initialization* menu that comes up, choose ** inlet** under

**. The**

*Compute From***for**

*Axial Velocity**all*cells will be set to 1 m/s, the

**to 0 m/s and the**

*Radial Velocity***to 0 Pa. The**

*Gauge Pressure***and**

*Turbulence Kinetic Energy***(scroll down to see it) values are set from the prescribed values for the**

*Dissipation Rate**Turbulence Intensity*and

*Hydraulic Diameter*at the inlet.

newwindow | ||||
---|---|---|---|---|

| ||||

https://confluence.cornell.edu/download/attachments/90737468/03solution_init.jpg?version=1 |

Click ** Init**. Close the

*Solution Initialization*window.

This completes the problem specification. Save your work:

**Main Menu > File > Write > Case...**

Type in `pipe100x30.cas for`

** Case File**. Click

**. Check that the file has been created in your working directory.**

*OK*#### Iterate Until Convergence

Solve for 100 iterations first.

**Main Menu > Solve > Iterate...**

In the *Iterate* menu that comes up, change the ** Number of Iterations** to

`100`

. Click **.**

*Iterate*You'll find that not all residuals have fallen below 1e-6 in 100 iterations. Solve for 200 more iterations. The solution converges in a total of 229 iterations.

newwindow | ||||
---|---|---|---|---|

| ||||

https://confluence.cornell.edu/download/attachments/90737468/03graph_windowfull.jpg?version=1 |

We need a larger number of iterations for convergence than in the laminar case since we have a finer mesh and are also solving additional equations from the turbulence model.

Save the solution to a data file:

**Main Menu > File > Write > Data...**

Enter `pipe100x30.dat`

for ** Data File** and click

**. Check that the file has been created in your working directory.**

*OK*Go to Step 6: Results