Sign-up for free online course on ANSYS simulations!| 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 Kinetic Energy and Turbulence Dissipation Rate equations to Second Order Upwind (if you do not see all of the equations scroll down to see them)
| 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 Convergence Criterion to be 1e-06 for all five equations being solved.
Select Print and Plot under Options. This will print as well plot the residuals as they are calculated which you will use to monitor convergence.
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 Compute From. The Axial Velocity for all cells will be set to 1 m/s, the Radial Velocity to 0 m/s and the Gauge Pressure to 0 Pa. The Turbulence Kinetic Energy and Dissipation Rate (scroll down to see it) values are set from the prescribed values for the 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 OK. Check that the file has been created in your working directory.
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 OK. Check that the file has been created in your working directory.
Go to Step 6: Results