Sign-up for free online course on ANSYS simulations!UNDER CONSTRUCTION
Author: Daniel Kantor and Andrew Einstein, Cornell University
Problem Specification
1. Create Geometry in GAMBIT
2. Mesh Geometry in GAMBIT
3. Specify Boundary Types in GAMBIT
4. Set Up Problem in FLUENT
5. Solve!
6. Analyze Results
7. Refine Mesh
Problem 1
Step 5: Solve!
We'll use a second-order discretization scheme.
Main Menu > Solve > Controls > Solution...
Take a look at the options available. Under Discretization, set Pressure to Standard, set Momentum to Second Order Upwind, set Turbulent Kinetic Energy to Second Order Upwind, and set Specific Dissipation Rate to Second Order Upwind. All other values should remain at their default.
Click OK.
Set Initial Guess
Initialize the flow field 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 X Velocity for all cells will be set to 2.7754 m/s, the Y Velocity to 0 m/s and the Gauge Pressure to 0 Pa. These values have been taken from the inlet boundary condition.
Click Init. This completes the initialization. Close the window.
Set Convergence Criteria
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...
Change the residual under Convergence Criterion for continuity, x-velocity, and y-velocity, all to 1e-6.
Also, under Options, select Plot. This will plot the residuals in the graphics window as they are calculated.
Click OK.
Monitor also the drag and lift coefficient on the sphere.
Main Menu > Solve > Monitors > Force...
Select Sphere under Wall Zones. Under Options, select Print, Plot and Write. Under Coefficient, choose Drag. Click Apply.
Choose Sphere under Wall Zones. Under Options, select Print, Plot and Write. Under Coefficient, choose Lift. Click Apply.
Setting Reference Values
To plot C d and C l we need to set the reference value.
Main Menu > Report > Reference Values...
Under Reference Values, change Area to 28.274, Density to 1.225, Velocity to 2.7754 and Viscosity to 1.7894E-05.
Click OK.
This completes the problem specification. Save your work:
Main Menu > File > Write > Case...
Type in SingleSphere.cas for Case File. Click OK. Check that the file has been created in your working directory. If you exit FLUENT now, you can retrieve all your work at any time by reading in this case file.
Iterate Until Convergence
Main Menu > Solve > Iterate...
In the Iterate Window that comes up, change the Time Step Size to 1, change the Number of Time Steps to 100, and change Max Iterations per Time Step to 10. Click Iterate. 
The residuals and drag coefficients for each iteration are printed out as well as plotted in the graphics window as they are calculated.
Save the solution to a data file:
Main Menu > File > Write > Data...
Enter SingleSphere.dat for Data File and click OK. Check that the file has been created in your working directory. You can retrieve the current solution from this data file at any time.