Sign-up for free online course on ANSYS simulations!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. Change the Domain Size.
8. Unsteady Flow.
Problem Set.
Citations.
Set Up Problem in FLUENT
Launch FLUENT
Start > Programs > Fluent Inc > FLUENT 6.3.26
Select 2ddp from the list of options and click Run.
Import File
Main Menu > File > Read > Case...
Navigate to your working directory and select the cylinder.msh file. Click OK.
Analyze Grid
Grid > Info > Size
Check how many cells and nodes the mesh has.
Display > Grid
Display the grid information.
Define Properties
Define > Models > Solver...
Under the Solver box, select Pressure Based.
Click OK.
Define > Models > Viscous
Select Laminar under Model
Click OK.
Define > Models > Energy
Do not select Energy Equation.
Define > Materials
Make sure air is selected under Fluent Fluid Materials. Set Density to constant and equal to 1 kg/m 3 and Viscosity to 0.025 kg/m-s. We choose these numbers so that Re = 40.
Click Change/Create.
Define > Operating Conditions
We'll work in terms of gauge pressures in this example. So set Operating Pressure to the ambient value of 101,325 Pa.
Click OK.
Define > Boundary Conditions
Set inlet, click Set... and set the Velocity Magnitude to 1 m/s. Click OK.
Set outlet, click Set... and set the Gauge Pressure at this boundary to 0. Click OK.
Go to Step 5: Solve.