Child pages
• FLUENT - Turbulent Flow Past a Sphere - Step 4

FLUENT - Turbulent Flow Past a Sphere - Step 4

UNDER CONSTRUCTION

Author: Daniel Kantor and Andrew Einstein, Cornell University

Step 4: Set Up Problem in FLUENT

Launch Fluent

Lab Apps > FLUENT 6.3.26

Select 3ddp from the list of options and click Run.

The "3ddp" option is used to select the 3-dimensional, double-precision solver. In the double-precision solver, each floating point number is represented using 64 bits in contrast to the single-precision solver which uses 32 bits. The extra bits increase not only the precision but also the range of magnitudes that can be represented. The downside of using double precision is that it requires more memory.

Import Grid

Navigate to the working directory and select the SingleSphere.msh file. This is the mesh file that was created using the preprocessor GAMBIT in the previous step. FLUENT reports the mesh statistics as it reads in the mesh:

Check the number of nodes, faces (of different types) and cells. Also, take a look under zones. We can see the three zones inlets, outlet, and sphere that we defined in GAMBIT.

Check and Display Grid

First, we check the grid to make sure that there are no errors.

Main Menu > Grid > Check

Any errors in the grid would be reported at this time. Check the output and make sure that there are no errors reported. Check the grid size:

Main Menu > Grid > Info > Size

The following info should appear (your number of cells might be slightly different because of slight different mesh criteria used):

To view the grid we first need to create a plane that cuts our 3D model in half (otherwise it would be too hard to see a good profile of the mesh). To do this we go into:

Main Menu > Surfaces > Plane...

We change the values to:
x0 =0; x1=0; x2=1;
y0=0; y1=1; y2=0;
z0=0; z1=0; z2=0;

It will look like this:

We name this Plane_Split. To view the grid we now go to:

Main Menu > Display > Grid...

Make sure we select our surface under Surfaces. Then click Display. The graphics window opens and the grid is displayed in it. You can now click Close in the Grid Display menu to get back some desktop space. The graphics window will remain.

Graphics Window Operation

Translation: The grid can be translated in any direction by holding down the Left Mouse Button and then moving the mouse in the desired direction.
Zoom In: Hold down the Middle Mouse Button and drag a box from the Upper Left Hand Corner to the Lower Right Hand Corner over the area you want to zoom in on.
Zoom Out: Hold down the Middle Mouse Button and drag a box anywhere from the Lower Right Hand Corner to the Upper Left Hand Corner.

Use these operations to zoom into the grid to obtain the view shown below.

The zooming operations can only be performed with a middle mouse button.

White Background on Graphics Window

To get white background go to:
Main Menu > File > Hardcopy
Make sure that Reverse Foreground/Background is checked and select Color in Coloring section. Click Preview. Click No when prompted "Reset graphics window?"

You can also look at specific parts of the grid by choosing the boundaries you wish to view under Surfaces (click to select and click again to deselect a specific boundary). Click Display again when you have selected your boundaries.

Define Solver Properties

Main Menu > Define > Models > Solver

Choose Pressure Based under Solver, Absolute under Velocity Formulation, Green-Gauss Node Based under Gradient Option, Unsteady under Time , 2nd-Order Implicit under Unsteady Formulation, and Superficial Velocity under Porous Formulation.

Main Menu > Define > Models > Viscous

Choose k-omega Model and check the SST. Leave all other values alone.

Main Menu > Define > Models > Energy

For incompressible flow, the energy equation is decoupled from the continuity and momentum equations. We need to solve the energy equation only if we are interested in determining the temperature distribution. We will not deal with temperature in this example. So leave the Energy Equation unselected and click Cancel to exit the menu.

Define Material Properties

Main Menu > Define > Materials...

The default values are the ones that we are going to use so we do not need to change anything here. These are the values that we specified under Problem Specification.

Click Change/Create. Close the window.

Define Operating Conditions

Main Menu > Define > Operating Conditions...

For all flows, FLUENT uses gauge pressure internally. Any time an absolute pressure is needed, it is generated by adding the operating pressure to the gauge pressure. We'll use the default value of 1 atm (101,325 Pa) as the Operating Pressure.

Click Cancel to leave the default in place.

Define Boundary Conditions

Main Menu > Define > Boundary Conditions...

Select Inlets and click Set. We should set Velocity Specification Method to Components, and set X-velocity to 2.7754. In the Turbulence Area, we should set Specification Method to Intensity and Length Scale, and set Turbulent Intensity to 1.

All other Boundary Conditions have been set during the meshing process so nothing else should be modified here.

Click Close to close the Boundary Conditions menu.

Go to all FLUENT Learning Modules

• No labels