3.4. Three-dimensional single-phase flow over a sphere¶

This tutorial shows how to create a three dimensional single-phase flow over a sphere.

Property	Value
geometry	60 cm 20 cm x 20 cm
mesh	30 x 10 x 10
gas velocity	1 m/s
temperature	298 K
pressure	101325 Pa

3.4.1. Create a new project¶

On the main menu, select New project
Create a new project by double-clicking on “Blank” template.
Enter a project name and browse to a location for the new project.
When prompted to enable SMS workflow, answer No, we will use the standard workflow for this tutorial.

Note

A new project directory will be created in the location directory, with the name being the project name.

3.4.2. Select model parameters¶

On the Model pane:

Enter a descriptive text in the Description field
Select “Single-phase” in the Solver drop-down menu.

3.4.3. Enter the geometry¶

On the Geometry pane enter the domain extents:

60/100 meters for the maximum x value
20/100 meters for the maximum y value
20/100 meters for the maximum z value

Next, add a sphere by clicking the button -> primitives -> sphere. This adds a sphere constructed of triangles (STL) to the project.

Change the center position and radius of the sphere so that it is located in the domain by entering the following:

10/100 for the center X position
10/100 for the center Y position
10/100 for the center Z position

Change the radius of the sphere by entering:

5/100 for the radius.

3.4.4. Enter the mesh¶

On the Mesh pane, Background sub-pane:

Enter 30 for the x cell value
Enter 10 for the y cell value
Enter 10 for the z cell value

3.4.5. Create regions for initial and boundary condition specification¶

Select the Regions pane. By default, a region that covers the entire domain is already defined.

A region for the sphere is needed to apply a wall boundary condition to:

Click the (all) button to create a region that encompasses the entire domain
change the name of the region to a descriptive name such as “sphere”
Check the Select facets (STL) checkbox to turn the region into a STL region. The facets of the sphere should now be selected.

Create a region to apply a mass inflow boundary condition to:

Click the
Enter a name for the region in the Name field (“inlet”)

Create a region to apply a pressure outlet boundary condition to:

Click the
Enter a name for the region in the Name field (“outlet”)

Finally, create a slice through the center to use as a vtk output region:

Click the
Enter a name for the region in the Name field (“slice”)
Enter zmax/2 in both the From Z and To Z fields to move the region to the center of the domain

3.4.6. Create Initial conditions¶

Select the Initial conditions pane
Select the already populated “Background” from the region list. This will initialize the entire flow field with air.
Enter 101325 Pa in the Pressure (optional) field

3.4.7. Create Boundary conditions¶

Select the Boundary conditions pane and create a wall boundary condition for the sphere by:

clicking the button
On the Select region dialog, select “No Slip Wall” from the Boundary type combo-box
Select the “sphere” region and click OK

Add a mass inflow boundary condition by:

clicking the button
On the Select region dialog, select “Mass Inflow” from the Boundary type combo-box
Select the “inlet” region and click OK
On the “Fluid” sub-pane, enter a velocity in the X-axial velocity field of 1.0 m/s

Finally, create a pressure outlet boundary condition by:

clicking the button
On the Select region dialog, select “Pressure outflow” from the Boundary type combo-box
Select the “outlet” region and click OK

Note

The default pressure is already set to 101325 Pa, no changes need to be made to the outlet boundary condition.

3.4.8. Select output options¶

On the Output pane:

On the Basic sub-pane, check the Write VTK output files (VTU/VTP) checkbox

Select the VTK sub-pane
Create a new output by clicking the button
Select the “slice” region from the list to save cell data at a slice through the domain
Click OK to create the output
Change the Write interval to “0.01” seconds
Select the Pressure, Velocity vector, Velocity x-component, Velocity y-component, and Velocity z-component checkboxes on the Fluid sub-sub-pane

3.4.9. Change run parameters¶

On the Run pane:

Change Stop time step to 2.0 seconds
Change Time step to 1e-2 seconds
Change Maximum time step to 1e-2 seconds

3.4.10. Run the project¶

Save project by clicking the button
Run the project by clicking the button
On the Run Solver dialog, select the executable
Click the Run button to actually start the simulation

3.4.11. View results¶

Results can be viewed, and plotted, while the simulation is running.

Create a new visualization tab by pressing the next to the Model tab
Select an item to view, such as plotting the time step (dt) or click the 3D view button to view the vtk output files.
On the VTK results tab, the visibility and representation of the *.vtk files can be controlled with the menu on the side.