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.

create project

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.

select model parameters

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 geometry button -> primitives -> sphere. This adds a sphere constructed of triangles (STL) to the project.

enter geometry

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.

enter geometry

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

enter mesh

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_region (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 region 1

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

  • Click the left_region

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

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

  • Click the right_region

  • 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 front_region

  • 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

create region 2

3.4.6. Create Initial Conditions

  • Select the Initial conditions pane

  • Select the already populated “Background IC” 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 add 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 add 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 add 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

new boundary condition
  • Select the VTK sub-pane

  • Create a new output by clicking the add 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 save button

  • Run the project by clicking the play button

  • On the Run Solver dialog, select the executable

  • Click the Run button to actually start the simulation

new boundary condition

3.4.11. View results

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

  • Create a new visualization tab by pressing the add 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.

results