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
fieldSelect “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 value20/100
meters for the maximum y value20/100
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 position10/100
for the center Y position10/100
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 valueEnter
10
for the y cell valueEnter
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:
Create a region to apply a pressure outlet boundary condition to:
Finally, create a slice through the center to use as a vtk output region:
3.4.6. Create Initial Conditions¶
Select the
Initial conditions
paneSelect the already populated “Background IC” from the region list. This will initialize the entire flow field with air.
Enter
101325
Pa in thePressure (optional)
field
3.4.7. Create Boundary Conditions¶
Select the Boundary conditions
pane and create a wall boundary condition for
the sphere by:
On the
Select region
dialog, select “No Slip Wall” from theBoundary type
combo-boxSelect the “sphere” region and click
OK
Add a mass inflow boundary condition by:
On the
Select region
dialog, select “Mass Inflow” from theBoundary type
combo-boxSelect the “inlet” region and click
OK
On the “Fluid” sub-pane, enter a velocity in the
X-axial velocity
field of1.0
m/s
Finally, create a pressure outlet boundary condition by:
On the
Select region
dialog, select “Pressure outflow” from theBoundary type
combo-boxSelect 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 theWrite VTK output files (VTU/VTP)
checkbox
Select the
VTK
sub-paneSelect the “slice” region from the list to save cell data at a slice through the domain
Click
OK
to create the outputChange the
Write interval
to “0.01” secondsSelect the
Pressure
,Velocity vector
,Velocity x-component
,Velocity y-component
, andVelocity z-component
checkboxes on theFluid
sub-sub-pane
3.4.9. Change run parameters¶
On the Run
pane:
Change
Stop time step
to2.0
secondsChange
Time step
to1e-2
secondsChange
Maximum time step
to1e-2
seconds
3.4.10. Run the project¶
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.