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 |
+------------------+-----------------------------------+
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.
.. figure:: /media/gui_new_project.png
:width: 8cm
:alt: create project
Select model parameters
^^^^^^^^^^^^^^^^^^^^^^^
On the ``Model`` pane:
- Enter a descriptive text in the
``Description`` field
- Select "Single-phase" in the ``Solver`` drop-down menu.
.. figure:: /media/gui_sphere_model.png
:width: 8cm
:alt: select model parameters
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.
.. figure:: /media/gui_sphere_add_geometry.png
:width: 8cm
:alt: 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.
.. figure:: /media/gui_sphere_geometry.png
:width: 8cm
:alt: enter geometry
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
.. figure:: /media/gui_sphere_mesh.png
:width: 8cm
:alt: enter mesh
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.
.. figure:: /media/gui_sphere_region1.png
:width: 8cm
:alt: 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
.. figure:: /media/gui_sphere_region2.png
:width: 8cm
:alt: create region 2
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
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.
Select output options
^^^^^^^^^^^^^^^^^^^^^
On the ``Output`` pane:
- On the ``Basic`` sub-pane, check the
``Write VTK output files (VTU/VTP)`` checkbox
.. figure:: /media/gui_tfm_2d_output.png
:width: 8cm
:alt: 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
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
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
.. figure:: /media/gui_run_dialog.png
:width: 8cm
:alt: new boundary condition
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.
.. figure:: /media/gui_sphere_results.png
:width: 8cm
:alt: results
.. include:: /icons.rst