.. _3D_fluidbed_tutorial:
Three-dimensional fluidized bed
-------------------------------
This tutorial shows how to create a three dimensional fluidized bed
simulation using the two-fluid model (TFM) and the discrete element
model (DEM). The model setup is:
+------------------+--------------------------------------------+
| Property | Value |
+==================+============================================+
| geometry | 10 cm diameter x 40 cm |
+------------------+--------------------------------------------+
| mesh | 20 x 60 x 20 |
+------------------+--------------------------------------------+
| solid diameter | 200 microns (:math:`200 \times 10^{-6}` m) |
+------------------+--------------------------------------------+
| solid density | 2500 kg/m\ :sup:`2` |
+------------------+--------------------------------------------+
| gas velocity | 0.25 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.
.. _fig_new_project:
.. 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 "Two-Fluid Model (MFiX-TFM)" in the ``Solver`` drop-down menu.
.. _fig_model_param:
.. figure:: /media/gui_3d_tfm_model.png
:width: 8cm
:alt: select model parameters
Enter the geometry
^^^^^^^^^^^^^^^^^^
On the ``Geometry`` pane:
- Create the cylindrical geometry by pressing the ``Add Geometry`` button
-> ``Primitives`` -> ``cylinder``
.. figure:: /media/gui_3d_tfm_add_cylinder.png
:width: 8cm
:alt: add cylinder
- Enter ``40/100`` meters for the cylinder height
- Enter ``10/2/100`` meters for the cylinder radius
- Enter ``30`` for the cylinder resolution
- Press the autosize button to fit the domain extents to the geometry
- Extend the height of the cylinder by adding ``0.1`` meters. This will hang
the stl file outside of the domain, allowing for a sharp and clean cut.
- Flip the normals by clicking the |filter| button and selecting the ``flip normals`` filter
.. figure:: /media/gui_3d_tfm_add_geo.png
:width: 8cm
:alt: enter cylinder input
Enter the mesh
^^^^^^^^^^^^^^
On the ``Mesh`` pane:
- On the ``Background`` sub-pane
- Enter ``20`` for the x cell value
- Enter ``60`` for the y cell value
- Enter ``20`` for the z cell value
.. note::
This is a fairly coarse grid for a TFM simulation. After completing this
tutorial, try increasing the grid resolution to better resolve the bubbles.
.. figure:: /media/gui_3d_tfm_add_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. This is typically used to initialize the flow field and
visualize the results.
- Click the |all_region| (all) button to create a new region to be used for the bed initial condition.
- Enter a name for the region in the ``Name`` field ("bed")
- Change the color by pressing the ``Color`` button
- Enter ``0`` in the ``To Y`` field
.. figure:: /media/gui_3d_tfm_add_region1.png
:width: 8cm
:alt: create region 1
- Click the |bottom_region| (bottom) button to create a new region to be used by the gas inlet boundary condition.
- Enter a name for the region in the ``Name`` field ("inlet")
.. figure:: /media/gui_3d_tfm_add_region2.png
:width: 8cm
:alt: create region 2
- Click the |top_region| (top) button to create a new region to be used by the
pressure outlet boundary condition.
- Enter a name for the region in the ``Name`` field ("outlet")
.. figure:: /media/gui_3d_tfm_add_region3.png
:width: 8cm
:alt: create region 3
- Click the |all_region| (all) button to create a new region to be used to select the
walls.
- Enter a name for the region in the ``Name`` field ("walls")
- Click the ``Select facets`` box. The region type should change from "box" to "STL".
All the facets of the cylinder should now be selected. Since the cylinder is
outside the domain extents, normal cells (i.e. not cut-cells) will be placed at
the outlet and inlet. This allows for the standard boundary conditions to be
applied.
.. figure:: /media/gui_3d_tfm_add_region4.png
:width: 8cm
:alt: create region 4
- Click the |left_region| (left) button to create a new region to be used to save a slice of cells at the center of the domain.
- Enter a name for the region in the ``Name`` field ("slice")
- Enter ``0`` in the ``From X`` and ``To X`` fields
.. figure:: /media/gui_3d_tfm_add_region5.png
:width: 8cm
:alt: create region 5
Create a solid
^^^^^^^^^^^^^^
On the ``Solids`` pane:
- Click the |add| button to create a new solid
- Enter a descriptive name in the ``Name`` field ("glass beads")
- Accept the radial distribution setting (Carnahan-Starling)
- Enter the particle diameter of ``200e-6`` m in the ``Diameter`` field
- Enter the particle density of ``2500`` kg/m\ :sup:`2` in the ``Density`` field
.. figure:: /media/gui_3d_tfm_solids.png
:width: 8cm
:alt: create a solid
Create Initial conditions
^^^^^^^^^^^^^^^^^^^^^^^^^
On 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 a new Initial Condition by pressing the |add| button
- Select the region created previously for the bed Initial Condition
("bed" region) and click the ``OK`` button.
- Select the solid (named previously as "glass beads") sub-pane and
enter a volume fraction of ``0.4`` in the ``Volume Fraction`` field.
This will fill the bottom half of the domain with glass beads.
.. figure:: /media/gui_3d_tfm_ics.png
:width: 8cm
:alt: initial conditions
Create Boundary conditions
^^^^^^^^^^^^^^^^^^^^^^^^^^
On the ``Boundary conditions`` pane:
- Create a new Boundary condition by clicking the |add| button
- On the ``Select region`` dialog, select "Mass Inflow" from the
``Boundary type`` drop-down menu
- Select the "inlet" region and click ``OK``
- On the ``Fluid`` sub-pane, enter a velocity in the ``Y-axial velocity``
field of ``0.25`` m/s
- Create another 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.
- Create another Boundary condition by clicking the |add| button
- On the ``Select region`` dialog, select "No Slip Wall" from the
``Boundary type`` combo-box
- Select the "wall" region and click ``OK``
Change numeric parameters
^^^^^^^^^^^^^^^^^^^^^^^^^
On the ``Numerics`` pane, ``Residuals`` sub-pane:
- Enter ``0`` in the ``Fluid Normalization`` field.
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 |add| button
- Select the "Background" region from the list to save all the cell data
- Click ``OK`` to create the output
- Enter a base name for the ``*.vtu`` files in the ``Filename base``
field
- Change the ``Write interval`` to ``0.01`` seconds
- Select the ``Volume fraction``, ``Pressure``, and ``Velocity vector``
checkboxes on the ``Fluid`` tab
- Create another output by clicking the |add| button
- Select the "Slice" region from the list to save all the cell data
- Click ``OK`` to create the output
- Enter a base name for the ``*.vtu`` files in the ``Filename base`` field
- Change the ``Write interval`` to ``0.01`` seconds
- Select the ``Volume fraction``, ``Pressure``, and ``Velocity vector``
checkboxes on the ``Fluid`` tab
.. figure:: /media/gui_3d_tfm_output.png
:width: 8cm
:alt: initial conditions
Change run parameters
^^^^^^^^^^^^^^^^^^^^^
On the ``Run`` pane:
- Change the ``Stop time`` to ``1.0`` seconds
- Change the ``Time step`` to ``1e-3`` seconds
- Change the ``Maximum time step`` to ``1e-2`` seconds
.. figure:: /media/gui_tfm_2d_run.png
:width: 8cm
:alt: new boundary condition
Run the project
^^^^^^^^^^^^^^^
- Save project by clicking |save| button
- Run the project by clicking the |play| button
- On the ``Run`` dialog, select the default executable from the list
- Click the ``Run`` button to actually start the simulation
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_3d_tfm_results.png
:width: 8cm
:alt: new boundary condition
Convert this project into a 3D DEM simulation
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
- Click the |reset| button and delete all simulation files.
- Close the VTK window
- On the ``Model`` pane, change the solver to ``MFiX-DEM``
- On the ``Mesh`` pane, coarsen the grid to `15`, `45`, and `15` cells in the
in the x, y, and z direction, respectfully.
.. note::
The grid resolution needs to be coarser because we are drastically
increasing the particle diameter below. The fluid grid cell size has to be
bigger than the particle size.
- On the ``Solids`` pane, change that particle diameter to ``5.0000e-03`` to
get a more reasonable particle count for tutorial purposes.
- On the ``Solids`` pane, ``DEM`` sub-pane:
- check the ``Enable automatic particle generation``
- enter a value of ``15`` in the ``Search grid partitions``, ``KMAX`` field.
- On the ``Boundary conditions`` pane, change the ``inlet`` ``Y-axial
velocity`` to ``0.6`` m/s
- On the ``Boundary conditions`` pane, delete the ``walls`` boundary condition
and re-add it to write the correct wall parameters for the DEM simulation.
- On the ``Output`` pane, ``VTK`` sub-pane:
- Delete the ``all`` or ``Background_IC`` output
- Create a new output, change the ``Output type`` to ``Particle data`` and
select the ``Background_IC`` region.
- Change the write frequency to ``0.01``
- Select the ``Diameter`` and ``Translational Velocity`` data
- Run the simulation
- Create a VTK window to visualize the data. It will automatically show the slice (cell data) and the particles.
.. figure:: /media/gui_3d_dem_results.png
:width: 8cm
:alt: new boundary condition
.. include:: /icons.rst