.. _3D_fluidbed_tutorial: Three Dimensional Fluidized Bed ------------------------------- This tutorial shows how to create a three dimensional fluidized bed simulation using the two fluid model 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 ^^^^^^^^^^^^^^^^^^^^ - (:numref:`fig_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 ^^^^^^^^^^^^^^^^^^^^^^^ (:numref:`fig_model_param`): 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| 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| 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| 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| button to create a new region to be used to select the walls. - Enter a name for the region in the ``Name`` field ("walls") 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| 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 IC" 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 IC" 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`` check-boxes 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`` check-boxes 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