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| 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)`` check-box 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 IC" 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 inlet 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`` check-boxes on the ``Fluid`` sub-sub-pane Change run parameters ^^^^^^^^^^^^^^^^^^^^^ On the ``Run`` pane: - Change the ``Stop Time step`` to ``2.0`` seconds - Change the ``Time step`` to ``1e-2`` seconds - Change the ``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