Step 3: Meshing the Geometry in the ANSYS Meshing Application

Now that you have created the mixing elbow geometry, you need to generate a computational mesh throughout the flow volume. For this tutorial, you will use the ANSYS Meshing application to create a mesh for your CFD analysis.

Note the Refresh Required icon ( ) within the Mesh cell for the system. This indicates that the state of the cell requires a refresh and that upstream data has changed since the last refresh or update (e.g., the geometry). Once the mesh is defined, the state of the cell will change accordingly. Likewise for the state of the remaining cells in the system. For more information about system cell states, see the separate FLUENT in Workbench User's Guide and the on-line documentation for ANSYS Workbench.

1.   Open the ANSYS Meshing application.

In the ANSYS Workbench Project Schematic, double-click the Mesh cell in the elbow fluid flow analysis system (cell A3). This displays the ANSYS Meshing application with the elbow geometry already loaded. You can also right-click on the Mesh cell to display the context menu where you can select the Edit... option.

Figure 1.11: The ANSYS Meshing Application with the Elbow Geometry Loaded

The first time you open the ANSYS Meshing application, the Meshing Options are displayed on the right-hand side of the application window where you can set various meshing options. For the purposes of this tutorial, nothing needs be set here, so click OK to close the Meshing Options window.

2.   Create named selections for the geometry boundaries.

In order to simplify your work later on in ANSYS FLUENT, you should label each boundary in the geometry by creating named selections for the pipe inlets, the outlet, and the symmetry surface (the outer wall boundaries are automatically detected by ANSYS FLUENT).

(a)   Select the large inlet in the geometry that is displayed in the ANSYS Meshing application.

(b)   Right-click and select the Create Named Selection option.

Figure 1.12: Selecting a Face to Name

This displays the Selection Name dialog box.

Figure 1.13: Applying a Name to a Selected Face

(c)   In the Selection Name dialog box, enter velocity-inlet-large for the name and click OK.

(d)   Perform the same operations for the smaller inlet velocity-inlet-small, the large outlet ( pressure-outlet), and the symmetry planes ( symmetry).

   To select multiple planes, hold down the $<CTRL>$ key and select the individual planes in the graphics window.

It is important to note that by using the strings "velocity inlet" and "pressure outlet" in the named selections (with or without hyphens or underscore characters), ANSYS FLUENT automatically detects and assigns the corresponding boundary types accordingly.

3.   Set some basic meshing parameters for the ANSYS Meshing application.

(a)   In the Outline view, select Mesh under Project/Model to display the Details view below the Outline view.

Note that since the ANSYS Meshing application automatically detects that you are going to perform a CFD fluid flow analysis using ANSYS FLUENT, the Physics Preference is already set to CFD and the Solver Preference is already set to Fluent.

(b)   Expand the Sizing node to reveal additional sizing parameters, and make sure that Use Advanced Size Function is set to On:Curvature.

(c)   Expand the Inflation node to reveal additional inflation parameters, and change Use Automatic Tet Inflation to Program Controlled.

4.   Generate the mesh.

Right-click Mesh in the project Outline tree, and select Update in the context menu.

Note:    Once the mesh is generated, to view the mesh statistics, open the Statistics node in the Details view to reveal information about the number of nodes, the number of elements, and other details.

Figure 1.14: The Computational Mesh for the Elbow Geometry in the ANSYS Meshing Application

Using the Generate Mesh option creates the mesh, but does not actually create the relevant mesh files for the project and is optional if you already know that the mesh is acceptable. Using the Update option automatically generates the mesh and creates the relevant mesh files for your project and updates the ANSYS Workbench cell that references this mesh.

5.   Close the ANSYS Meshing application.

You can simply close the ANSYS Meshing application. ANSYS Workbench automatically saves the mesh and updates the Project Schematic accordingly (the Refresh Required icon in the Mesh cell is replaced by a check mark, indicating that there is a mesh now associated with the fluid flow analysis system).

6.   View the files generated by ANSYS Workbench.

View $\rightarrow$ Files

Figure 1.15: ANSYS Workbench Displaying the Files View for the Project After Mesh Creation

Note the addition of the mesh files ( FFF.msh and FFF.mshdb) to the list of files. The FFF.msh file is created when you updated the mesh, and the FFF.mshdb file is generated when you close the ANSYS Meshing application.