First, save the project at this point. Click on the "Save As…" button, which is located at the top of the Workbench Project Page. Save the project as "suddenExpansionFlow" in your working directory. When you save in Ansys software a file and a folder will be created. For instance, if you save as "suddenExpansionFlow", a "suddenExpansionFlow" file and a folder called "suddenExpansionFlow_files" will appear. To reopen the Ansys files in the future you will need both the ".wbpj" file and the folder. If you do not have BOTH, you will not be able to access your project.
On the left-hand side of the Workbench window, you will see a toolbox full of various analysis systems. To the right, you see an empty workspace. This is the place where you will organize your project. At the bottom of the window, you see messages from the Ansys software.
Left click (and hold) on Fluid Flow (Fluent), and drag the icon into the empty space in the Project Schematic. Your Ansys Workbench window should now look comparable to the image below.
Since we selected Fluid Flow (Fluent), each cell of the system corresponds to a step in the process of performing CFD analysis using Fluent. Rename the project to suddenExpansion.
We will work through each step from top down to obtain the solution to our problem.
In the Project Schematic of the Workbench window, right click on Geometry and select Properties , as shown below.
The properties menu will then appear to the right of the Workbench window. Under Advanced Geometry Options, change the Analysis Type to 2D as shown in the image below.
In the Project Schematic , double click on Geometry to start preparing the geometry.
At this point, a new window, Ansys Design Modeler will be opened. You will be asked to select a length unit. Use the default meter unit and click OK .
Start by creating a sketch on the XYPlane . Under Tree Outline , select XYPlane , then click on Sketching right before Details View . This will bring up the Sketching Toolboxes .
Click on the +Z axis on the bottom right corner of the Graphics window to have a normal look of the XY Plane.
In the Sketching toolboxes, select Rectangle. In the Graphics window, create the first rough Rectangle by clicking once on the origin and then by clicking once somewhere in the positive XY plane. (Make sure that you see a letter P at the origin before you click. The P implies that the cursor is directly over a point of intersection.)
Repeat, and create the second rectangle with smaller length and width. Also, make sure these two rectangles are connected. At this point you should have something comparable to the image below.
The overlapped lines of these two rectangles are extraneous and will be removed. Under Sketching Toolboxes, click Modify and cut the line indicated by the figure below. This will delete the width of the smaller rectangle.
Then, trim the width (only the lower part) of the lager rectangle which overlaps the small rectangle. You should have the image below.
At this point the rectangle will be properly dimensioned.
Under Sketching Toolboxes, select Dimensions tab, use the default dimensioning tools. Dimension the geometry as shown in the following image.
Under the Details View table (located in the lower left corner), set H1=20m, H2=100m, V3=1m and V4 = 2m, as shown in the image below.
To create the surface body, first (Click )Concept > Surface From Sketches as shown in the image below.
This will create a new surface SurfaceSK1. Under Details View, select Sketch1 (go to XYplane and expand it to see Sketch1, click on it) as Base Objects, and then under Surface body select the thickness to 0.1m and click Apply. Finally, right click SurfaceSK1 and select Generate to generate the surface. You should see “1 part, 1 Body ” under SurfaceSK1.
At this point, you can close DesignModeler and go back to Workbench Project Page. You should see two green check marks next to Geometry and Mesh. Press Refresh Project and Update Project, then save your work thus far in the Workbench Project Page.
For users of Ansys 15.0, please check the following topic for procedures for turning on the Auto Constraint feature before creating sketches in DesignModeler.