Geometry

For users of ANSYS 15.0, please check this link for procedures for turning on the Auto Constraint feature before creating sketches in DesignModeler.

Saving

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 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. In order 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.

Fluid Flow (FLUENT) Project Selection

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 work space. This is the place where you will organize your project. At the bottom of the window, you see messages from ANSYS.

Left click (and hold) on  Fluid Flow (FLUENT) , and drag the icon into the empty space in the  Project Schematic . Your ANSYS 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. 

Analysis Type

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  Advance Geometry Options , change the  Analysis Type  to 2D as shown in the image below. 

 

Launch Design Modeler

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 desired length unit. Use the default meter unit and click  OK

Creating a Sketch

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  tab, 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. 

 

Dimensions

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. 

 

Surface Body Creation

In order 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 the  Design Modeler  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


Go to Step 3: Mesh

Go to all FLUENT Learning Modules

  • No labels