ANSYS 12 - Cantilever Beam Geometry

Step 2: Geometry

Double-click on the geometry button, ,   in the Project Schematic area, which should launch the Design Modeler in ANSYS.
A folder called "A: Static Structural (ANSYS) should be expanded in the tree outline of the Design Modeler.  If it is not expanded, then expand it now.

Click once on the XYPlane button, .  Next, click once on the royal blue Z vector (displayed below) which should be in the bottom right section of the Design Modeler window.
Now, you should be looking directly at the XY plane and the axises in the bottom right corner should be oriented as they are in the image below.

 
Click once on the "Sketching" Tab which appears at the bottom of the Tree Outline.
Click once on "Line" in the "Draw" tab that automatically appears. Then place the mouse cursor directly over the origin of the XY plane unit a P appears.  Once the P appears then click once on the mouse. Next, move the mouse over to the right so it lies somewhere on the positive x axis.  Prior, to clicking again make sure that a C appears. You should now have a line that starts a the origin and terminates somewhere on the positive axis.

At this point, the dimension of the line needs to be specified, so click once on the "Dimensions" tab.  Then, click once on "Horizontal". The next step is to click somewhere on the y axis and then click on the endpoint of the line (the point that lies upon the positive x axis). Now, raise the cursor (which should now be a horizontal line and a pencil) above the line and click once.  You should see a dimension labeled H2 above the horizontal line. Now, the length of the line will be manually edited. Underneath the "Sketching Toolboxes" there will be a column called "Details View". In "Details View there is a subcategory called "Dimensions: 1". Change the numerically value of H1 to 4 meters and press enter.

The next step is to turn the line that was drawn into a line body. In order to do this click on "Concept" which will be on top of the Design Modeler window, then click on "Lines from Sketches". Next, click on the blue horizontal line that you drew. The blue horizontal line should have changed from blue to yellow. In the "Details View" column a yellow box to the right of "Base Objects" should be highlighted in yellow. Click on the yellow box and then click apply. Then, click on the "Generate" button which has a lightening bolt on it and is located on the top left portion of the Design Modeler.

Now, a cross section will be given the line body.  First go to "Concept" then go click on "Cross Section" then finally click on "Rectangular".  Now, the width and height of the cross section need to be defined.  Under "Details View" set B to 0.346 meters and set H to 0.346 meters. Then click on the "Generate" button.

Now the defined cross section will be "merged" with the line body.  First, expand "1 Part, 1 Body" which is located in the "Tree Outline". Next, click on "Line Body", and there should be a yellox box to the right of Cross Section under the "Details of Line Body". Click on the yellow box and select "rect1".

At this point the specified geometry can be checked in order to make sure all has gone well.  Click on "View" and then "Cross Section Solids".  If you click on "1 Cross Section" in the Tree Outline and then click on the light blue dot  you should now see a three dimensionally rendered beam in an isometric view. At this point, the Design Modeler window can be closed.

Exporting The Geometry to The Model

In order to make sure to get the geometry data transferred to the Model a couple of steps must be taken.  First, right click on "Geometry" then click on "Properties". Under "Properties of Schematic A3: Geometry" expand "Basic Geometry Options" and check the box to the right of "Line Bodies" as seen below. Double-click on the geometry button in the Project Schematic area, which should launch the Design Modeler in ANSYS.