Geometry

Initial settings

In order to make sure the geometry data gets 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. A window should pop up asking for units. Units are in meters, so select Meters and press Ok. 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.

Proper Orientation

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 axes in the bottom right corner should be oriented as they are in the image below.

Line Sketching

First instinct is to make a rectangular solid as a model for our cantilever; While this would work, it would make the mesh more complex than it needs to be. This is a one-dimensional problem, so all we really need at our base is a one-dimensional figure: a line; (We still need to tell ANSYS it has volume, though.)

Click once on the Sketching tab, , which appears at the bottom of the Tree Outline. Click once on the Line button, , 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 at 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 the Horizontal button, . 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 H1 above the horizontal line as shown below.


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 numerical value of H1 to 4 meters and press enter.

Line Body

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, as can be seen in the following picture.


Next, click on the blue horizontal line that you drew. The blue horizontal line should have changed from blue to yellow as can be seen below.


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 ; it is located on the top left portion of the Design Modeler.

Cross Section

Now, a cross section will be given to the line body; First go to Concept then click on Cross Section then finally click on Rectangular, as shown below.


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, as can be seen below;


Then click on the Generate button, .

Assign the Cross Section with the Line Body

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 yellow box to the right of Cross Section under the Details of Line Body. Click on the yellow box and select rect1 as seen below. ANSYS will calculate the moment of inertia along the line body rather than the rectangular model.

Verify Geometry

At this point the specified geometry can be checked in order to make sure all has gone well; Click on View > Cross Section Solids, as shown below;


If you click on the 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. Don't worry - your work will be saved.

Go to Step 3: Mesh

Go to all ANSYS Learning Modules