ANSYS 12 - Beam (2D Element) - Step 2

Step 2: Geometry

Our geometry is 2D. At Workbench, in the Beam cell, right click on Geometry, and select Properties. You will see the properties menu on the right of the Workbench window. Under Advance Geometry Options, change the Analysis Type to 2D.

In the Project Schematic, double left 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 meterunit and click OK.

Strategy for Geometry Creation

We need to apply point boundary conditions at four points A, B, C and D shown in the figure below. In ANSYS, point boundary conditions are applied to nodes. When we mesh the rectangle using the ANSYS Mesher, nodes will automatically be created at A and B since these are corner points; the corresponding displacement BC's can be applied to these corner nodes. However, there is no guarantee that there will be nodes exactly at C and D since these are not corners. In this case, ANSYS will apply the forces at the nodes that are closest to C and D. This is possibly acceptable if the mesh is sufficiently fine.

 
An alternative scenario is that we get clever and force C and D to be exact points. This can be done by splitting the top and bottom edges into three section as shown below. This will force nodes to be created at points C and D. Then, the point forces can be applied to these nodes. This is the strategy we'll use in creating the geometry.

Creating a Sketch

Like any other common CAD modeling practice, we start by creating a sketch.

Start by creating a sketch on the XYPlane. Under Tree Outline, select XYPlane, then click on Sketching next to Modeling tab. This will bring up the Sketching Toolboxes.

Note: In sketching mode, there is Undo features that you can use if you make any mistake.

Select Sketching Toolbox Demo

On the right, there is a Graphic window. At the lower right hand corner of the Graphic window, click on the +Z axis to have a normal look of the XY Plane.

Select Normal View Demo

In the Sketching Toolboxes, select Rectangle. In the Graphicswindow, create a rough Rectangle from starting from the origin in the positive XY direction (Make sure that you see a letter P at the origin before you start dragging the rectangle. The letter P at the origin means the geometry is constrained at the origin.)

You should have something like this:

Note: You do not have to worry about geometry for now, we can dimension them properly in the later step.

Modify the Sketch

We would like to split the top and bottom with three edges. Click Modify tab and select Split. Roughly select four points on the top and bottom of the rectangle.

Dimensions and Constraints

Under Sketching Toolboxes, select Dimensions tab, use the default dimensioning tools. Dimension the geometry as shown:

 
Now we need to constraint the lower rectangle with the top of the rectangle which has been properly dimensioned. Click Constraints tab, select Equal Length. Click the appropriate top and bottom edge and set them to be of equal length.

Under Details View on the lower left corner, input the value for dimension appropriately.
V1: 0.05 m
H2: 0.1 m
H3: 0.2 m
H4: 0.1 m

At this point, you should see something like this for your sketch:

Create Surface 

Now that we have the sketch done, we can create a surface for this sketch.

Concept > Surfaces From Sketches

This will create a new surface SurfaceSK1. Under Details View, select Sketch1 as Base Objects and click Apply. Finally click Generate to generate the surface. This is what you should see under your Tree Outline.

You can close the Design Modeler and go back to Workbench (Don't worry, it will auto save).

Go to Step 3: Mesh

See and rate the complete Learning Module

Go to all ANSYS Learning Modules