The structure is made up of beams. You may recall that a beam is a structural element whose length is very large compared to the other two dimensions.

Units: Use S.I. units ONLY

Geometry: The members have a annular cross-section. The cross sections (A) of each of the truss members is 5.5e-3 sq meter. The polar radius of gyration (R) is 5.5e-2 meter. (hint: Use the values of A and R to find Izz then find the value of the outer diameter (The beam height))

Material: Assume the structure is made of steel with modulus of elasticity E=210 GPa.

Boundary conditions:  All the DOFs are constrained at the bottom end, i.e. the bottom end is a built-in end.

Loading: The structure is loaded at the ends of the two arms. The load is in the negative Y direction. The load value is 5000 N each.

Objective:

	To determine deflections at the points of application of load.
	To determine the maximum stress in the structure.
	Also determine the maximum possible load the frame can take. Look up for the value of yield stress for steel. Assume a factor of safety of 1.25.

You are required to hand in print outs for the above.

Figure:

Click on ANSYS 6.1 in the programs menu.

Select Interactive.

The following menu that comes up. Enter the working directory. All your files will be stored in this directory. Also enter 64 for Total Workspace and 32 for Database.

Click on Run.

Go to the ANSYS Utility Menu

Click Workplane>WP Settings

The following window comes up

Check the Cartesian and Grid Only buttons

Enter the values shown in the above.

Go to the ANSYS Main Menu

Click Preprocessor>Modeling>Create>Keypoints>On Working Plane

The following window comes up

Now we will pick the end points of the trusses.

	5 meters is now 1 X 5 units, since each cell in the grid is 1 unit across, 5 meters is 5 cells wide.
	Using this conversion select the keypoints on the workplane grid. Your points should look like this.

If you cannot see the complete workplane then go to Utility Menu>PlotCntrls>Pan Zoom Rotate and zoom out to see the entire workplane.

Now create lines connecting the keypoints

	Click on Preprocessor>Modeling>Create>Lines>Lines>Straight Line
	Create lines by picking keypoints to make the figure shown below.

Go to the ANSYS Main Menu

Click Preprocessor>Material Props>Material Models.  In the window that comes up choose Structural>Linear>Elastic>Isotropic. The following window will appear.

Double Click Isotropic. The following window comes up.

Fill in 2.1e11 for the Young's modulus and 0.3 for Poisson's Ratio. Click OK

Now the material 1 has the properties defined in the above table. We will use this material for the structure.

Click Preprocessor>Element Type>Add/Edit/Delete... In the 'Element Types' window that opens click on Add... The following window opens.

Type 1 in the Element type reference number.

Click on Structural Beam and select 2D elastic. Click OK. Close the 'Element types' window.

So now we have selected Element type 1 to be a structural Beam- 2D elastic element. The trusses will be modeled as elements of type 1, i.e. structural beam element. This finishes the selection of element type.

Now we need to define the cross sectional area, the second moment of inertia etc. for this element.

Go to Preprocessor>Real Constants.

In the "Real Constants" dialog box that comes up click on Add

In the "Element Type for Real Constants" that comes up click OK. The following window comes up

Type in 5.5e-3 for cross sectional area, calculate Izz from the value of the cross-sectional area and polar radius of gyration and enter it. Also calculate and enter the height and click on OK. The height of the beam is required to calculate the maximum stress, which will be at the top surface of the beam.

We have now defined the geometric properties of the beam element.

Go to Preprocessor>Meshing>Size Controls>Manual Size>Lines>All Lines. In the menu that comes up type 1 in the field for 'Number of element divisions'.

Click on OK.

Now go to Preprocessor>Meshing>Mesh>Lines

Select all the lines and click on OK in the "Mesh Lines" dialog box.

Now each line is a truss element (Element 1).

The tower is constrained in the DOFs at the bottom node.

Go to Main Menu

Click on Preprocessor>Loads>Define Loads>Apply>Structural>Displacement>On Keypoints.

Select the keypoint on which you want to apply displacement constraints. The following window comes up.

Select All DOF and click OK.

Go to Main Menu

Click on Preprocessor>Loads>Define Loads>Apply>Forces/Moment>On Nodes.

Select the top right node and the top left node.

Click on OK in the 'Apply F/M on Nodes' window. The following window will appear.

Enter the value of the force.