The tower is made up of trusses. You may recall that a truss is a structural element that experiences loading only in the axial direction. 

Units: Use S.I. units ONLY

Geometry: the cross sections of each of the truss members is 6.25e-3 sq. meter.

Material: Assume the structure is made of steel with modulus of elasticity E=200 GPa.

Boundary conditions: The tower is constrained along X and Y directions at the bottom left corner, and along Y direction at the bottom right corner.

Loading: The tower is loaded at the top. The load is in horizontal direction only, and its magnitude is 5000 N.

Objective:

	To determine deflection at each joint.
	To determine stress in each member.
	To determine reaction forces at the base.

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

Figure:

The five trusses at the top are each 3m in length.

IMPORTANT: Convert all dimensions and forces into SI units.

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. Give your file a jobname.

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 figure 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.

	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 which is shown below, for Material Model 1, choose Structural>Linear>Elastic>Isotropic.

Enter 1 for the Material Property Number and click OK. The following window comes up.

Fill in 2e11 for the Young's modulus and 0.3 for minor Poisson's Ratio. Click OK.

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

SELECTING ELEMENT TYPE:

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 Link and select 2D spar. Click OK. Close the 'Element types' window.

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

Now we need to define the cross sectional area 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 6.25e-3 for cross sectional area and click on OK.

We have now defined the cross sectional area of the link element.

DIVIDING THE TOWER INTO ELEMENTS:

Go to Preprocessor>Meshing>Size Cntrls>ManualSize>Lines>All Lines.

In the menu that comes up type 1 in the field for 'Number of element divisions'. This divides each of the lines in your figure into 1 element.

Click on OK. Now when you mesh the figure ANSYS will automatically divide each line into 1 element.

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).

APPLYING BOUNDARY CONDITIONS

	The tower is constrained in the X and Y directions at the bottom left corner and in the Y direction at the bottom right corner.
	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 UX and UY for the bottom left corner and UY for the bottom right corner and click OK. The default displacement value is taken to be zero.

APPLYING FORCES

Go to Main Menu.

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

Select the top node.

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

Select FX and enter 5000 as the Force/Moment value.

Click on OK.

The figure on the ANSYS Graphics window will look like the following.

Now the Modeling of the problem is done.

Go to ANSYS Main Menu>Solution>-Analysis Type->New Analysis.

Select static and click on OK.

Go to Solution>-Solve->Current LS.

Wait for ANSYS to solve the problem.

Click on OK and close the 'Information' window.

Listing the results.

Go to ANSYS Main Menu.

Click on General Postproc>List Results>Nodal Solution. The following window will come up.

Select DOF solution and All U's. Click on OK. The nodal displacements will be listed as follows.

Similarly you can list the stresses for each element by clicking Gen Postprcessing>List Results>Element Solution.

Now select LineElem Results. The following table will be listed.

You can also plot the displacements and stress.

Go to General Postproc>Plot Results>-Contour Plot->Element Solution. The following window will come up.

Select a stress to be plotted and click OK.  The output will be like this.