Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

 

S1 2D Truss Structure
Home Course Info Problems Test Problems Students Reference

Structural #1: Analysis of a power transmission tower

 

Introduction: In this example you will learn to use the 2-D Truss element in ANSYS.

Physical Problem: A power transmission tower is a common example of a structure that is made up of only truss members. These towers are actually 3-D structures, but for the sake of simplicity we will take a cross-sectional face of the tower. The tower is mainly subjected to loading in the vertical direction due to the weight of the cables. Also it is subjected to forces due to wind. In this example we will consider only loading due to the weight of the cables, which is in the vertical direction.

Problem Description:        

bullet

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. 

bullet

Units: Use S.I. units ONLY

bullet

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

bullet

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

bullet

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.

bullet

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

bullet

Objective:
bullet

To determine deflection at each joint.

bullet

To determine stress in each member.

bullet

To determine reaction forces at the base.

 

bullet

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

bullet

Figure:
bullet

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

 

 

bullet

IMPORTANT: Convert all dimensions and forces into SI units.

 

STARTING ANSYS

bullet

Click on ANSYS 6.1 in the programs menu.

bullet

Select Interactive.

bullet

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.

bullet

Click on Run.

 

 

MODELING THE STRUCTURE

 

bullet

Go to the ANSYS Utility Menu
bullet

Click Workplane>WP Settings

bullet

The following window comes up

 

 

bullet

Check the Cartesian and Grid Only buttons

bullet

Enter the values shown in the figure above.

bullet

Go to the ANSYS Main Menu

 

   

 

bullet

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

bullet

The following window comes up

 

 

bullet

Now we will pick the end points of the trusses.
bullet

Select the keypoints on the workplane grid. Your points should look like this.

bullet

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

 

 

bullet

Now create lines connecting the keypoints
bullet

Click on Preprocessor>-Modeling->Create>-Lines->Lines>Straight Line

bullet

Create lines by picking keypoints to make the figure shown below

 

 

 

MATERIAL PROPERTIES

 

bullet

Go to the ANSYS Main Menu

bullet

Click Preprocessor>Material Props>Material Models.

bullet

In the window that comes up which is shown below, for Material Model 1, choose Structural>Linear>Elastic>Isotropic.

 

 

bullet

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

 

          

 

bullet

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

bullet

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

 

ELEMENT PROPERTIES

 

bullet

SELECTING ELEMENT TYPE:

bullet

Click Preprocessor>Element Type>Add/Edit/Delete...

bullet

In the 'Element Types' window that opens click on Add... The following window opens.

 

 

bullet

Type 1 in the Element type reference number

bullet

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

bullet

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.

bullet

Now we need to define the cross sectional area for this element.

bullet

Go to Preprocessor>Real Constants

bullet

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

bullet

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

 

 

bullet

Type 6.25e-3 for cross sectional area and click on OK.

bullet

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

 

MESHING:

 

bullet

DIVIDING THE TOWER INTO ELEMENTS:

bullet

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

bullet

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.

 

 

bullet

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

bullet

Now go to Preprocessor>-Meshing->Mesh>lines

bullet

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

bullet

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

 

BOUNDARY CONDITIONS AND CONSTRAINTS

 

bullet

APPLYING BOUNDARY CONDITIONS
bullet

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.

bullet

Go to Main Menu. Click on Preprocessor>Loads>Define Loads>Apply>Structural>Displacement>On Keypoints

bullet

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

 

 

bullet

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.

bullet

APPLYING FORCES

bullet

Go to Main Menu.

bullet

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

bullet

Select the top node.

bullet

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

 

 

bullet

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

bullet

Click on OK.

bullet

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

 

bullet

Now the Modeling of the problem is done.

 

SOLUTION

 

bullet

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

bullet

Select static and click on OK.

bullet

Go to Solution>-Solve->Current LS.

bullet

Wait for ANSYS to solve the problem.

bullet

Click on OK and close the 'Information' window.

 

POST-PROCESSING

 

bullet

Listing the results.

bullet

Go to ANSYS Main Menu.

bullet

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

 

 

bullet

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

 

 

bullet

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

bullet

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

 

 

MODIFICATION

 

bullet

You can also plot the displacements and stress.

bullet

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

 

 

bullet

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

 

 

 

Home Course Info Problems Test Problems Students Reference
Send mail to the Teaching Staff with questions or comments about this web site.