Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

 

S4 3D Truss Structure
Home Course Info Problems Test Problems Students Reference

Structural #4: Analysis of a 3-D truss structure

 

Introduction: In this example you will learn to use the 3-D Truss element in ANSYS.

Physical Problem: Analysis of the 3D truss structure shown in the figure below.

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 1.56e-3 sq meter.

bullet

Material: Assume the structure is made of aluminum with modulus of elasticity E=75 GPa.

bullet

Boundary conditions: The structure is constrained in the X, Y and Z directions at the bottom three corners.

bullet

Loading: The tower is loaded at the top tip. The load is in the YZ plane and makes an angle of 75 with the negative Y axis direction. The load value is 2500 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

Give three examples where similar 3D trusses are used in practice. Model one of them (with reasonable assumptions of dimensions, material properties and loading) using ANSYS. You don't have to solve it. You can do so to check whether your assumptions were reasonable!!

bullet

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

bullet

Figure:

                

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 an appropriate job name.

bullet

Click on Run.

      


MODELING THE STRUCTURE

bullet

Go to ANSYS Utility Menu. Click on Workplane>Change Active CS to..>Global Cartesian.

bullet

Go to the ANSYS Main Menu.

bullet

Click Preprocessor>Modeling>Create>Keypoints>In active CS

bullet

The following window comes up

     

bullet

Fill in the keypoint number (1,2,3...) and the coordinates. Make sure you get the correct coordinates from the figure. Create all the 10 keypoints. Make sure the numbering of your keypoints matches the numbering of the joints in the figure.

bullet

If you cannot see the grid then go to Utility Menu>Display Working Plane

bullet

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

bullet

Now create lines connecting the keypoints
bullet

Click on Preprocessor>Modeling>Create>Lines>Lines>In Active Coord.

bullet

Pick the endpoints of each element to create the lines.  Rotate the figure for more accessible views.

   

bullet

You can use the Utility Menu>PlotCtrls>Pan Zoom Rotate window to rotate the model and see its 3D nature.

 

MATERIAL PROPERTIES

bullet

Go to the ANSYS Main Menu

bullet

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.

 

           

bullet

Double click Isotropic for Material Model 1.

              

bullet

Fill in 7.5e10 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 elements of the structure.

 

ELEMENT PROPERTIES:

bullet

SELECTING ELEMENT TYPE:
bullet

Click Preprocessor>Element Type>Add/Edit/Delete... 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 3D spar. Click OK. Close the 'Element types' window.

bullet

So now we have selected Element type 1 to be a structural Link- 3D spar (cable) 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 1.56e-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 Controls>Manual Size>Lines>All Lines. In the menu that comes up type 1 in the field for 'Number of element divisions'.

 

 

bullet

Click on OK.

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, Y and Z directions at the four bottom corners.

bullet

Go to Main Menu

bullet

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, UY, UZ and click OK.

 

bullet

APPLYING FORCES
bullet

First find the components of the force along the Y and Z directions

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

Enter the value of the Z-component of the force.

bullet

Repeat the procedure to apply the Y-component of force.

 

 

    

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 Postprocessing>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 General Postprocessing>List Results>Element Solution. Now select LineElem Results.

 

MODIFICATIONS:

bullet

You can also plot the displacements and stress.

bullet

Go to General Postprocessing>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.