Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

## S4 3D Truss Structure

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:

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 1.56e-3 sq meter.

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

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

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.

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

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

Figure:

 IMPORTANT: Convert all dimensions and forces into SI units.

STARTING ANSYS

 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 an appropriate job name. Click on Run.

MODELING THE STRUCTURE

 Go to ANSYS Utility Menu. Click on Workplane>Change Active CS to..>Global Cartesian. Go to the ANSYS Main Menu.
 Click Preprocessor>Modeling>Create>Keypoints>In active CS The following window comes up

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.

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

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

Now create lines connecting the keypoints
 Click on Preprocessor>Modeling>Create>Lines>Lines>In Active Coord. Pick the endpoints of each element to create the lines.  Rotate the figure for more accessible views.

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

MATERIAL PROPERTIES

 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.

 Double click Isotropic for Material Model 1.

 Fill in 7.5e10 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 elements of the structure.

ELEMENT PROPERTIES:

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 3D spar. Click OK. Close the 'Element types' window. 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. 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 1.56e-3 for cross sectional area and click on OK. We have now defined the cross sectional area of the link element.

MESHING:

 DIVIDING THE TOWER INTO ELEMENTS: 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).

BOUNDARY CONDITIONS AND CONSTRAINTS

APPLYING BOUNDARY CONDITIONS
 The tower is constrained in the X, Y and Z directions at the four bottom corners. 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, UY, UZ and click OK.

APPLYING FORCES
 First find the components of the force along the Y and Z directions 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. Enter the value of the Z-component of the force. Repeat the procedure to apply the Y-component of force.

 Now the Modeling of the problem is done

SOLUTION

 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

POST-PROCESSING

 Listing the results Go to ANSYS Main Menu Click on General Postprocessing>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 General Postprocessing>List Results>Element Solution. Now select LineElem Results.

MODIFICATIONS:

 You can also plot the displacements and stress. Go to General Postprocessing>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.