Truss Bending Tutorial

Truss Bending Analysis:

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

Physical Problem: A truss structure deflects under load.

Problem Description:

· The truss structure is made up of two-force members. Each two force member only experiences loading in the axial direction.

· Units: Use S.I. units ONLY

· Geometry: the cross sections of each of the truss members is 6.25e-6 (m²).

· Material: Assume the structure is made of aluminum with modulus of elasticity E=70e9 (N/m²) and Poisson ratio 0.33.

· Boundary conditions: The structure is constrained along X and Y directions at the left top end, and along the X direction at the bottom left corner.

· Loading: The structure is loaded at the bottom right corner. with a vertical force acting downward with magnitude 5 N.

· Objective:

o To determine the force in member AB.

o To determine the downward deflection at G

· Figure:

The horizontal and vertical truss members are all .1m long.

STARTING ANSYS

ANSYS is found on the start menu under Programs -> Math and Stats.

MODELING THE STRUCTURE

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. This makes each grid's dimensions 10 cm by 10 cm.

Go to the ANSYS Main Menu

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

Another way of picking Keypoints is by manually entering the coordinates. This is more useful for 3d structures, but it is worth noting here anyway...
o        Click Preprocessor>Modeling>Create>Keypoints>In Active CS

o        Choose a number for each Keypoint, say 1,2,3…

o        enter coordinates for each Keypoint:

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

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 and the following window comes up.

Fill in 70e9 for the Young's modulus and 0.33 for minor Poisson's Ratio (PRXY). Click OK.
Now the material 1 has the properties defined in the above table.

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.

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-6 for cross sectional area of Element Type Reference number 1 and click on OK.
While not needed for this specific problem, if you wanted to add different cross sectional areas to your structure you have to define multiple real constants.
- Go to Preprocessor>Real Constants
- Click add and enter the cross section area the same way as before. Make sure the Real Constant Set No. box is incrementing by 1 each time you add a real constant. The next section will show you how to set each element's cross section area

MESHING:

DIVIDING THE STRUCTURE 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 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).
This is not necessary for this problem, but if you specified multiple real constants above (if your structure has multiple cross sectional areas) you have to tell ANSYS which elements have which area:
- Go to Preprocessor>Meshing>Mesh Attributes>Default Attribs
- Here you can choose which real constant to use when specifying the mesh. For example...choose element 2
- Now go to Preprocessor>Meshing>Mesh>lines
- Select all the lines you want to have the cross section of real constant 2 and click on OK in the "Mesh Lines" dialog box.
- Repeat this process for all of your real constants

BOUNDARY CONDITIONS AND CONSTRAINTS

APPLYING BOUNDARY CONDITIONS
- The structure is constrained along X and Y directions at the left top end, and along X direction at the bottom left 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 top left corner. The default displacement value is taken to be zero
Repeat this procedure for the bottom left corner but only constrain UX.
APPLYING FORCES
Go to Main Menu.
Click on Preprocessor>Loads>Define Loads>Apply>Structural>Forces/Moment>On Nodes.
Select the bottom right node.
Click on OK in the 'Apply F/M on Nodes' window. The following window will appear.

Select FY and enter -5 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.

SOLUTION

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.
To determine the Force in member AB goto General Postproc>List Results>Element Solution and click on LineElem>Structual ELEM and click OK:

The output displays the forces in each element. If you followed the numbering above, element 2 corresponds to member AB:

If you used a different numbering scheme you can output the element numbers onto the main screen by going to the file menu and selecting PlotCtrls>Numbering and selecting Element numbers:

To determine the the deflection of point G goto General Postproc>Query Results>Subgrid Solution and select DOF Solution and UY.

When you click ok you can pick the node corresponding to point G. The displacement will then be displayed next to the node: