ANSYS Lab

Tutorial (40 pts.) ANALYSIS OF A TRUSS CONSIDERING SYMMETRY OF THE

PROBLEM You need to submit the following items for this tutorial:

1- Show the deformed structure of the truss (screen snapshot is OK). Write down the

displacement of each node in x and y directions.

2- Create the snapshot of the window that lists stress on each member.

3- Find the reaction at support 1 (or 4).

Consider the steel truss structure shown in Figure below, which possesses symmetry in geometry

and loading. Node and element numbers are also shown in this figure. Element 3 has a cross-

sectional

area of A=20 in2 while the other elements have A=10 in2. The elastic modulus for all of

the elements is E= 30 x 106 psi. Due to the symmetry condition, only half the geometry is

modeled with appropriate boundary conditions, i.e., the x-displacement at nodes 2 and 3 is zero

and the applied force at node 2 is halved. Also, for the element located along the symmetry line,

one half of the cross-sectional area is used.

1! !

STEPS:

PREPROCESSING:

Go to utility menu>File and select “Change Jobname …” and enter “Lab 4” and then click OK.

If you want to change the working directory, go to utility menu>File and select “Change Directory” and specify the new directory in the opened window.

1) Select the element type

Main Menu > Preprocessor > Element Type > Add/Edit/Delete

Click on Add,

Select Link and 3D finit stn 180 as shown below, click ok, close

2! !

2) Specify the cross section.

To specify the cross section, we include two methods. Method 1 is for ANSYS 16.2 and method 2 is for ANSYS 17.1.

Method 1 (ANSYS 16.2):

Main Menu > Preprocessor > Real Constant > Add/Edit/Delete

Click add, highlight type 1 link 180; click ok; enter 10 for area; click ok; close.

Method 2 (ANSYS 17.1):

Main Menu > Preprocessor > Sections> Link> Add

Enter 1 for the ID. Click OK.

In the new window, enter “sec1” for section name, and enter 10 for link area. And then click OK.

3! !

3) Specify the material

Main Menu > Preprocessor > Material Props > Material Models

Successively click linear-elastic-isotropic, and enter values for EX = 30e6 and PRXY = 0.3, click ok, Material > exit

4) Create Nodes

Main Menu > Preprocessor > Modeling > Create > Nodes > In Active CS

Create 3 nodes with (X, Y) coordinates as follows 1 (0, 0), 2 (96, 0) and 3 (96, 72) and set Z coordinate to 0.

For Creating, enter node number and location (X,Y), click apply for creating node 1 and 2 and while creating the last node i.e. 3 just click ok instead of apply.

4! !

5) Create elements from the nodes.

Main Menu > Preprocessor > Modeling >Create > Elements > Auto Numbered > Thru Nodes

We will create 3 elements.

Element 1 is defined by nodes 1 and 3. Similarly, elements 2 and 3 are defined by nodes (1-2) and (2-3), respectively.

In pick menu pick nodes 1 and 3, click apply to create element 1, Repeat this procedure for creating element 2 and 3. If you click on OK, you have to reopen this window. For the last element, you may click on OK to close the selection window.

5! !

SOLUTION

1) Apply displacement constraint

Main Menu > Solution > Define Loads > Apply > Structural > Displacement on nodes

Pick node 1, click apply, then highlight UY in the new window and then click on OK.

Similarly pick node 2 and 3 click on UY to remove highlight and click on UX to highlight.

Click ok.

6! !

7! !

2) Apply force.

Main Menu > Solution > Define Loads > Apply > Structural > Force/Moment > On Nodes

Pick node 2 and apply FY = -10000; click ok.

3) Solve

Main Menu > Solution > Solve > Current LS

Click ok on ansys status report window and wait until ansys responds with ‘Solution is done’

8! !

POSTPROCESSING

1) List displacement results at nodes

Main Menu > General PostProc > List Results > Nodal Solution

Click on DOF solution and Y-Component of displacement, click ok.

The list appears with the values for the y-displacement at nodes 2 and 3 as -0.19200E-01 and - 0.16800E-01, respectively.

2) Review stress values in the element table

Main Menu > General PostProc > Element Table > Define Table

Click Add; Enter label ELSTRS for element stress; in the left list scroll down to select “by sequence number” and select LS in the right list. Finally type LS,1 in the last text field. Click ok.

9! !

Main Menu > General PostProc > Element Table > List Elem Table

In the element table dialog box, Highlight ELSTRS; click ok.

Below list appears.

• To see the element numbers on the truss, go to “plot” in the utility menu and select “elements”. Then go to “plotCtrls” and click on “Numbering …”. In the “plot Numbering Controls” window, select “Element Numbers” in the drop down menue for Elem/Attrib numbering. Now you can see the element numbers on each element.

• To find the reaction at the node 1 (the support), use:

Main Menu > General PostProc > List Results > Reaction Solu

Then select “All items” in the new window and click on OK.

• To show the deformed structure, use:

Main Menu > General PostProc > Plot Results > Deformed Shape

And select “Def+Undeformed” and select OK.

• Click on “Save_DB” in the toolbar menu.

10! !

Lab problem (60 pts.) A space truss is shown below. The crate has a weight of 150 lb. Use the same materials as the one in the tutorial. Use A=10 in2 for all links. The links that attach points A and B to the wall are just to show which components of the displacements are constrained at these points. For example, point A is constrained in y and x directions. When you create the model, ignore these links, as such point A and B are on the wall.

You need to submit the following items for this assignment:

1- Show the deformed structure of the truss (snapshot of the screen is OK). Determine the displacement vector of joint C.

2- Create the snapshot of the window that lists stress on each member. 3- Find the reactions in supports A, B, and D in the constrained directions.