Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

## S2 2D Beam Structure

Structural #2: Analysis 2-D Beam structure

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

Physical Problem: Structural analysis of the frame shown below.

Problem Description:

The structure is made up of beams. You may recall that a beam is a structural element whose length is very large compared to the other two dimensions.

Units: Use S.I. units ONLY

Geometry: The members have a annular cross-section. The cross sections (A) of each of the truss members is 5.5e-3 sq meter. The polar radius of gyration (R) is 5.5e-2 meter. (hint: Use the values of A and R to find Izz then find the value of the outer diameter (The beam height))

Material: Assume the structure is made of steel with modulus of elasticity E=210 GPa.

Boundary conditions:  All the DOFs are constrained at the bottom end, i.e. the bottom end is a built-in end.

Objective:
 To determine deflections at the points of application of load. To determine the maximum stress in the structure. Also determine the maximum possible load the frame can take. Look up for the value of yield stress for steel. Assume a factor of safety of 1.25.

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. Click on Run.

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 above.

 Go to the ANSYS Main Menu Click Preprocessor>Modeling>Create>Keypoints>On Working Plane The following window comes up

Now we will pick the end points of the trusses.
 5 meters is now 1 X 5 units, since each cell in the grid is 1 unit across, 5 meters is 5 cells wide. Using this conversion 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.

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 choose Structural>Linear>Elastic>Isotropic. The following window will appear.

 Double Click Isotropic. The following window comes up.

 Fill in 2.1e11 for the Young's modulus and 0.3 for Poisson's Ratio. Click OK Now the material 1 has the properties defined in the above table. We will use this material for 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 Beam and select 2D elastic. Click OK. Close the 'Element types' window. So now we have selected Element type 1 to be a structural Beam- 2D elastic element. The trusses will be modeled as elements of type 1, i.e. structural beam element. This finishes the selection of element type. Now we need to define the cross sectional area, the second moment of inertia etc. 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 in 5.5e-3 for cross sectional area, calculate Izz from the value of the cross-sectional area and polar radius of gyration and enter it. Also calculate and enter the height and click on OK. The height of the beam is required to calculate the maximum stress, which will be at the top surface of the beam. We have now defined the geometric properties of the beam element.

MESHING:

DIVIDING THE STRUCTURE 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 DOFs at the bottom node. 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 All DOF and click OK.

APPLYING FORCES

 Go to Main Menu Click on Preprocessor>Loads>Define Loads>Apply>Forces/Moment>On Nodes. Select the top right node and the top left node. Click on OK in the 'Apply F/M on Nodes' window. The following window will appear. Enter the value of the force.

The figure looks like this now.

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

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 Gen Postprocessing>List Results>Element Solution. Now select LineElem Results. The following table will be listed.

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.