Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

 

S3 2D Bracket
Home Course Info Problems Test Problems Students Reference

Structural #3: Analysis of a Steel Bracket

 

Introduction: In this example you will learn to use the Solid 8 Node element in ANSYS.

Physical Problem: Structural analysis of the Steel Bracket shown in the figure. This is a typical bracket used to support bookshelves.

Problem Description:

 

bullet

We will model the bracket as a solid 8 node plane stress element. By a plane stress element we are assuming that there are no stresses in the thickness direction of the bracket. 

bullet

Geometry: The thickness of the bracket is 3.125 mm

bullet

Material: Assume the structure is made of steel with modulus of elasticity E=200 GPa.

bullet

Boundary conditions: The bracket is fixed at its left edge.

bullet

Loading: The bracket is loaded uniformly along its top surface. The load is 2625 N/meter.

bullet

Objective:
bullet

Plot deformed shape

bullet

Determine the principal stress and the von Mises stress. (Use the stress plots to determine these)

bullet

Remodel the bracket without the fillet at the corner, and see how principal stress and von Mises stress change.

bullet

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

bullet

Figure:

         

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.

bullet

Click on Run.

      

 

 

MODELING THE STRUCTURE:

 

bullet

Go to the ANSYS Utility Menu
bullet

Click Workplane>WP Settings

bullet

The following window comes up

 

 

 

bullet

Check the Cartesian and Grid Only buttons

bullet

Enter the values shown in the figure above.

 

bullet

Go to the ANSYS Main Menu Preprocessor>Modeling>Create>Keypoints>On Working Plane

bullet

Outline a part of the bracket as shown in the figure.

 

    

 

bullet

Note: To turn on the numbering: ANSYS Utility Menu>Plot Controls>Numbering...

 

bullet

Now create lines between keypoints, then create area inside. Go to Preprocessor>Modeling>Create>Areas>Arbitrary>By Lines.

 

 

 

bullet

Now go to Preprocessor>Modeling>Create>Lines>Line Fillet.

bullet

The following window comes up. Select the two lines between which you want the fillet and click OK.

 

 

 

bullet

In the box that comes up enter 0.025 for fillet radius and click OK.

 

 

 

bullet

Now go to Preprocessor>Modeling>Create>Areas>Arbitrary>By Lines to fill the fillet area.

 

 

 

bullet

Go to Preprocessor>Modeling>Create>Areas>Circles>Solid Circle and create the two circles with centre at the midpoint of the right edge and the bottom edge of the bracket and the diameter equal to the length of that edge.

 

 

 

Now go to Preprocessor>Modeling>Operate>Booleans>Add>Areas and select all areas you have created to make a single area.

 

 

 

bullet

Now go to Workplane>WP Settings and change the Snap Incr and grid settings to 0.00625.  We do this so that we can make the small inner circle whose radius is 0.00625 meter.

bullet

Go to Preprocessor>Modeling>Create>Areas>Circles>Solid Circle and create the a circle with center at the midpoint of the right edge of the horizontal rectangle and the radius equals to 0.00625. Do the same thing for the vertical rectangle.

 

 

 

Now go to Preprocessor>Modeling>Operate>Booleans>Subtract>Areas. First select the base area from which the smaller area will be subtracted. Say OK. Now select the smaller circles and say OK. the smaller circles will now be subtracted and the figure will look like this:

 

 

 

MATERIAL PROPERTIES:

 

bullet

Go to the ANSYS Main Menu>Preprocessor>Material Props>Material Models.  From this window, select Structural>Linear>Elastic>Isotropic.

 

 

 

bullet

Enter 1 for the Material Property Number and click OK. The following window comes up.

 

 

 

bullet

Fill in 2e11 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 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 Solid and select Quad 8 node 82. Click OK. Close the 'Element types' window.

bullet

Click Preprocessor>Element Type>Add/Edit/Delete... In the 'Element Types' window that opens click on Options... The following window opens.

 

 

 

bullet

Select Plane strs w/thk for K3 and click OK.

bullet

So now we have selected Element type 1 to be a Structural Solid 8 node element. The bracket will now be modeled as elements of this type.

bullet

Now we need to define the thickness 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

Fill in the relevant values and click on OK.

bullet

We have now defined the thickness of the element.

 

MESHING:

 

bullet

DIVIDING THE BRACKET INTO ELEMENTS:
bullet

Go to Preprocessor>Meshing>Size Controls>Manual Size>Lines>Picked Lines. Pick all the lines on the outer boundary of the figure and click OK.

bullet

In the menu that comes up type 0.0125 in the field for 'Element edge length'.

 

 

 

bullet

Click on OK.

bullet

Repeat the process to divide the lines forming the small inner circle. In this case enter 0.001 in the field for 'Element edge length'.

bullet

Now go to Preprocessor>Meshing>Mesh>Areas>Free.

bullet

Select the area and click on OK in the "Mesh Areas" dialog box.

bullet

Now the bracket is divided into Solid 8 node elements.

 

BOUNDARY CONDITIONS AND CONSTRAINTS:

 

bullet

APPLYING BOUNDARY CONDITIONS
bullet

The bracket is fixed at the left edge.

bullet

Go to Main Menu Preprocessor>Loads>Define Loads>Apply>Structural>Displacement>On Lines.

bullet

Select the line on the left edge and click OK. The following window comes up:

 

 

 

bullet

Select All DOF and click OK.

 

bullet

APPLYING FORCES
bullet

Go to Main Menu Preprocessor>Loads>Define Loads>Apply>Structural>Pressure>On Line.

bullet

Select the top line.

bullet

Click on OK in the 'Apply PRES on lines' window. The following window will appear:

 

 

 

bullet

Enter the value of the pressure as shown above.

bullet

Click OK.

 

bullet

The model should look like the one below.

 

 

 

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

 

 

 

MODIFICATIONS:

 

bullet

You can also plot the displacements and stress.

bullet

Go to General Postprocessing>Plot Results>Deformed shape. The following window comes up.

 

 

 

Select Def+undeformed and click OK. The output will be like the figure below.

 

    

 

Select a stress (SEQV) 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.