Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

## S3 2D Bracket

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:

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.

Geometry: The thickness of the bracket is 3.125 mm

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

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

Objective:
 Plot deformed shape Determine the principal stress and the von Mises stress. (Use the stress plots to determine these) Remodel the bracket without the fillet at the corner, and see how principal stress and von Mises stress change.

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 figure above.

 Go to the ANSYS Main Menu Preprocessor>Modeling>Create>Keypoints>On Working Plane Outline a part of the bracket as shown in the figure.

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

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

 Now go to Preprocessor>Modeling>Create>Lines>Line Fillet. The following window comes up. Select the two lines between which you want the fillet and click OK.

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

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

 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.

 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. 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:

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

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

 Fill in 2e11 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 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 Solid and select Quad 8 node 82. Click OK. Close the 'Element types' window. Click Preprocessor>Element Type>Add/Edit/Delete... In the 'Element Types' window that opens click on Options... The following window opens.

 Select Plane strs w/thk for K3 and click OK. 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. Now we need to define the thickness 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.

 Fill in the relevant values and click on OK. We have now defined the thickness of the element.

MESHING:

DIVIDING THE BRACKET INTO ELEMENTS:
 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. In the menu that comes up type 0.0125 in the field for 'Element edge length'.

 Click on OK. 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'. Now go to Preprocessor>Meshing>Mesh>Areas>Free. Select the area and click on OK in the "Mesh Areas" dialog box. Now the bracket is divided into Solid 8 node elements.

BOUNDARY CONDITIONS AND CONSTRAINTS:

APPLYING BOUNDARY CONDITIONS
 The bracket is fixed at the left edge. Go to Main Menu Preprocessor>Loads>Define Loads>Apply>Structural>Displacement>On Lines. Select the line on the left edge and click OK. The following window comes up:

 Select All DOF and click OK.

APPLYING FORCES
 Go to Main Menu Preprocessor>Loads>Define Loads>Apply>Structural>Pressure>On Line. Select the top line. Click on OK in the 'Apply PRES on lines' window. The following window will appear:

 Enter the value of the pressure as shown above. Click OK.

 The model should look like the one below.

 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 Postprcessing>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>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.