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.

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

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.

	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.

	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.

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

	You can also plot the displacements and stress.
	Go to General Postprocessing>Plot Results>Deformed shape. The following window comes up.