We will model the object using solid Tetrahedral 10 node element.

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

Boundary conditions: The object is fixed around the inner surface of the hole.

Loading: The object is loaded uniformly (1000 N/cm²) along the top surface of the extended beam.

Objective:

	To plot deformed shape.
	To determine the principal stress and the von Mises stress. (Use the stress plots to determine these. Do not print the stress list)
	What is the maximum load the object can take. Clearly mention the yield stress that you have assumed for steel. Also assume factor of safety of 1.25.

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

Figure:

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.

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.

We will model the object as four seperate volumes and then add them up.

Go to the ANSYS Main Menu Preprocessor>Modeling>Create>Volumes>Blocks>By 2 corners & Z.

Select the two corners and enter the depth in the "depth " field so as to create the first rectangular part of the figure. The isometric view looks like the figure below.

Now create two cylinders representing the holes. Use the Preprocessor>Modeling>Create>Volumes>Cylinder>Solid Cylinder, and select the center and the radius and the depth of the cylinder.

Now subtract these two cylinders from the main rectangular block. Use the Preprocessor>Modeling >Operate>Booleans>Subtract>Volumes menu. Select the base area first (the rectangular block). Then select the volumes to be subtracted (the two cylinders). Click OK. The isometric view of the figure looks like the figure below.

Now we will create the extended portion of the object.

Go to Utility Menu>WorkPlane>Offset Workplane by Increments. The following window will come up.

Now offset the workplane in the +Z direction by an amount equal to the thickness of the previous rectangular block we made. This thickness is 0.01 m which is 4 times of the snap (0.0025). So we set the 'snaps' to 4 and click on the +Z once. The workplane looks like this from the left side view.

Now offset the workplane further along the +Z axis by an amount equal to the length of the extended block (0.06 meter).

So the workplane looks like this from the left side view.

Now create another block (block 3) by

Preprocessor>Modeling>Create>Volumes>Blocks>By 2 corners & Z.

We make this block separately so that we can create the required fillet easily.

Now create the block 4.

Now glue parts together. Go to Preprocessor>Modeling>Operate>Booleans>Glue>Volumes.

In the window that comes up click Pick All and click OK.

Now we will create the fillet. Go to Preprocessor>Modeling>Create>Lines>Line Fillet
Select two lines on the "L" shape to create Fillet in between. Do this for both top and bottom sides. See the Figure below:

Now create two lines. Go to Preprocessor>Modeling>Create>Lines>Lines>Straight Line.
Pick keypoints to create lines as shown in the figure below:

Now, create areas to close the fillet.
Go to Preprocessor>Modeling>Create>Areas>Arbitrary>By Lines
Create 3 areas of the fillet (Top, Bottom and Front) as shown in Figure below

Two more areas are needed to define the fillet volume.
Go to Operate>Booleans>Divide>Area by Line.
Select the inner area of the "L" shape click OK.

Then select the line as shown to divide the area into two pieces and click OK

Repeat the dividing areas steps for the other inner area of the "L" shape

Now create the volume within the fillet by Preprocessor>Modeling>Create>Volumes>Arbitrary>By Areas. Select the areas which enclose the fillet volume and click OK. The final model will look as follows.

Now go to Preprocessor>Modeling>Operate>Booleans>Add>Volumes. Click on Pick All. So now we have added all the volumes into a single volume.

Go to the ANSYS Main Menu

Click Preprocessor>Material Properties>Material Models.  In the window that comes up, select Structural>Linear>Elastic>Isotropic.

Material model 1 is automatically selected. 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.

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 Tet 10node 92. Click OK. Close the 'Element types' window.

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 0.005 in the field for 'Element edge length'.

Click on OK.

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

Click Pick All in the "Mesh Areas" dialog box. The meshed model looks like this.

Now the object is divided into Solid Tetrahedral elements.

APPLYING BOUNDARY CONDITIONS

The object is fixed around the inner faces of the holes.

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

Select the areas on the inner surface of the holes and click OK. The following window comes up.

Select All DOF and click OK. The holes will look like the following after zooming in.

APPLYING FORCES

Go to the Main Menu

Click on Preprocessor>Loads>Define Loads>Apply>Structural>Pressure>On Area.

Select the top surface of the cantilever like arm.

Click on OK in the 'Apply PRES on areas' 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.

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.