Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

 

S6 3D Solid
Home Course Info Problems Test Problems Students Reference

Structural #6: Analysis of a 3D solid object

 

Introduction: In this example you will learn to use the Solid element in ANSYS. Also you will learn some basic 3D modeling.

Physical Problem: See figure.

Problem Description:

 

bullet

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

bullet

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

bullet

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

bullet

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

bullet

Objective:
bullet

To plot deformed shape.

bullet

To determine the principal stress and the von Mises stress. (Use the stress plots to determine these. Do not print the stress list)

bullet

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.

bullet

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

bullet

Figure:

             

    

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

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

bullet

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

bullet

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.

 

 

bullet

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.

bullet

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.

 

 

bullet

Now we will create the extended portion of the object.

bullet

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

 

                     

 

bullet

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 create the first extended rectangular block. The figure will look like the one below in isometric view.

 

 

bullet

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

bullet

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

 

 

bullet

Now create another block (block 3) by

bullet

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

bullet

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

 

bullet

Now create the block 4.

 

           

 

bullet

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

bullet

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

bullet

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:

 

 

bullet

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

 

 

bullet

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

 

 

bullet

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.

 

 

bullet

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

 

 

bullet

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

bullet

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.

          

bullet

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.

 

MATERIAL PROPERTIES:

 

bullet

Go to the ANSYS Main Menu

bullet

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

 

 

bullet

Material model 1 is automatically selected. 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 Tet 10node 92. Click OK. Close the 'Element types' window.

 

MESHING:

 

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 0.005 in the field for 'Element edge length'.

 

 

bullet

Click on OK.

bullet

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

bullet

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

 

 

bullet

Now the object is divided into Solid Tetrahedral elements.

 

BOUNDARY CONDITIONS AND CONSTRAINTS:

 

bullet

APPLYING BOUNDARY CONDITIONS

bullet

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

bullet

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

bullet

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

 

 

bullet

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

 

 

bullet

APPLYING FORCES

bullet

Go to the Main Menu

bullet

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

bullet

Select the top surface of the cantilever like arm.

bullet

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

 

You can also plot the displacements and stress.

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

 

 

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

 

 

 

 

Select a stress (say von Mises) 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.