Define element type and options

Note: It is assumed that you are able to take the steps prior to this on your own. See beam problem or bar problem for details.

For this analysis, we will use only one element type, PLANE42 which is a 2-D structural solid element can be used either as a plain stress or plain strain element. It is a 4 node Quad but can be used as a CST (constant strain triangle) as well.

Main Menu:

  1. Preprocessor
  2. Element Type
  3. Add/Edit/Delete
  4. Add an element type
  5. Solid family of elements
  6. Choose "Quad 4node 42"
  7. OK to apply the element type and close the dialog box
  8. Options for PLANE42
  9. Make sure that Element behavior is Plane stress
  10. OK to close "PLANE42 element type option" dialog box
  11. Close to close Element type dialog box


Define real constants

No real constant is needed for PLANE42 element.

Define material Properties

Material properties are constitutive properties of material such as modulus of elasticity density and are independent of geometry.

For this analysis, Young's modulus of elasticity and Poisson's ratios are the only material property that need to be entered.

Main menu:

  1. Preprocessor
  2. Material Props
  3. Isotropic
  4. OK since we are defining material 1
  5. Enter 30e6 for EX
  6. Enter 0.3 for Poisson's ratio (NUXY)
  7. OK to close the dialog box


Solid Modeling

Create the Area:

  1. Preprocessor
  2. Create
  3. Rectangle
  4. By Dimensions
  5. Enter 1 for X2 (if you don't enter coordinate values ANSYS takes 0 as default)
  6. Enter 1 for Y2
  7. OK to close the dialog box and to create the area



Your graphics screen should look something like the following.


Meshing the area

  1. Preprocessor
  2. Shape & Size
  3. For All Lines
  4. Enter 1 for NDIV
  5. OK to close the dialog box

    Note: Before meshing you need to specify what kind of element you want to use (i.e. CST or 4node Quad or mixture of both). To do that:
    1. Preprocessor
    2. Shape & Size
    3. Element shape ….
    4. Turn on "Tri Only | Tetra"
    5. OK to apply the settings and close the dialog box
  6. Mesh
  7. Areas
  8. Pick the area you just created
  9. OK to mesh the area

Your graphics window should look like something like following

If you plot your nodes you should get the following plot. (turn node numbering on )

Set the boundary conditions

Apply X and Y direction constraints to node 1 and Y direction constraint to node 2. Apply -300 lb load in the Y direction to the node 3 and 4. This process is the same (for now) as when you were dealing with bar and beam elements. Compare you graphics display with the following figure.


Solution

  1. Solution
  2. Current LS
  3. OK to start solution
  4. YES to ignore the warning

Postprocessing

Animate the deformed shape

  1. PlotCtrls
  2. Animate
  3. Deformed shape

Plot the Y direction displacement

  1. General Postproc
  2. Plot Results
  3. Nodal Solu …..
  4. DOF solution
  5. UY
  6. OK


Plot stresses

  1. General Postproc
  2. Plot Results
  3. Nodal Solu …..
  4. Stresses
  5. Y-direction SY
  6. OK