Interactive Step-by-Step Solution

The procedure for entering the ANSYS program is to be discussed in the class.

Preprocessing

A typical ANSYS analysis begins with preprocessing, where you provide data such as the geometry, materials, and the element types to the program.

Specify title

Although the step is not required for an analysis, it is recommended that you make it part of all your analysis. The title (maximum of 72 characters) will appear on all graphics display and will be included on the solution output.

Utility Menu:

  1. File
  2. Change Title
  3. Enter the title "Beam"
  4. OK to define the title and close the dialog box


Set Preferences

The "Preferences" dialog box allows you to choose the desired engineering discipline for context filtering of menu choices. By default, menu choices for all disciplines are shown, with non applicable choices "dimmed" based on a set of element types in your model. If you prefer not to see the dimmed choices at all, you should turn on filtering. For example, turning on structural filtering here completely suppresses all thermal, electromagnetic, and fluid menu topics.

Main Menu:

  1. Preferences
  2. Turn on structural filtering
  3. OK to apply filtering and close the dialog box

Define element type and options

In any analysis, you need to select from a library of element types and define the appropriate ones for your analysis. The element type determines, among other things, the degree-of-freedom set (displacements and/or rotations, temperatures, etc.) the characteristic shape of the element (line,quadriletral, brick, etc.) and whether the element lies in 2-D space or 3-D space. Many element types also have additional element options to specify such things as element behavior and assumptions, element result printout options, etc.

For this analysis, we will use only one element type, 2D Beam (BEAM3), which is a 2-D structural beam element.

Main Menu:

  1. Preprocessor
  2. Element Type
  3. Add/Edit/Delete
  4. Add an element type
  5. Beam family of elements
  6. Choose the 2D elastic
  7. OK to apply the element type and close the dialog box
  8. Options for BEAM3
  9. Choose "Include output"
  10. OK to close "BEAM3 element type option" dialog box
  11. Close to close Element type dialog box



Define real constants

For element types whose geometry is not fully defined by its node locations, real constants provide the additional geometry information. Typical real constants include shell thicknesses for shell elements and cross-sectional area for bar elements.

Main Menu:

  1. Preprocessor
  2. Real Constants
  3. Add a real constant set
  4. OK for BEAM3
  5. Enter1 for AREA
  6. Enter 1 for IZZ
  7. Enter 1 for HEIGHT
  8. OK to define real constant and close the dialog box
  9. Close to close Real constant dialog box


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 is the only material property that needs 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. OK to close the dialog box


Toolbar: SAVE_DB

Define Nodes

There are two ways to create the model namely solid modeling and direct generation. The latter is used here. (Node 1 is at the Global origin)

Main Menu:

  1. Preprocessor
  2. Create
  3. Nodes
  4. In Active CS
  5. Apply to create node 1 at the global origin
  6. Enter 5 for Node number
  7. Enter 8 for X and 0 for Y
  8. OK to create node 5 and close the dialog box
  9. Turn on node numbering (Utility Menu: PlotCtrls >Numbering > Node numbers ON)
  10. Plot nodes (Utility Menu: Plot > Nodes)
  11. Preprocessor
  12. Create
  13. Nodes
  14. Fill between Nds
  15. Choose Node 1 and 5
  16. OK
  17. OK to accept the default values and to close the dialog box



Create Elements

Main Menu:

  1. Preprocessor
  2. Create
  3. Element
  4. Element Attributes (Before creating elements you need to specify element attributes. For this problem since we have only one element type, real constant set and material property set, the default values are correct)
  5. OK to accept the default values
  6. Thru Nodes
  7. Pick node 1 and 2
  8. OK to create element 1

Copy Element 1

  1. Preprocessor
  2. Copy
  3. Auto Numbered
  4. Pick the element you just created (Element 1)
  5. OK
  6. Enter 4 for the total number of copies (Note that original is included in the number of copies)
  7. Enter 1 for NINC
  8. OK to copy the elements


Toolbar: SAVE_DB

Solution

Apply displacement constraints

Main Menu:

  1. Solution
  2. Apply
  3. Displacement
  4. On Nodes
  5. Pick Node 1
  6. OK
  7. Choose ALL DOF
  8. OK to apply constraints


Apply force

Main Menu:

  1. Solution
  2. Apply
  3. Force/Moment
  4. On Nodes
  5. Pick Node 5
  6. OK
  7. Choose FY
  8. Enter -50

Solve

Main Menu:

  1. Solution
  2. Current LS
  3. Review the information in the status window,
    then pick File Close to close the window
  4. OK to begin the solution
  5. Close the Information window when solution is done

Postprocessing

Postprocessing is where you review the results of the analysis through graphics display and tabular listings The general postprocessor (POST!) is used to review results at one substep (time step) over the entire model. The time history postprocessor (POST26) is used to review results at specific points in the model over all time steps

Enter the general postprocessor and read in the rsults.

List the displacements

Main Menu:

  1. General Postproc
  2. List results
  3. Nodal Solution
  4. Choose DOF solution
  5. Choose ALL DOFs DOF
  6. OK to list the results


List the stresses

Main Menu:

  1. General Postprocessor
  2. Element Table
  3. Define Element Table
  4. Add to define Element Table Data
  5. Enter a name (Optional)
  6. Choose By sequence num
  7. Choose SMISC,
  8. Enter 2
  9. Apply to define first element table item
  10. Repeat 6 -9 and in step 8 enter 8,1,7,6,12
  11. OK to close the Define Additional element Table Items dialog box
  12. Close to close the dialog box


List the stresses/moments

Main Menu:

  1. General Postprocessor
  2. Element Table
  3. List Element Table
  4. Choose SMIS6 (Moment at I)
  5. OK to list the results


EMA 405's Homepage
WebMaster:
Last Update: 10/1/1996