MET 415 - FEA Applications I

Prof. Dave Johnson, psuprofdj@psu.edu, Penn State - Erie, The Behrend College

Homework Assignment 4B

Concepts:

• 2D Plane Stress (with thickness) Element Types
  • 2D 8-Node Structural Solid
  • Behavior Option: Plane Stress w/Thickness
  • Real Constant for thickness values
  • Multiple parts / different materials & real constants (assignment of element Attributes)
• Model construction with actual, physical interference
• Contact pairs with ramped, initial interference
• NON-Linear Solution:
  • small or large deformations ?
  • gradual load application (substeps)
  • automatic time stepping
  • iterative solution, (equilibrium) convergence
  • results controls
• Postprocessing:
  • Selecting (scoping) to examine results in each part
  • Contact Manager: display contact pair results
    

---

A STEEL cantilever beam (left) is 0.5" x 0.5" x 5" and extends (1") at the tip underneath a TITANIUM cantilever beam (right) which is 0.25" x 0.25" x 4".  There is an interference of 0.005" between these parts.

Use the ANSYS material library for properties of both bodies (1020 Steel & Titanium)

Model two rectangles for a 2D simulation.  These rectangles must physically overlap by the amount of interference defined for this problem.  Assign material and real constant attributes to the areas and mesh.

Use the Contact Manager/Contact Wizard to create a contact pair at the interface between these parts.  Specify default contact options except under the "Initial Adjustment" Tab, select "Include Everything With Ramped Effect."  Ignore friction between these parts (MU = 0).

Turn in:

• A plot showing the elements using color to distinguish different MATERIAL assignment AND showing different thickness in a 3D view with element shape based on real constant data
  [under PlotCtrls > Style > Size and Shape ... > turn ON the "Display of Element Shape Based on Real Constants" and specify a "Real Constant Multiplier" of 1.  Also, PowerGraphics must be ON]
• A plot showing ALL constraints and loads.
• Plots showing the normal stress (SX) for each beam, separately.
• A plot showing the contact pressure distribution between the parts
• A hand calculation of the force (Fy) created by the interference COMPARED to the Reaction Solution for EITHER part (not both).
• A hand calculation of the normal bending stress in the outermost fiber of each beam COMPARED to the normal stress (SX) for each beam.  [Beware of the "excessive constraint singularity" at the fixed end of each beam]
• The modeling session log file (with comments added).
  After successfully solving the model, Utility Menu: File > Write DB log file... > use a file name like "HW-4Blog.txt" and "Write Essential Commands ONLY"