Spring 2008, MET 415 - FEA Applications I

Prof. Dave Johnson, dhj1@psu.edu
Penn State - Erie, The Behrend College

Homework Assignment 4A

Concepts:

• 2D Element Type, plane stress with thickness
• Multiple parts AND Changing contact between parts
• IGES geometry import
• NON-Linear Solution:
  • small or large deformations ?
  • gradual load application (substeps)
  • automatic time stepping
  • iterative solution, (equilibrium) convergence
  • results controls
• Postprocessing: 
  • Different Bodies (Selecting/Scoping)
  • Contact pair results

Two plastic parts snap together as show in the figure below.  The parts are 10 mm thick. 
The material is low density polypropylene (E = 350 MPa, Poisson’s ratio = 0.35 and Sy = 28 MPa).  The coefficient of friction of this material is 0.1 in the expected assembly conditions.
The intention of the design is that the total force to push the parts together must be under 20 N.
Also, a Factor of Safety of 2 is required based on energy distortion theory.

A 2D IGES file is provided - it contains ONLY lines and points on the XY plane. 

• Right-click on this link:  IGES File 

• "Save Target As...", then "Save as type: All Files", and use a file name like: "snap_fit.igs"  

Import the model to ANSYS:

• Why can't symmetry be used for this simulation ?

• Create appropriate areas from the set of lines.  
  Main Menu: Preprocessing > Modeling > Create > Areas > Arbitrary > By Lines (Try picking with "Loop")

• Copy the smaller area of the insert, "up" 22 mm to place it above the larger body.  

• Then, delete the original instance of the insert body.

• Set Attributes for ALL Areas: Material, 1; Element Type,1; Real Constant Set, 1

• Suggested mesh size: 0.5 mm global size + SMRTSIZE, 1 or 2

• Open the "Contact Manager" (ANSYS GUI, last button, top right)
  The "Contact Wizard" is the first button in the "Contact Manager"

• Use the Contact Wizard to create a set of contact/target pairs between the mating faces of the parts

• Use the Contact Wizard to create a set of contact/target pairs to detect self-contact on the inner walls of the insert.

• For BOTH contact pairs, suggested settings:

  • symmetric contact/target element pattern

  • update stiffness, each substep (pair based)

  • penalty method formulation

• If you decide to re-mesh the areas, delete all contact pairs and rebuild them after meshing
  Contact/Target elements are created on the element faces of the current mesh.

• To prepare for solving, don't forget nonlinear solution settings:
  Main Menu: Solution > Analysis Type > SolnCtrls...
  Large Deflection, Static; Automatic Time Stepping, ON; Substeps: Initial, Max, Min (100, 10000,5); Output Frequency (-20)

Turn in:

• A plot showing the mesh
• A plot showing the constraints on the model
• Produce an animation of the results (vonMises stress over time)
  Utility Menu: PlotCtrls > Animate > Over Time... : 20 Frames, Time Range (0 - 1), stress, vonMises
• A plot showing the maximum vonMises stress that occurs on the model.
• Evaluation of this design:
  • does the model require < 20 N to engage the snap fit ?
    [check each results set to find the maximum force reaction, Fy, on either body.  Report the maximum Fy value and the time when it occurs]
    • Select either body (you must select only one.  WHY ?): 
      Utility Menu: Select > Entities > Areas > By Num/Pick
       then Utility Menu: Select > Everything Below > Areas
    • General Postprocessor: Read Results > First Set 
      List Results > Reaction Solution ... FY
    • Then, 
      Read Results > Next Set
      List Results > Reaction Solution ... FY
    • Repeat
  • Is yielding of the material likely to occur ?  Is a factor of safety > 2 maintained ?
• Use an animation to examine the variation of contact pressure between the two parts.
  Utility Menu: PlotCtrls > Animate > Over Time... : 20 Frames, Time Range (0 - 1), contact, pressure
  Also, the "Contact Manager" may be used to view contact pair results
  Report the maximum contact pressure value and the time when it occurred.
• 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-4Alog.txt" and "Write Essential Commands ONLY"
  Comments are not needed on graphical picking commands (FLST, FITEM), but should be on the action command that follows the picking.  For example: 
  ASBW,P51X        !  Divide areas by WP based on graphical picking, above
  You can view a SAMPLE LOG FILE.
  A word of advice:  the comments you add to the logfile should make it read like a story of the process you followed in creating the model.  Log file comments are NOT simply ANSYS command definitions.  Start with the ANSYS command definition (from the ANSYS Help System, Command Reference Guide), then add or describe how the command is used in your modeling.  ALL "action" commands should have a comment.  Postprocessing does not need to be included.