Spring 2008, MET 415 - FEA Applications I

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

Homework Assignment 3A

Concepts:

• Multiple parts / different materials (assignment of element Attributes)
• 2D Axisymmetric Element Types
• Materials which may yield (plasticity)
• Density Material Property, Units
• Structural Temperature Load / Thermal Strain
• 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)

An injection molding process surrounds a disc-shaped magnet with a polyethylene plastic which covers all of the magnet except one disc face and the plastic forms a small, round central handle on the opposite face.  A concern in producing this part is that as the hot plastic cools, the brittle ceramic magnet may fail.  The plastic solidifies at 136^oC.  The magnet disc insert in the mold is assumed to also be 136^oC as the plastic solidifies around it.  We want to simulate the cooling to room temperature (20^oC) from the moment that the plastic solidifies.

[All dimensions are given in mm]

---

• Make a Pro/ENGINEER assembly of these parts - make a 1/4 sector of the whole assembly

• create a datum coordinate system (to orient the part when imported into ANSYS). We need a face of the sector to lie in the ANSYS XY plane, on the +X side with the assembly's centerline exactly on the Y-axis.

• In Pro/E, under: FILE -> Save a Copy -> change the file TYPE to: Parasolid (*.x_t) -> hit OK -> choose "Solid" & "Shell", pick a coord. system, and write the Parasolid file. 

• In the ANSYS File menu, under "IMPORT...", choose Parasolid (PARA...), use the default settings (and pick the Parasolid file that was just created by Pro/ENGINEER

• In the Preprocessor, Main Menu: Modeling > Delete > Volumes Only, Pick All

• Then, Delete > Areas & Below, Pick ALL areas which are NOT on the XY plane

• Glue (or Overlap or even Merge coincident KP) to make sure the parts share their common edges.

• CHECK ALL Model dimensions (to make sure the transfer to ANSYS gives you the model you need).  For a quick check, use the command ASUM - estimated area should be ~(11 x 9) - (8.5 x 4) mm² =  65 mm²
  [Scale the model dimensions if necessary: Preprocessor > Modeling > Operate > Scale > Areas, Pick,All]

The properties for the ceramic magnet material are:

• Elastic Modulus, EX: 150,000 MPa

• Poisson's ratio, PRXY: 0.3

• Density, DENS: 5 x 10^-6 metric tonne/cu. mm.

• (secant) Coefficient of Thermal Expansion, ALPX: 9 x 10^-6 mm/mm/^oC

• assign the Reference Temperature (stress-free state): 136 C

• Ultimate Tensile Strength: 50 MPa

• Ultimate Compressive Strength: 700 MPa

The properties for the HDPE material are:

• Elastic Modulus, EX: 1,100 MPa

• Poisson's ratio, PRXY: 0.42

• Density, DENS: 9.5 x 10^-10 metric tonne/cu. mm.

• (secant) Coefficient of Thermal Expansion, ALPX: 2.3 x 10^-4 mm/mm/^oC

• assign the Reference Temperature (stress-free state): 136 C

• Yield Strength for this HDPE: 25 MPa

• for a bilinear stress-strain model, the Tangent Modulus is 8.0 MPa

Nonlinear Solution:
Main Menu: Solution > Analysis Type > SolnCtrls...
To define: LOAD STEPS, SUBSTEPS, OUTPUT CONTROLS

Turn in:

• A plot showing the mesh - with different materials shown by different color
• A plot showing the constraints on the model
• A plot showing the deformation of the entire assembly
• A plot showing the equivalent stress on the plastic material ONLY.
  Utility Menu: Select > Entities... > Elements, By Attributes, Material Num, 1 (or 2), From Full, OK
  Interpret this plot: Has the plastic been stressed at or above its yield point ?
• A plot showing the tensile stress (first principal stress) on the magnet disk ONLY.
  Utility Menu: Select > Entities... > Elements, By Attributes, Material Num, 2 (or 1), From Full, OK
  Interpret this plot:  Is the magnet likely to crack ?
• 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-3Alog.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.