Fall 2007, MET 425 - FEA Applications II:
P-Method Finite Elements

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

Homework Assignment #1-B

Concepts:

• Review of 3D Modeling
• Taking advantage of geometric and load symmetry
• Definition of P-Method finite elements
• Different considerations for solving & postprocessing P-Method elements
• Application of strength of materials concepts (MCH T 213 and MET 320)
• ANSYS Workbench Environment (ANSYS WBE)

A plastic "coat pin" is to be evaluated considering a 50 N load on the tip of the smaller, round protrusion, down in the -Y direction.  The part is constrained at the flat end of the larger round protrusion.
This part is supplied to you in a Parasolid text file format: coat-pin.x_t  (This file is developed with SI units)
You may click here to access the Parasolid File   
BETTER YET: Use a Right-click on this link, then "Save Target As...", then "Save as type: All Files", and use a file name like: coat-pin.x_t 

• Young's modulus for polyethylene: 1.1x10⁹ Pa
• Poisson's ratio of polyethylene: 0.42
  
• Use the 3D Solid, P-Method elements in ANSYS to solve this problem. 
• SI Units are required for this analysis.
• Specify higher, local P convergence at the region(s) of high stress. 
• Exclude the p-elements near singularities from p-convergence consideration.

ANSYS Workbench Environment (WBE):  At ANSYS 11.0, P-elements are NOT available in WBE

You may import the CAD model in the ANSYS-WBE, Design Modeler (DM) or Pro/ENGINEER-Wildfire or directly into ANSYS

• You may need a modeling program to modify the CAD geometry for FEA
• If you use Design Modeler,
  • before leaving DM, under "File" you can "Export" the geometry as ANF (ANSYS Neutral File).
  • Close ANSYS-WBE; Open ANSYS traditional
  • Under "File" in the Utility Menu, "Read Input from..." the ANF file you saved in WBE-DM
• If you use Pro/ENGINEER or ANSYS, import the Parasolid file directly,
• Under "Preferences" in the side menu, request P-method, structural discipline
• Define element type 1 as 3D Tet, SOLID148.  Check the element options for proper values.
• Add material properties, 
• set mesh controls and free mesh the model with tetrahedral solid elements 
  Remember, P-elements can be coarser than H-elements.  A mesh with ~1000 P-elements is adequate.
• Define constraints:  make sure rigid body motion is NOT possible.
• Define load
• Under Load Step Options, add the P-element controls for polynomial range, polynomial "freeze" criteria, convergence levels (both global and local settings), and EXCLUDE elements where load singularities exist.
• solve and postprocess (remember, you must "Read Results" for P-element models and you may need to adjust /EFACET for smoothing contours)

Turn in:

• an element plot showing your mesh
• a node plot showing ALL loads and constraints
• a plot showing ALL P-convergence control points
• an element plot showing the elements which you have "excluded" from convergence calculations (use PltCtrls > Numbering to set /PNUM,EXCL,1 and do this with PowerGraphics = OFF)
• the final element p-level display
• the p-convergence history plot
• the vonMises stress contour plot
• a plot of the deformation results
• hand calculation of stress to support the simulation model, compared to an appropriate ANSYS stress result.
• Include a session log file, to which you have added comments describing the process of modeling and loading the model.  "Write a DB Log File" after you have constructed and successfully solved the original part mesh.  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.
  Try to have your comments describe the modeling process, not just a simple definition of ANSYS commands.