Fall 2007, MET 425 - FEA Applications II:
H-Method vs. P-Method Finite Element Formulations,
A Stress Concentration Study

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

Homework Assignment #1-A

Concepts:

• Review of 2D Modeling - different thickness bodies form a single part
• 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 GUI and ANSYS Workbench Environment (ANSYS WBE)

A plastics engineer needs to find the ultimate load that can be sustained by a product.  Deformation is not a concern.  The materials is Polyetheretherketones (PEEK), also referred to as polyketones.

• Young's modulus for PEEK: 2.06x10⁶ psi.
• Poisson's ratio of PEEK: 0.40
• The thick end is fixed and the slotted end experiences a force which puts the part in direct tension
• Evaluate the stress, mesh error, and deflection of this part
• Determine the force this part can carry without exceeding the allowable stress limit of 24,000 psi.  
  (PEEK is considered a "ductile" material.)

Part 1:  Perform the analysis using H-Method elements in ANSYS-Workbench. Specify mesh controls to produce mesh error < 5%

Turn in:

1. an element plot showing your mesh
2. (environment) plot showing ALL constraints and loads
3. the SX stress contour plot
4. the vonMises stress contour plot
5. the total deformation or UX deformation contour plot
6. a display of the individual element error, SERR. Include the global error %, SEPC, as an annotation on your plot
7. any other plots needed to illustrate the quality of the stress results with respect to mesh error issues

Part 2:  

Use the P-Method elements in ANSYS to solve this problem. Use the DEFAULT mesh size + SMRTSIZE  

Specify higher, local P convergence at locations of high stress which you discovered in Part 1.

Turn in:

1. "Environment" plot showing ALL constraints and loads
2. a node plot showing ALL P-convergence control points
3. an element plot showing your mesh, including:
   the EXCLUDED p-elements, and
   the proper model thickness specification [use PlotCtrls > Style > SIZE & SHAPE]
   (optional) include the P-convergence control points, and ALL loads and constraints
4. SX stress contour plot 
5. the vonMises stress contour plot
6. the total deformation (USUM) or UX deformation contour plot
7. the P-convergence history graph
8. the final element p-level display

Make a table comparing the P-Method and H-Method results: maximum SX and SEQV, maximum deflection, and the reaction force total in the horizontal direction. Also, report the number of elements and the number of nodes for each type of analysis.
Report the force that will cause stress to reach the allowable level.
Finally, compute and compare the maximum stress SX determined by classical stress concentration formula; and an estimate of the axial deflection of the plate compared to the FEA model maximum deformation.

ANSYS Workbench Environment (WBE):  At ANSYS 10.0, P-elements are NOT available in WBE

You may build the model in the ANSYS-WBE, Design Modeler (DM)

• use "Sketching" to create the cross-sections for a "Multi-body Part",
• in DM, under "Concept" create "Surface from Sketches" and enter the 2D part thickness, here
• From DM, under "File" you can "Export" the geometry as ANF (ANSYS Neutral File) to use later.

Move the solid model into ANSYS-WBE, Design Simulation (DS)

• switch back to the WBE-Project Page and under "Advanced Geometry Default" request 2-D
• enter the properties of PEEK (in the Model Tree, open Geometry, click on Surface Body) - remove heat transfer and magnetic properties, remove unnecessary structural properties, adjust value of modulus.
• create a mesh appropriate for this analysis.  
  Remember, WBE is using H-elements.  Consider: Advanced mesh controls:
  • element size
  • curve/proximity sensitivity
  • aggressive shape checking
• apply constraints (frictionless surface = symmetry).  Make sure rigid body motion is NOT possible.
• apply a force load on the right edge to create a state of tension in the part
• For the DS solution, use:
  • small deflections, linear
  • weak springs: OFF
  • define solution results needed for the H-element model: SX stress, error, deformation, etc.
  • add "Command Object" under SOLUTION in the Model Tree, to evaluate overall mesh error (SEPC) and the reaction force

    /SHOW,PNG ! send plots to PNG file /GFILE,350 ! plot file resolution /RGB,INDEX,100,100,100,0 ! switch the /RGB,INDEX,0,0,0,15 ! B/W colors /VIEW,1,0,0,1 ! set the viewing direction PLDISP,2 ! plot deformed shape w/undeformed edge /SHOW,TERM ! direct plots back to screen PRERR ! Print global error, SEPC PRRSOL,FX