Fall 2011, MET 425 - FEA Applications II

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

HW-1B: plastic part

Concepts:

• Review of 2D Modeling - different thickness bodies, form a single part
• Taking advantage of geometric and load symmetry
• Review considerations for meshing, solving & postprocessing
• Application of strength of materials concepts (MCH T 213)
• 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 face is fixed (A) and the slotted end experiences a force (B) which puts the part in direct tension

Note: Frictionless Support (C) is equivalent to a Symmetry edge condition

• 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.)  USE Trial-and-Error to find the allowable force.

Perform the analysis using ANSYS-Workbench. Specify mesh controls to produce mesh error < 5%

Turn in:

1. an element plot showing your mesh. Report the number of elements and the number of nodes
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
8. Report the force that will cause stress to reach the allowable level
9. Compute and compare the maximum stress SX determined by classical stress concentration formula
10. Estimate of the axial deflection of the plate compared to the FEA model maximum deformation

ANSYS Workbench Environment (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.

REMEMBER: 2D models are "surface bodies" and must lie on the XY plane

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 WB Project Schematic, open “Engineering Data,” create a new material, PEEK, and enter modulus and Poisson's ratio).
• 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 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,500    ! 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