Spring 2008, MET 415 - FEA Applications I

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

Homework 6B:  3D Solid Modeling

Concepts:

• SI Units
• 3D Modeling
• "Symmetry" features in modeling
• Symmetry (and Loads that lie on the Symmetry Plane)
• Singularity:  Stress under a point load
• Multi-body Parts
• Scoping Results
  

---



---

A steel triangular plate represents an idealization^[1] of a leaf spring (above).

• The plate is 90 cm. long, 25 cm. wide, and 2.5 cm. thick.
• A 4500 N load acts on each tip of the plate.
• At the center, the plate rests on a knife edge support.
• Elastic Modulus = 211x10⁹ Pa, Poisson's Ratio = 0.3

^[1]  R. C. Juvinall & K. M. Marshek, Fundamental of Machine Component Design, 2nd ed. Wiley & Sons, 1991, pp. 454-6.  Equations for maximum normal stress on outer fibers at center and tip deflection:
     where L is the length from knife-edge to tip

Use ANSYS-Workbench DesignModelerŽ to construct the complete 3D model.  [Or, make the complete part in Pro/E and Import it to DesignModeler]

• under Tools > Symmetry: create two symmetry objects to create a 1/4 symmetry model

In ANSYS-Workbench DesignSimulation:

• Under Mesh, Insert a "Method," scope: all bodies, Type: Hex Dominant (to create mostly brick-shaped elements)
• define knife-edge support (displacement with one direction, 0.0, and the others, free)
• apply load as force at a vertex (either components or vector direction)
• for the solution
  • turn off weak springs, 
  • request results of vonMises stress and total deformation, and to show the bending behavior normal stress and directional deformation, in appropriate directions
  • insert a Command Object which will determine mesh error (SEPC) for your model
    [You will notice SEPC is very high.  You know this model has singularities.  How can you evaluate results and mesh error away from the point load ?]
  • OPTION 1 (Multi-body part):
    • Return to DesignModeler:
      • create a New Sketch - draw a single line to cut the tip off the triangle, ~90% of distance from knife-edge to tip.
      • Extrude that line; Cut Material; Through All; Thin: Yes, with 0 thicknesses
      • Select both bodies and "Form New Part" (so they are "glued" together)
    • Return to DesignSimulation:
      • Update the simulation model
      • make sure all mesh settings, loads, & constraints are still properly defined on the updated model
      • add results plots for normal stress and vonMises stress which are SCOPED to the body which does NOT include the tip singularity
      • some selecting is needed to check SEPC with the model's tip removed - a deformed shape plot before and after selection is adequate
  • OPTION 2 (Command Object - advanced selecting):
    • Use an expanded command object to:
      • select nodes on the single-body part which exclude the tip
      • select elements attached to those nodes
      • plot the needed stress and deflection results
• "Duplicate" the first model
  • Change the Mesh - Method to "Tetrahedrons"
  • solve and examine/compare results
• Finally, from the WB Project Tab, Open either one of your simulations in ANSYS and examine the constraints to see if symmetry is enforced.

---

Turn in:

• TWO element plots showing your meshes, both the hex-dominant and tetrahedral mesh.  Label (caption or annotate) the element type and element shape on these plots.
  [Rather than generating the lengthy WB Report, once you create the display you need on the screen, there is a button on the top, far right end of the button toolbar that will allow you to capture figures to a PNG file. Use the "Image to File..." option]
• A plot showing BOTH of the symmetry regions of the model
• A plot showing ALL of the loads and constraints (i.e., the analysis environment)
• A hand calculation of the maximum tip deflection and the bending stress on the top face, directly above the support.  Use the hand calc. to verify the FEA model.
• A table comparing the solution which lists:
  • the different element types/shapes used,
  • the number of nodes and elements, 
  • actual maximum deflection, 
  • The total (overall) mesh error, SEPC, as well as the interpreted SEPC*, 
  • maximum normal stress*.  
  • Include the hand. calc. results in this table.
  • Include comments/footnotes on the level of error at the location where the max. stress occurs - explain why we use scoping/selecting to evaluate this analysis

• Contour plots of the solution results which shows the ACTUAL maximum normal stress* for BOTH models
• Deformed shape plots which show the ACTUAL tip deflection for BOTH models
   * Hint: To find the maximum deflection, the entire model should be scoped/selected.  Then, since a point load is applied to this model, there will be a high stress (and high error spot) directly under the load. Scope to exclude the loaded tip or UN-select the nodes and elements near the tip of the beam to find the maximum stress and the relevant error (SEPC) for this model.  Singularity is also present around the knife-edge support and effects the compressive stress levels.  (Don't draw any conclusions about the maximum compressive stress.)
• Answer these Questions:
  As Symmetry Objects from modeling are transferred to simulation:
  • Why are "Named Selections" created ?
  • Why is a coordinate system necessary ?
  • How can we be sure proper constraints are applied ?
    Include the regular ANSYS node plot showing all constraints