FEA Applications I, Homework 6B

MET 415 - FEA Applications I

Prof. Dave Johnson, psuprofdj@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 and at knife edge support
Multi-body Parts
Meshing Methods: Hex Dominant, Tetrahedral, Swept; Lower- and Higher-Order Elements
Scoping Results
Transfer model from Workbench to ANSYS

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 which estimate the maximum normal stress on outer fibers at center and tip deflection:
where L is the length from knife-edge to tip

Use ANSYS-Workbench DesignModeler® 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:

Set "Relevance" and "Element Size" for the entire model. Make sure there are at least 3 elements through the plate thickness. Use a Mesh Control on face, if needed.

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 ?]

Step 1 (create a "Multi-body" part):

Return to DesignModeler:

create a New Sketch - draw a single line to cut the tip off the triangle, ~75% 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 - "Refresh Geometry" at the top of the Outline

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, showing SEPC, before and after selection is required

Step 2 (Command Object - advanced selecting):

In DesignSimulation, create a "Named Selection" of the part which is NOT the tip

Use a command object to:

select the elements of the single-body which excludes the tip [CMSEL,S,"name"]

select nodes attached to those elements [NSLE,S]

plot the needed deflection results (can ONLY be done by commands)

MODEL-2: "Copy" the first model: in the WB Schematic, right mouse on "Model" then pick "Duplicate"

Change the Mesh - Method to "Tetrahedrons"

adjust mesh size to make sure the mesh error that matters is < 5%

solve and examine/compare results

MODEL-3: "Copy" the first model again

Change the "Element Midside Nodes" ADVANCED Mesh setting to: "Dropped" to force a lower-order element choice

Change the Mesh - Method to "Sweep"

adjust mesh size to make sure the mesh error that matters is < 5%

solve and examine/compare results

Finally, from the WB Schematic, for MODEL-3: right mouse on "Setup" and then, "Transfer Data to New >" "Mechanical APDL." This creates a new linked object on the schematic page.
Next, right mouse on "Analysis" and then, "Edit in Mechanical APDL" to open the model in ANSYS and examine the constraints to see if symmetry is enforced.

Turn in:

THREE element plots showing your meshes, both the hex-dominant and tetrahedral mesh for the higher-order cases and the swept mesh for the lower-order case. Label (caption or annotate) ALL element types, the element shape, and the number of nodes & elements 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*,
- The real (not artificial), maximum normal stress*.
- Include comments/footnotes on the level of error at the location where the max. stress occurs - explain why scoping/selecting was used to evaluate this analysis

Contour plots of the solution results which shows the ACTUAL maximum normal stress* for ALL THREE models. (Actual max. stress values exclude artificial high values from singularities)
Deformed shape plots which show the ACTUAL tip deflection for ALL THREE 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 do we want to make sure there are at least 3 elements through the plate thickness ?
- Why are "Named Selections" create ? (Describe BOTH reasons you have "Named Selections" for this project)
- Why is a coordinate system necessary ? What is it used for ?
- How is the concentrated vertex load in WB applied to the ANSYS model ?
- How can we be sure proper constraints are applied for the symmetry conditions?
  Include the regular ANSYS node plot showing proper constraints to enforce symmetry