FEA Applications II, Homework 4

Fall 2011, MET 425 - FEA Applications II

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

HW-2A: MECHANICA P-element Model

Concepts:

CAD model - meshing/loading in Pro/ENGINEER-Wildfire 4.0
Taking advantage of geometric and load symmetry
Solving and postprocessing with Pro/ENGINEER-Mechanica
Application of strength of materials concepts (MCH T 213 and MET 320)
Different considerations for meshing, solving & postprocessing P-elements

A plastic latch, in the figure above, has Young's modulus: 350,000 psi, Poisson's ratio: 0.40

This part was modeled in Pro/ENGINEER. You may click here to access the IGES File

The part is fixed to a wall on the vertical flat (left) face

The sharp edge of the catch must be depressed 0.25" to engage/disengage the latch.

Open the IGES model as a part in Pro/ENGINEER

In Pro/E, define the material properties and assign the material properties to the part.
Under File >Properties: Units … change (choose a useful set of units for this model: inch - lbf - sec)
Under File >Properties: Material … change … File > New - define a new material named: plastic with modulus and Poisson's ratio (and density, if required)

Create a cut for the 1/2 symmetry model - include other appropriate simplifications.
In Pro/E-Widfire, under: Applications -> Mechanica -> approve the Units being used,
Use Model Type: "Structure"; make sure Mode: "FEM Mode" is OFF (UNchecked);
Default Interface: "Bonded"; then click on OK

On the RIGHT side action buttons:

Assign the material properties to the part
click on button for "Symmetry Constraint"
- Name: "SYMMETRY"
- member of "ConstraintSet1"
- type: "Mirror"
- pick the symmetry face (surface)

click on button for "Displacement Constraint"
- Name: "BASE"
- member of "ConstraintSet1"
- References: "Surfaces"
- Coordinate System: use [WCS] or pick your own CSYS from left side menu
- pick the latch base face (surface)
- set ALL translations and rotations to "fixed"
click on button for " Displacement Constraint"
- Name: "IMPOSED_DISPLACEMENT"
- member of "ConstraintSet1"
- References: "Edges/Curves"
- Coordinate System: use [WCS] or pick your own CSYS from left side menu
- pick the top edge of the sloped face (line)
- set ONLY the vertical translation to "prescribed" and enter 0.25" down (all other DOF's are "free")
this model has no other loads (no pressure, force, temperature, etc.)

On the RIGHT side action buttons:

Find the button for "Simulation Measure" (looks like a ruler) [or, from the main toolbar, "Insert > Simulation Measure..."]

"Measures" define result quantities at specific locations to be monitored during an analysis
"Measures" are important for convergence of the analysis model
"Predefined measures" are automatically calculated, are "global" (apply to the entire model); examples: maximum stress, strain energy, and displacement
"User-defined measures" (or custom measures) may be added; can be "scoped" to a face, edge, or point; and can be defined at or near a datum point

DEFINE appropriate user-defined measures

Mesh: Mechanica meshes the model automatically before each solution
The AutoGEM (Automatic Geometric Element Mesher) is used to inspect the mesh, adjust size, correct meshing problems.
In the Main Menu, click on AutoGEM - > Control... for mesh sizing controls -OR- > Create... to make a mesh
For this exercise, use the default mesh - insert NO mesh controls. Record the number of nodes and elements created.

In the Main Menu, click on Analysis - > Mechanica Analyses/Studies...

create a "New Static" Analysis
Name: Latch_Press_P
Description: (optional)
Constraint Sets: include ConstraintSet1
Load Sets: (none)
Nonlinear ? (not needed)
Inertia Relief ? (not needed)
Convergence TAB: Method: Multi-Pass Adaptive
Polynomial Order - Minimum:2, Maximum: 9
Limits - Percent Convergence (use value < 10%)
Converge On: MEASURES (pick your user defined stress measures)
Output TAB: calculate stresses, reactions, local stress errors
Excluded Elements TAB: default settings
then click on "OK"

Run (Green Flag) the Analysis Study - view interactive diagnostics (yes)
When the run is complete - save the Diagnostics as a text file
Also, view and save the Run Status information as a text file

Review Results:

Name: WINDOWx
Title (if desired)
Display Type: Fringe
Quantitiy: Stress, VonMises (or Stress, XX or others)
Display Locations (entire model, selected face, edge ?)
Display Options: Contour plot ? Continuous Tone ?
Format > Result Window > Background color: WHITE
"EDIT the Selected Definition" to view different results or add additional results windows to the display

Hand calculation:

Estimate the force required to bend a simplified, similar "cantilever" beam by 0.25" and compare this to the FEA model reaction total Fy on the edge of the sloped face of the latch
Estimate the max. normal stress on the the top face of the latch, beyond the 0.75" fillet (using the bending force, Fy from the FEA solution). Compare it to the proper FEA results plot to validate your model.

Turn in:

a Mechanica element mesh plot (document the number of elements),
[File > Save A Copy... TYPE: JPEG or TIFF]

a Mechanica plot showing ALL the loads and constraints (environment) and the "user-defined measures",

Append the "Simulation Diagnostics" report for this model (which you saved when you solved)
Answer these Q: were there any warnings about your model ? What should you do about them ?

Append the "Run Status" report for this model (which you saved when you solved)
Make a statement to summarize the no. of p-loop passes and the lowest/highest polynomial level used for the model.

Find the Mechanica spreadsheet report on ALL "Measures" (*.csv) and include it in the HW packet as a spreadsheet table - note your user defined measures on the table.

a plot showing the highest equiv. stress on the part
[File > Export > Image... TYPE: JPEG or TIFF; To File: browse for folder & assign name]

a plot showing the normal stress along the top face of the latch

a plot showing the p-levels

a plot showing the Element Stress Error Estimate

Determine and report the y-direction reaction force resultant from Mechanica. Document the procedure you used to find the reaction force.

Hand calc of force and normal stress, compared to proper FEA results