FEA Applications II, Homework 3

MET 425 - FEA Applications II

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

HW-2B: Meshing in CAD

Concepts:

CAD model - meshing/loading in Pro/ENGINEER-Wildfire 5.0
Taking advantage of geometric and load symmetry
solving imported mesh with ANSYS, not Workbench

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). Save to MODEL.

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 ON (checked);
Default Interface: "Bonded"; Properties: "Merge Coincident Nodes is ON (checked); then click on OK
Pro/ENGINEER-Wildfire 4.0 Help tells us:
"FEM mode enables you to run integrated mode using Mechanica's finite element modeling functionality instead of its P-code functionality. This functionality enables you to create FEM modeling entities like loads, constraints, and idealizations. It also enables you to mesh your model with H-code elements, run various types of finite element analyses including NASTRAN, ANSYS, and so forth, and review the results of the run. You can activate FEM mode by selecting the FEM Mode toggle on the Model Type dialog box before you enter Structure or Thermal in integrated mode."

On the RIGHT side action buttons:

click on button for "Planar Constraint"
- Name: "SYMMETRY"
- member of "ConstraintSet1"
- pick the symmetry face (surface)
click on button for "New 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 " New 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.)

In the Main Menu, click on Analysis - > FEM Analysis...

create a "NEW" Simulation
Name: Latch_Press
Type: Structural
Description: (optional)
Constraint Sets: include ConstraintSet1
Load Sets: (none)
Done/Return

Mesh Controls:

click the button for "Mesh Controls":
- Name: "GlobalMax"
- Type: "Maximum Element Size"
- References: "Components"
- enter the size for this setting.
click the button for "Mesh Controls":
- Name: "MeshControl2"
- Type: "Maximum Element Size"
- References: "Surfaces"
- pick the area of the 0.75" fillet face (surface)
- enter the size for this setting.
Remember: Global MIN <= Local MAX or MIN <= Global MAX (or the Local setting will be ignored)

In the main button menu, press the button to create the mesh. Mesh Type: "SOLID." Check the element count in the info window. Close the "Elem Quality Checks" dialog box.

In the main button menu, press the "Run a Finite Element Model" (green flag) to create an "ANSYS" file, for "Structural" analysis, with "Parabolic" elements. Include the "ANALYSIS" case and the datum coordinate system (to orient the part), and use "Output to File" Notice in the Pro/E info window, the number of nodes and elements are reported. Quit the Review Mesh menu.

Solver: ANSYS
Analysis: Structural
Element Shape: Parabolic
Analyses: include the "Latch_Press" simulation environment
Coordinate System: either the World CSYS [WCS] or your own CSYS [CS0]
Output To File: Analysis_name.ANS in the current Pro/E working directory - analysis folder

In ANSYS, "Read Input from..." the Pro/E output file.

Before solving, check everything: check element type, material properties, loads, constraints through plots or listings

Turn in:

an ANSYS element mesh plot,

an ANSYS plot showing ALL the loads and constraints (environment),

a plot showing the highest equiv. stress on the part

any other plot(s) needed to justify the mesh error like SERR, deformed shape with SEPC, etc. [SEPC < 5%]

a plot showing the highest normal bending stress on the top face

In a TABLE, compare these results to HW-2A [force (FY), max. se, max sx on top face].
Also compare: the solid element type used, the number of node and elements.