Spring 2009, MET 415 - FEA Applications I

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

Homework Assignment 7A

Concepts:

• 3D Element Types
• Multiple parts, different materials, AND changing contact between parts
• Parasolid geometry import of an assembly
• Linear Solution:
  • Contact/Target behavior (bonded and no separation)
    • no separation contact: contact/target pairs which are close together, cannot separate along the normal direction to the contact surface (sliding is permitted).
    • bonded contact: contact/target pairs which are close together, cannot separate along both the normal and tangent directions to the contact surface (fully bonded).
• Postprocessing: 
  • Different Bodies (Selecting/Scoping)
  • Contact pair results (Contact Tool & Hide Body function)

A five-part assembly represents an impeller type pump. Our primary goals are to analyze the assembly with a preload on the belt of 100N to test that:

• the impeller will not deflect more than 0.075mm with the applied load.

•  the use of a plastic pump housing will not exceed the material’s elastic limits around the shaft bore. 

A geometry file is provided on your MET 415, ANGEL Lessons Page

• Click on the "lesson" - HW-7A geometry (zipped Parasolid text: Pump_assy3.x_t) 

• Right click on the file name, Pump_assy3.zip,  

• Then "Save Target As..." and use a file name like: "Pump_assy3.zip"

• Unzip the file to find the Parasolid geometry: Pump_assy3.x_t

Import the model to ANSYS-Workbench SIMULATION:

• Open a new, empty project in WB

• Link to the Parasolid file

• Open a New Simulation

• Set UNITS to Metric (mm, ...)

• Rename each Part to have useful names: pump_housing, impeller, pulley, shaft, nut

• Assign WB material library properties for polyethylene to the pump housing

• Assign WB material library properties for structural steel to the other (4) bodies

• In the Tree Outline, seven (7) contact regions should be automatically detected by WB
  Right-mouse on "Connections" and use "Rename Based on Definition" to update to the new, useful part names

• In the Tree Outline, seven (7) contact regions should be automatically detected by WB:

  1. inside of housing to top of impeller body

  2. top of housing to pulley hub face

  3. hole through top of housing to O.D. of shaft

  4. hole through center of impeller to O.D. of shaft

  5. face of impeller to face of nut

  6. hole in center of pulley to O.D. of shaft

  7. I.D. of nut to O.D. of shaft

  • Contact Regions 1,2, and 4 are to be treated as "No Separation" (click on each one and set behavior in the Details Area)

  • Contact Regions 3 and 5 - 7 are to be treated as "Bonded" (click on each one and set behavior in the Details Area)

• Assume the pump housing is rigidly mounted to the rest of the pump assembly. To simulate this, apply frictionless support to the mounting face.

• Apply frictionless support on the mounting hole counter bores to simulate the mounting bolt contacts.

  • Each of the required surfaces (8) could be selected individually while holding the CTRL key however we will use a macro (Select by Size) provided with the DS installation. After selecting the initial surface, running the macro finds and selects all surfaces of the same size (area). [Note, this macro also works with edges or bodies.] 

    • Highlight 1 of the countersink surfaces (arbitrary - any one of them).

    • Choose “Tools > Run Macro . . ."

    • Browse to the ANSYS Installation Directory ...\ANSYS Inc\v110\AISOL\DesignSpace\DSPages\macros

    • In the browser choose “selectBySize.js”

    • Click “Open”

• Apply a bearing load (F_X = 100 N) on the pulley to simulate the load from the drive belt. The bearing load will distribute the force over the face of the pulley only where the belt contact would occur (parabolic distribution)

• This contact analysis is a LINEAR simulation (No Separation & Bonded contact options are not automatically nonlinear)

• Weak spring should be suppressed - not needed
  Note : Because of the presence of frictionless supports & non-bonded contact, Workbench-Simulation will trigger the use of weak springs during the solution. If we know the model is fully constrained we can turn off this function.

Turn in:

• A plot showing the mesh (document the number of nodes and elements used)
• An "environment" plot showing all the loads and constraints on the model
• A plot showing the total deformation that occurs on the model.
• A plot showing the maximum vonMises stress that occurs on the model.
• A plot showing the total deformation that occurs on the impeller alone (SCOPE results to one body)
• A plot showing the maximum vonMises stress that occurs on the impeller alone (SCOPE results to one body)
• A plot showing the total deformation that occurs on the housing alone (SCOPE results to one body)
• A plot showing the maximum vonMises stress that occurs on the housing alone (SCOPE results to one body)
• A plot showing the contact pressure on the top face of the housing where it mates with the hub of the pulley (Use a Contact Tool Object, scoped to the desired face, to see results on that face).  HINT: under Geometry, it is useful to hide other bodies temporarily while finding the faces you want on the housing
• A plot showing the contact pressure on the top face of the impeller hub where it mates with the inner face of the housing (Use a Contact Tool Object, scoped to the desired face, to see results on that face) 
• Evaluation of this design:
  • Does the impeller deflect more than  0.075mm under the given loading ?
  • Is yielding of the housing material likely to occur ? (use the tensile yield strength from the WB material library data)
• A plot showing the normal bending stress on the shaft, compared to a hand calculation of the expected bending stress on that body.
  Note: The shaft diameter is 25 mm & its length is 75 mm. Along the shaft axis, it is 6.5 mm from the mid-plane of the pulley to the interface of the pulley hub/housing.  Also, from the mid-plane of the pulley to the inner face of the housing is 36.5 mm.