Spring 2009, MET 415 - FEA Applications I

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

Linear Assembly Practice Problem for Exam 2

Concepts:

• 3D Element Types
• Multiple parts 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)

A three-part assembly represents a butterfly valve. Analyze this device for condition of pressure on one side of the valve plate while holding the handle fixed using a LINEAR contact FEA model.

Analysis objectives: 

• evaluate deflection of valve plate when pressurized on one side

• evaluate stress in each body

 A ParaSolid geometry file is provided: 

• Right-click on this link:  butterfly_valve2.x_t "Save Target As...", then 

• "Save as type:" All Files, and use a file name like: "butterfly_valve2.x_t"  

Import the model to ANSYS-Workbench DesignSimulation:

• Open a new, empty project in WB

• Link to the Parasolid file

• Open DesignSimulation

• Set UNITS to Inches (in, lbm, lbf, ...)

• All parts will be structural steel

• When the model is imported to DesignSimulation, THREE contact regions should be automatically detected:

  • To keep this analysis LINEAR, use only bonded or no-separation contact conditions and small deflection analysis settings.

  • Use No Separation - Frame To Valve_Plate (for valve plate post to frame hole contact)

  • Use No Separation - Frame To Handle (keeps handle on top of frame)

  • Use Bonded - Valve_Plate To Handle (bonds handle to top of valve plate post)

• Apply a pressure load of 500 psi on the flat faces on one side of the valve plate.

• Use a CYLINDRICAL Support on the 8 holes in the valve frame.  Remember, you may use the macro:

  • Highlight 1 of the holes (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”

• For the CYLINDRICAL Support: zero the Radial and Axial directions, leave theTangential direction, Free.

• Apply FIXED Support to the end face of the handle

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

• Weak spring should be suppressed - not needed.  The solution can be solved as a single load step without gradual loading or substeps.

ANSWER THE FOLLOWING QUESTIONS:

Does this part have symmetry ? If so, how (describe precisely)?
    There is NO symmetry in this model
What element types/shapes were used (cross-out ALL INCORRECT responses)?
2D
3D
solid
shell
tetrahedral
quadrilateral
brick
triangle
prism

How many nodes and elements were created ? 
    77,179 nodes; 44,412 elements
List ALL element types used ?
    SOLID187, CONTA174, TARGE170, SURF154
What is the volume of the model (in in³) ?
    291.44 in³
What is the maximum deflection of your model (in in.) ?    0.016 in

Report the maximum vonMises stress (in psi) on the entire model ?    62,504 psi


Where does the maximum vonMises stress on the entire model occur at ?
    On the frame body, at the hole where the valve post is supported

Report the maximum vonMises stress (in psi) on the valve plate/post ?    51,922 psi


Where does maximum vonMises stress on the valve plate/post ?
    on the valve plate post at the edge of the frame support hole

Are the maximum stress values reported above real or artificial ? Explain.
   Likely artificial - sharp edges of no-separation contact support - probably some singularity effect