Spring 2008, MET 415 - FEA Applications I

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

Homework 6A:  3D Solid Modeling

Concepts:

• 3D Modeling
• Solid element types
• Tetrahedral meshing
• Element size control
• Concentrated Force/Moment Loading
• 3D Stress State evaluation
• Mesh error evaluation on large 3D models and around singular points

Problem Description:

A common steel link for the steering of a Cub Cadet lawn tractor is shown above.   A tie rod is attached by a bolt through the hole at the right end of the link.   The solid cylindrical protrusion on the left end transmits the load from the tie rod to the front wheel as a torque on the cylinder.  Part dimensions are given (in inches) in the figure below.

The loading to be considered for this part includes:

• The flat round end face of the cylindrical protrusion is fixed.
• A torque of 375 inch-lb_f CCW about the Z-axis acts from the hole about the axis of the cylindrical protrusion.  (You may apply a 125# load in the y-direction to the inside walls of the hole - investigate the "Bearing Load")
• A torque of 150 inch-lb_f CCW about the Y-axis acts from the hole on the right end  (Apply a 50# load in the -z direction on the edge of the hole)

For these loading descriptions, the Z-axis is the centerline of the cylindrical stub, and the X-axis runs from the center of the cylinder to the center of the hole.

Turn in:

• Answer these questions:

  • Does this model exhibit symmetry ?  
  • Is this a linear, static analysis ?  
  • Must you use a 3D model ?  
  • What element type should be used ?   
    
• An element plot showing your final mesh.  
  [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 simulation environment plot showing ALL the loads and constraints

• A hand calculation (from Strength of Materials) of the maximum equivalent stress on the cylindrical protrusion, just past the fillet on the +X axis side.  
  (This is a state of combined stress; use Mohr's circle sketch or formulae for your calculations)
  
• A stress plot to compare to your hand calculations and to illustrate the maximum stress on the part.
  
• Plots of deformed shape (include SEPC) and the element mesh error (SERR).  
  Is there any indication of singularity in this solution ? 
  • It is likely the mesh error, SEPC, may exceed 5%, but observing the element mesh error plot we may notice that the elements which add significant error may be far away from the region of concern (near the fillet).  
    Why refine the mesh near the hole or at the end of the cylindrical protrusion ? Is this a waste of resources ?
  •  Instead, use a Command Object to exclude those regions (the fixed support and the hole where the load is placed) by "Selecting" nodes and elements in and around the region of interest. Investigate commands: NSEL,S,LOC,... and NSEL,R,LOC,... and ESLN,S,n
  • By this method, we hope to conclude that the mesh error is low near the fillet where the max stress occurs and on the side of the post where our hand calc is checked.
  • Turn in the plot illustrating the mesh error from this method
    
• A printout of the ANSYS, FSUM result for forces and moments about the post centerline, at the end face of the post (SPOINT).  Use the FSUM output to confirm proper loading has been applied to the model.  SPOINT and FSUM commands may be embedded in a Command Object.  Their output will be found in "Solution Information"
  
• The ANSYS commands used in the WB Command Object to evaluate the mesh error and to check the forces and moments on the part.
  
• Answers to the other questions embedded in this section.