Fall 2007, MET 425 - FEA Applications II

Nonlinear Behavior: Plasticity

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

Homework Assignment 5-B

Concepts:

• Material Plasticity, Large Deformation Effects
• Material properties graph plot
• Iterative, Non-linear analysis options and controls
• Ramped loading, automatic time stepping, convergence issues

The part shown in figure is made of common steel and is 0.20" thick. 
This material yields at 48,000 psi.  E = 30x10⁶ psi, Poisson's ratio is 0.3
After yielding, the tangent modulus is 340,000 psi. 
INCLUDE a 0.0625" fillet at the sharp corner.
Include large deformation effects in the solution.

For ANSYS Workbench Environment:

• In Design Simulation: 
• For the MODEL, define the material properties including the stress-strain curve
• For ENVIRONMENT, define the fixed boundary, and apply the traction load gradually, over some series of load steps.  Use a PRESSURE ("NORMAL To") load along the model's edge.  You may start with -1000 psi then ramp the load to its final value, -5000 psi.
• For SOLUTION, activate large deformation effects, Auto Time Stepping, and set the substeps (initial, minimum, and maximum).  "Weak" springs should be unnecessary.

Turn in:

• A graph plot showing the nonlinear material stress-strain curve for the steel material.
• An environment plot showing the model and boundary conditions.
• A plot showing the finite element mesh
• A time history graph of the reaction forces (Fx and Fy) on the fixed boundary vs. TIME.  (Export reactions to a spreadsheet to create the graph)
  NOTE: A significant, non-zero FX reaction force is expected - if FX is nearly zero, find the error.
• A time history plot illustrating the convergence characteristics* (force convergence, plastic strain increment) of the problem solution.  Under the plot, interpret what the plot is showing.
• A contour plot showing which sections of the part have experienced plastic deformation at the end of the process (Use equiv. plastic strain results plot).
• A contour plot showing the vonMises stress at the end of the process.
• A plot showing in the total deformation at the end of the process.
• At the FINAL solution step, check on reaction forces (X & Y directions): hand calculation compared to ANSYS Reactions at the fixed edge totals.
• Answer these questions:
  • Is this a 2D or a 3D system ?
  • How many nodes, elements, and what element types were used ?
  • Does the location of the maximum stress/strain make sense ?  Is it a real maximum or is it artificial (if artificial, what and where is the real maximum) ?
  • Why is there a non-zero, final Fx reaction ?

* - to plot time history data using the old time history postprocessor, insert a command object under solution with these lines:

/POST26         ! enter time history postprocessor
SOLU,2,FOCV     ! store force convergence value
SOLU,3,PSINC    ! store plastic strain increment
prvar,2,3       ! list data
/PLOTP,INFO,1   ! set up plot format
/SHOW,PNG       ! send plots to PNG file
/GFILE,400      ! plot file resolution
/RGB,INDEX,100,100,100,0     ! switch the
/RGB,INDEX,0,0,0,15          ! B/W colors
plvar,2         ! plot force convergence value
plvar,3         ! plot plastic strain increment
finish

/POST1           ! enter the general postprocessor