Fall 2007, MET 425 - FEA Applications II
Nonlinear Behavior: Changing Contact and Plasticity
Prof. Dave Johnson, dhj1@psu.edu, Penn State
Erie,
The Behrend College
Homework Assignment 5A
Concepts:
- Material Plasticity
- Material properties graph plot (with enhancement)
- Defining and usage of Contact/Gap Elements
- Asymmetric vs. Symmetric pattern of contact pairs
- Iterative, Non-linear analysis options and controls
- Ramped loading, automatic time stepping, convergence issues
- Time History Postprocessing
- Time History Animation
The part shown in figure is made of 6061-T6 aluminum
alloy and is
0.125" thick.
The process is designed so the aluminum part will experience permanent, plastic
deformation.
It is pushed to the right 0.5" from its original position, contacts the 0.2"
diameter steel pin (which is 0.5" thick), and passes under it.
The steel is a typical 1020 grade and yielding of the steel is not to be considered.
The pin is rigidly constrained around its 0.04" I.D.
Create flexible-to-flexible body contact
elements between the surfaces which may come in contact.
Use a friction coefficient of 0.15 between the aluminum part and the steel pin.
Define material properties for the aluminum and steel using the ANSYS material library.
Add nonlinear stress-strain data for the aluminum assuming a perfectly plastic behavior
(Tangent modulus = 0) after yielding at 40 ksi.
Use a global mesh size of 0.015" with SmartSize = 3 (mostly quad. shaped),
add some finer mesh settings in the areas where you expect high stress and
where contact interactions will occur. This will keep the model size and run
time reasonable. (Giving about 1000-2000 elements).
Load the model by imposing a 0.5" displacement to the RIGHT on the LEFT edge of the
part's base. (This is an appropriate place to use Coupled DOF's - it helps
with postprocessing, later)
The bottom of the part is on rollers, i.e., it can have no vertical
displacement, only left-to-right movement.
Turn in:
- A "enhanced" graph plot showing the nonlinear material
stress-strain curve for the Aluminum part.
- A geometry plot showing the model and boundary conditions.
- A geometry plot showing the contact region defined for
these parts.
- A tabular listing of horizontal force vs. load step and
displacement during the process.
- A time history plot of the horizontal force/displacement graph as the part is
pushed under the pin
- Time history plots illustrating the convergence characteristics*
(force convergence, time
step size; no. of equilibrium iterations) of the problem solution. On
each 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 contour plot (or plots) showing the contact pressure between the parts
at the
time when the highest horizontal force is required to push the part under the pin.
- Prepare an animation (showing equiv. stress contours over time) to
show the process (for an in-lab homework grade). Use
"true" displacement scaling, the same contour legend, and
"frozen" view settings for all the images
animated.
- CONSIDER and COMMENT ON: Since SEPC is of NO value, how would you quantify/evaluate the mesh error in this
model ?
- Hand calc: If you consider the aluminum part is a
cantilever beam, is the force high enough to cause yielding at the fillets
on the base ?
* a useful command object is:
/POST26
! enter time history postprocessor
SOLU,2,FOCV ! store force convergence value
SOLU,3,DTIME ! store time step size
SOLU,4,EQIT ! store no. of equilibrium iter.
prvar,2,3,4 ! 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 time step size
plvar,4 ! plot no. of equilibrium
iter.
finish