Spring 2012, MET 415 - FEA
Applications I
Prof. Dave Johnson, psuprofdj@psu.edu, Penn State - Erie, The Behrend College
Debriefing: Plate
with a Hole - In-class Example
A 12" x 12" x 1" aluminum plate has a
1" diameter hole at the center. This plate experiences a tensile (distributed)
load of 1000 psi in the horizontal direction. This model exhibits two planes of
symmetry. Determine the stress near the hole. Determine the deflection of
the plate.
CONCEPTS:
2D modeling
Planes of Symmetry
Stress Concentration
Geometric Construction: Primitive Shapes, Boolean
Operations
Finite Element Meshing / Mesh Controls
Presenting and Interpreting FEA Results
WHAT ELSE DID WE LEARN ?
- Choice of ELEMENT TYPE:
- Utility Menu: Help ->
Mechanical APDL > Element Reference
- Look up PLANE183 and PLANE182
- Why can we use a two-dimensional model of this plate ?
plane stress
- What gives this model "symmetry" ?
(geometry and ALL loads reflect)
- What is a Symmetry Boundary Condition ?
constraint - material cannot cross
or leave the symmetry plane
- Symmetry is (Important
or NOT Important) on such a simple model.
- We use symmetry because
simplifies
support (constraint) and reduces model size
- Location of ANSYS Material Library:
C:\Program Files\Ansys Inc\v140\ansys\matlib
Z:\Labsoft\Ansys\Ansys14\Ansys
Inc\v140\ansys\matlib
- Picking in ANSYS
- Right mouse toggles Pick/UnPick mode
- Left click-hold-move mouse, allows you to preview the pick
- If the PickTool does not appear when it should (Windows bug), "Reset
Picking"
- Order of Picking Entities may be critical (in subtraction) !
- Geometry of AREAS includes LINES and KEYPOINTS
(these are geometric entities “below” an area)
- What is the difference between "OK" and "APPLY" ?
both perform an operation, but OK
then dismisses the dialog box, APPLY keeps dialog box for additional
operations
- DELETE "AREAS AND BELOW" to completely remove unwanted geometry
- (UNDO) SAVE and RESUME of the ANSYS database file
- HW-1, Meshing:Clear the mesh, change mesh controls, and mesh again.
- Solid Model Loads vs. Finite Element Model Loads
- What is LS (when you Solve Current LS) ?
Load Step
Postprocessing:
- Do reaction force totals make sense ?
- What should the SF values be ?
- Does the deformed shape make sense
(direction and magnitude) ?
- Can deformation occur ACROSS the symmetry plane ?
- Can deformation occur ALONG the symmetry plane ?
- Do the values and the sign on the normal stress, SX (or
sx) make sense ?
- What is a reasonable target for SEPC (structural
% error in energy norm) ?
- SEPC measures error from
only the element mesh .
- If you want to reduce the SEPC, which elements should you refine*, i.e., make smaller ?
- How do you find those elements ? (Contour plot,
Element Soln. result SERR )
- What is SMNB and SMXB in the legend of the SX contour plot ?
related to mesh error, estimated lower
and upper "bounds" of result that you plotted
- What is the difference between a contour plot of Nodal Soln. and Element Soln. ?
Smoothed (averaged) contours vs. not
smoothed (unavg., perhaps jagged looking)
- What effect does PowerGraphics have on your plots ?
speed (faster), may effect appearance
and may allow or hide mesh error information
*HW-1: Mesh Convergence (means, refine the mesh
where needed, to achieve acceptable solution accuracy) process:
- Evaluate Mesh Error: Is SEPC acceptable ?
If "yes," then finish.
- If not, evaluate the individual element
Structural Error Energy (SERR). Refine the elements with the highest
SERR to most effectively reduce SEPC
Note: when SEPC and SERR are not available,
we evaluate change in results after successive mesh refinements, to decide
if the mesh has converged, i.e., no longer changes the answers significantly
as it is refined further.