MET 425 - FEA Applications II

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

Lecture Notes: P-Elements

P-elements have a different mathematical formulation than h-elements.

P-elements have shape functions with variable polynomial order. Convergence is achieved by increasing the polynomial order for a given mesh.
H-elements have a fixed shape function polynomial. Convergence is achieved by refining the mesh in regions where higher accuracy is needed.
P-elements can capture more complex behavior with a coarser mesh than h-elements, but are more resource intensive, both computer memory and disk space.
With P-elements, the user is LESS responsible for manually designing an accurate mesh.
Recent advances in (Mechanica) P-element capabilities: large deformation and contact problems, transient thermal and structural behavior, 2D modeling

At ANSYS 13.0, p-elements at NO LONGER included. Pro/ENGINEER-Wildfire, Mechanica uses p-elements

At ANSYS 12.1 and earlier, only available in ANSYS, not in Workbench

(structural):
- PLANE145: 2D Quad 145
- PLANE146: 2D Triangle 146
- SOLID147: 3D Brick 147
- SOLID148: 3D Tetrahedral 148
- SHELL150: 3D Shell 150
(electrostatic):
- SOLID127: 3D Tetrahedral 127
- SOLID128: 3D Brick 148

What is different about a P-element modeling ?

In meshing, you can use a coarser mesh than you would with h-elements

In solution:

Loading: You should avoid applying single-point loads or constraints, since they cause stress concentrations . If these loads or constraints are applied, exclude the elements attached to these nodes from the convergence computations.

Set the Convergence Criteria: in Mechanica these are called "measures"
Mechanica “Simulation Measures” are similar to ANSYS SERR & SEPC error checking

Exclude parts of the model from convergence testing, if needed

The solution automatically loops, adjusting p-levels to reach convergence criteria.
Make sure the solution converges before you use the results !!!
HOW ? look at the MECHANICA Run Status report

Possible Causes of P-element Convergence FAILURE	Solution
The convergence criteria is too tight for the maximum allowable p-level and the mesh.	Relax the convergence criteria.
The convergence criterion was specified at a singularity (infinite stress or strain value, such as under a point load) or the elements near the singularity were not excluded.	Do not monitor a singularity point.
The mesh is too coarse, especially in the area where the stress is high.	refine the mesh in those areas
The maximum p-level was restricted lower than that required for convergence.	Allow the maximum p-level to go higher.

After SOLVING (postprocessing), check

The P-Convergence: for the specific criteria/measures you set in solution
The P-Levels: to see what polynomial level was used for each element in the model. Does it make sense (high polynomials needed at stress concentration) ?

MECHANICA Analyses TYPES:
(from the Pro/E Help System > Mechanica Simulation Advisor)

Static
Static w/large deformations
Modal analysis
Prestressed static or modal analysis
Buckling
Contact
Dynamic
Fatigue
Thermal analysis, steady-state or transient
Sensitivity study
Optimization design study

Mechanica Simulation Advisor also discusses “idealizations” which means simplified to shell, beam, lumped mass, or spring

Models can be solids or shells or both

Can we analyze assemblies or parts only ? BOTH

Parts can be connected by contacts, rigid links, welds, beams, springs, etc.

Simplify models: 2D ? beams ? springs ? shells ? symmetry ?

suppress outside rounds/chamfers, etc.

Singularities affect Mechanica solutions. Point loads, point constraints, sharp corners, even at the interface between elements of different properties, materials, or element types

After solving, select Info>Status from the “Analyses and Design Studies” dialog box.

For each analysis in the design study, Mechanica reports:

warning or error messages
statistics on convergence and performance
predefined and user-defined “measures”

Mechanica Convergence:

Default: SPA (Single-Pass Adaptive) which is the most efficient choice for general problems.

In the first of two solutions, Mechanica calculates results and estimates errors, based on continuity of stresses over element boundaries—these errors are then used to predict the polynomial order required for a converged solution. The software then performs a second run that produces the final converged results.

Alternative: MPA (Multi-Pass Adaptive) is available in cases where SPA does not apply, or when you require more convergence feedback. In this method, the software adapts the polynomial orders across element edges until global or user-defined measures no longer change within a user-specified tolerance or until the maximum polynomial level is reached.

Static analysis models MUST have sufficient constraint

Mechanica’s color fringe plots are “contour plots”

Elements near singularities may be excluded – Mechanica would ignore the stress and displacement data of the excluded elements in evaluation of “measures” of the solution quality