METBD 450 Lecture Notes: P-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.

Advantages of p-elements	Disadvantages of p-elements
- can capture more complex behavior with a coarser mesh than h-elements	- are resource intensive, both computer memory and disk space
- are better suited to automatic adaptivity than h-elements (in ANSYS we have adapt.mac - manual adaptivity)	- cannot model nonlinear behavior (plasticity, large deflections, creep, stress stiffening, etc.) - This restriction is changing as the theory develops.
- easy to use (?)	- cannot model transient (time dependent) systems
- error estimates can be calculated locally (as well as globally) in the model	- cannot be mixed with h-elements
	- all p-elements must have mid-side nodes

In the ANSYS Main Menu > Preferences > Set the "Structural Discipline Option" for p-Method (/PMETH,ON command). Then ANSYS will only show you the p-elements and related modeling information.
Otherwise, manually change to a p-element type by typing the element type command in the Input Window: ET,1,PLANE145. (If preferences are default, i.e., h-Method, then the p-element family is not seen in the ANSYS element library, but may be activated manually)

set the P-Range: PPRANG, the global min. and max. p-levels (Defaults: 2 and 8)
set the Solution Option: PMOPTS used to "freeze" or "fix" the p-level of elements whose strain energy error is less than the tolerance (Default: 5%)
set the Convergence Criteria: PCONV can set the global criteria for strain energy error (Default: 5%). Also, sets the criteria for stress, strain, or deflection at node points on the model (Local for Solids/Shells)
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 !!! Look in the Output Window.
In Postprocessing under Plot Results, check

the p-Convergence: for the specific criteria you set in solution
the p-Levels: to see what polynomial level was used for each element in the model.
use Read Results > Last Set (SET command) before plotting other quantities
- "normal" results like: deformed shape, stress contours, reaction forces, etc.
adjust plot facets (display accuracy) for smoother contours using:
- PlotCtrls > Style > Size and Shape, OR
- Postprocessing > Options for Output, OR
- simply type in the /EFACET command