- Mapdl.layer(num='', **kwargs)#
Specifies the element layer for which data are to be processed.
APDL Command: LAYER
N - The layer number to process. The default value is 0.
FCMAX - Processes the layer with the largest failure criteria.
Specifies the element layer for which results data are to be listed, plotted, or otherwise processed.
Applies to stress and strain data for layered elements SHELL163, SHELL181, SHELL281, ELBOW290, SOLID185, SOLID186, SOLSH190, SHELL208, SHELL209, REINF264, and REINF265; heat flux and heat gradient for SHELL131 and SHELL132.
The SHELL command may then be used (with shell elements) to specify a location (TOP, MID, BOT) within the layer for output. (The SHELL command does not apply to thermal shell elements SHELL131 and SHELL132.) Transverse shear stresses for MID are linearly averaged from TOP and BOT, and do not reflect a parabolic distribution. Setting KEYOPT(8) = 2 for SHELL181, SHELL281, SHELL208, SHELL209, and ELBOW290 writes the mid-surface values directly to the results file and yields more accurate values than linear averaging.
Because energy is a per-element quantity, you cannot use this command for energy output.
When using the LAYER command with SHELL181, SOLID185, SOLID186, SOLSH190, SHELL208, SHELL209, SHELL281, and ELBOW290, KEYOPT(8) must be set to 1 (or 2 for SHELL181, SHELL281, ELBOW290, SHELL208, and SHELL209) in order to store results for all layers.
When NUM = FCMAX, you must provide the failure criterion input. If specifying input via the FC command, all structural elements are processed. For more information, see the documentation for the FC command.
Use this command with RSYS,LSYS to display results in the layer coordinate system for a particular layer.
For the ANSYS LS-DYNA product, this command works differently than described above. For SHELL163, you must first use EDINT during the solution phase to define the integration points for which you want output data. Be aware that the output location for SHELL163 data is always at the integration point, so “top” and “bottom” refer to the top or bottom integration point, not necessarily the top or bottom surface. For more information, see the ANSYS LS-DYNA User’s Guide.