13.1.4.5. Selecting Elements with a Specific Layer Number
Use the ESEL,S,LAYER command to select elements that have a certain layer number. If an element has
a zero thickness for the requested layer, the element is not selected.
For energy output, the results are applicable only to the entire element. You cannot get output results
for individual layers.
13.1.4.6. Specifying a Layer for Results Processing
Use the LAYER command (in the POST1 postprocessor) or the LAYERP26 (in the POST26 postprocessor)
to specify the layer number for which results should be processed.
The SHELL command specifies a TOP, MID, or BOT location within the layer.
The default in POST1 is to store results for the bottom of the bottom layer, and the top of the top layer,
and the layer with the maximum failure criterion value. In POST26, the default is layer 1.
If KEYOPT(8) = 1 (data stored for all layers), the LAYER and LAYERP26 commands store the TOP and
BOT results for the specified layer number. MID values are then calculated by average TOP and BOT
values.
If KEYOPT (8) = 2 is set for SHELL181 or SHELL281 during SOLUTION, then LAYER and LAYERP26
commands store the TOP, BOTTOM, and MID results for the specified layer number. In this case, MID
values are directly retrieved from the results file. For transverse-shear stresses with KEYOPT(8) = 0,
therefore, POST1 can only show a linear variation, whereas the element solution printout or KEYOPT(8)
= 2 can show a parabolic variation.
13.1.4.7. Transforming Results to Another Coordinate System
By default, the POST1 postprocessor displays all results in the global Cartesian coordinate system. Issue
the RSYS command to transform the results to a different coordinate system. In particular,RSYS,SOLU
allows you to display results in the layer coordinate system if LAYER is issued with a nonzero layer
number.
13.2. The FiberSIM-ANSYS Interface
FiberSIM (a product of Vistagy, Inc.) is a fiber draping tool used within popular CAD systems. FiberSIM
provides accurat e fiber paths for structural analysis, allows you to optimize potential laminate architec-
tures, and generat es flat patterns for product definition.
The FiberSIM-ANSYS interface allows you to use the information contained in a FiberSIM .xml file in
your ANSYS model. (ANSYS does not use FiberSIM .fml files.) Generated by FiberSIM's draping calcu-
lations, the .xml file data contains the order of layers (including dropped layer information) and the
layer orientation. In ANSYS, you supplement that information by adding material and thickness inform-
ation to each layer via ANSYS section (SECxxx) commands.
Elements Supported
The FiberSIM-ANSYS interface applies to the following elements only:SHELL181,SOLID185 Layered
Solid,SOLID186 Layered Solid,SOLSH190, and SHELL281. When using solid elements, only one solid
element thru the thickness should be used. The interface does not support the VT Accelerator or ANSYS
DesignXplorer products.
Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential informationComposites