Mechanical APDL Basic Analysis Guide - Ansys

Chapter 8:The Time-History Postprocessor (POST26)
8.2. Entering the Time-History Postprocessor
You enter the time history processor to process time or frequency related results data. Once you have solved
an analysis, ANSYS uses your results data to create a “Results File.” The active results file (*.RST, *.RFL,
*.RTH, *.RMG, etc.) is automatically loaded when you enter postprocessing. If the current analysis contains
no results file, you are queried for one. You can also use the file option to load any other results file for
processing.
8.2.1. Interactive
Selecting Main Menu> TimeHist PostPro starts the time-history postprocessor and loads the time-history
variable viewer. The following discussions of interactive mode deal with the variable viewer portion of the
Graphical User Interface (GUI). Alternate GUI methods are discussed in the appropriate command descriptions.
If you need to reopen the variable viewer while still in the time-history postprocessor, click Variable Viewer
in the TimeHist PostPro menu.
8.2.2. Batch
The command /POST26 opens the time-history postprocessor for batch and command line operations.
Notes:
• You must have your geometry loaded and a valid results file must be available in order to perform timehistory
post processing (interactive or batch)
• By default, the time-history processor looks for one of the results files mentioned in The General Postprocessor
(POST1). You can specify a different file name using the FILE command (batch) or from the
file menu of the variable viewer.
• The data sets and variable definitions you create in the time history postprocessor are maintained for
the current ANSYS session. This allows you to move, for example, between POST1 and POST26 without
losing stored information (see the KEEP command for more information).
• If you define variables outside of the variable viewer, but want to use it for postprocessing, you must
refresh the variable viewer by either pressing the F5 button on your keyboard with the variable viewer
selected, or by choosing the refresh button in the variable viewer's toolbar.
• Use the Clear time-history Data button to remove all defined variables and return settings to their default
values.
8.3. Defining Variables
Your time-history operations deal with variables, tables of result item versus time (or versus frequency). The
result item may be the UX displacement at a node, the heat flux in an element, the force developed at a
node, the stress in an element, the magnetic flux in an element, etc. You assign unique identifiers to each
of your variables. Up to 200 such variables can be defined. TIME is reserved for the time value, and FREQ is
reserved for the frequency value. All other identifiers must be unique, and can be made up of 32 letters and
characters. If you don't supply a unique identifier, ANSYS will assign one. In addition to the unique identifiers,
ANSYS uses numerical indices (reference numbers) to track and manipulate the variables. These numbers
can be used interchangeably with the identifiers at the command level, and in some interactive operations.
The numerical index is displayed, along with any name you choose in the data properties dialog box.
8.3.1. Interactive
Follow these steps to enter time-history data using the variable viewer.
192
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.