Mechanical APDL Basic Analysis Guide - Ansys

Chapter 7: The General Postprocessor (POST1)
Use POST1, the general postprocessor, to review analysis results over the entire model, or selected portions
of the model, for a specifically defined combination of loads at a single time (or frequency). POST1 has many
capabilities, ranging from simple graphics displays and tabular listings to more complex data manipulations
such as load case combinations.
To enter the ANSYS general postprocessor, issue the /POST1 command (Main Menu> General Postproc).
The following POST1 topics are available:
7.1. Reading Results Data into the Database
7.2. Reviewing Results in POST1
7.3. Using the PGR File in POST1
7.4. Additional POST1 Postprocessing
7.1. Reading Results Data into the Database
The first step in POST1 is to read data from the results file into the database. To do so, model data (nodes,
elements, etc.) must exist in the database. If the database does not already contain model data, issue the
RESUME command (Utility Menu> File> Resume Jobname.db) to read the database file, Jobname.DB.
The database should contain the same model for which the solution was calculated, including the element
types, nodes, elements, element real constants, material properties, and nodal coordinate systems.
Caution
The database should contain the same set of selected nodes and elements that were selected
for the solution. Otherwise, a data mismatch may occur. For more information about data mismatches,
see Appending Data to the Database (p. 133).
After model data are in the database, load the results data from the results file by issuing one of the following
commands: SET, SUBSET, or APPEND.
7.1.1. Reading in Results Data
The SET command (Main Menu> General Postproc> Read Results> datatype) reads results data over
the entire model from the results file into the database for a particular loading condition, replacing any data
previously stored in the database. The boundary condition information (constraints and force loads) is also
read in, but only if either element nodal loads or reaction loads are available; see the OUTRES command for
more information. If they are not available, no boundary conditions will be available for listing or plotting.
Only constraints and forces are read in; surface and body loads are not updated and remain at their last
specified value. However, if the surface and body loads have been specified using tabular boundary conditions,
they will reflect the values corresponding to this results set. Loading conditions are identified either by load
step and substep or by time (or frequency). The arguments specified with the command or path identify
the data to be read into the database. For example, SET,2,5 reads in results for load step 2, substep 5. Similarly,
SET,,,,,3.89 reads in results at time = 3.89 (or frequency = 3.89 depending on the type of analysis that
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
131