Mechanical APDL Basic Analysis Guide - Ansys

Chapter 7:The General Postprocessor (POST1)
transformation of results data), you may see some unexpected results such as negative values after a square
operation or negative values even when you request absolute values.
This feature is mainly intended for reading in data from your own, special-purpose program. By writing
output data from that program in the form of the above commands, you can read them into POST1 and
process them the same way you would ANSYS results. If you do have an ANSYS results file, it will not be
affected by these commands.
7.4.6. Splitting Large Results Files
If you have a results file that is too large for you to postprocess on your local machine (such as from running
a large model on a server or cluster), you can split the results file into smaller files based on subsets of the
model. You can then process these smaller files on your local machine. For example, if your large model is
an assembly, you can create individual results files for each part.
You can also use this capability to create a subset of results for efficient postprocessing. For example, you
could take the results file from a large model that had all results written, and create a smaller results file
containing only stresses on the exterior surface. This smaller file would load and plot quickly, while not losing
any of the detailed data written to the full results file.
When you use this feature, the subset geometry is also written to the results file so that you do not need
the database file (no SET required). However, you must not resume any database when postprocessing one
of these results files, and your original results file must have the geometry written to it (i.e., do not issue
/CONFIG,NORSTGM,1).
To use the results file splitting feature:
Command(s): RSPLIT
GUI: Main Menu> General Postproc>
You can use this feature in conjunction with INRES to limit the amount of data written to the results files.
A brief example of how you might use this feature is shown below:
/POST1
FILE,jobname,rst ! Import *.rst file
ESEL,all
INRES,nsol,strs ! Write out only nodal solution and stresses
RSPLIT,ext,esel,myexterior ! Write the results for the exterior of the whole model to a file
! named myexterior.rst
FINISH
/EXIT
...
/POST1
FILE,myexterior
PLNS,s,eqv ! Postprocess the myexterior.rst file as usual
PLNS,u,sum
FINISH
7.4.7. Magnetics Command Macros
The following ANSYS magnetic command macros are also available for calculating and plotting results from
a magnetic analysis:
• CURR2D (Main Menu> General Postproc> Elec&Mag Calc> Element Based> Current) calculates
current flow in a 2-D conductor.
• EMAGERR (Main Menu> General Postproc> Elec&Mag Calc > Element Based> Error Eval) calculates
the relative error in an electrostatic or electromagnetic field analysis.
182
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.