Mechanical APDL Basic Analysis Guide - Ansys

Chapter 5: Solution
TM_INCR=1.5 ! Time increment
*DO,TM,TM_START,TM_END,TM_INCR ! Do for TM from TM_START to TM_END in
! steps of TM_INCR
TIME,TM ! Time value
F,272,FY,FORCE(TM) ! Time-varying force (at node 272, FY)
NSEL,... ! Select nodes on pressure surface
SF,ALL,PRES,PRESSURE(TM) ! Time-varying pressure
NSEL,ALL ! Activate all nodes
NSEL,... ! Select nodes for temperature specification
BF,ALL,TEMP,TEMP(TM) ! Time-varying temperature
NSEL,ALL ! Activate all nodes
SOLVE ! Initiate solution calculations
*ENDDO
See the Command Reference for discussions of the *DO, TIME, F, NSEL, SF, BF, and *ENDDO commands.
You can change the time increment (TM_INCR parameter) very easily with this method. With other methods,
changing the time increment for such complex load histories would be quite cumbersome.
5.8. Terminating a Running Job
You can terminate a running ANSYS job, if necessary, with the help of system functions such as a system
break, issuing a kill signal, or deleting the entry in the batch queue. For nonlinear analyses, however, this is
not the preferred method, because a job terminated in this manner cannot be restarted.
To terminate a nonlinear analysis "cleanly" on a multitasking operating system, create an abort file, named
Jobname.ABT (or, on some case-sensitive systems, jobname.abt), containing the word nonlinear on the
first line, starting in column 1. At the start of an equilibrium iteration, if the ANSYS program finds such a file
in the working directory, the analysis will be stopped and can be restarted at a later time.
Note
If commands are being read using a file specified via the /INPUT command (Main Menu> Preprocessor>
Material Props> Material Library, or Utility Menu> File> Read Input from), the
abort file will terminate the solution, but the program will continue to read commands from the
specified input file. Thus, any postprocessing commands included in the input file will execute.
5.9. Restarting an Analysis
Occasionally, you may need to restart an analysis after the initial run has been completed. For example, you
may want to add more load steps to the analysis. These may be additional loading conditions in a linear
static analysis or additional portions of a time-history loading curve in a transient analysis. Or, you may need
to recover from a convergence failure in a nonlinear analysis.
ANSYS allows a multiframe restart for structural static, structural transient (full or mode-superposition
methods), and thermal analyses. Distributed ANSYS supports multiframe restarts for nonlinear and full transient
analyses. You can also re-run a VT Accelerator analysis using information available from a previous run.
The multiframe restart can resume a job at any point in the analysis for which information is saved, allowing
you to perform multiple analyses of a model and gives you more options for recovering from an abnormal
termination.
Rerunning an analysis completed with VT Accelerator can reduce the number of iterations needed to obtain
the solution for all load steps and substeps. Rerunning a VT Accelerator analysis is described in VT Accelerator
Re-run (p. 123).
116
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.