When restarting a simulation using the results of a previous
analysis, you specify the particular point in the simulation's load history
from which to restart the analysis.
The model used in the restart analysis, however, must be the same
as the model used in the original analysis up to the restart location.
Specifically,
the restart analysis model must not modify or add any geometry, mesh,
materials, sections, beam section profiles, material orientations, beam section
orientations, interaction properties, or constraints that are already defined
in the original analysis model; and
similarly, it must not modify any step, load, boundary condition,
predefined field, or interaction at or before the restart location.
You may, however, define new sets and amplitude curves in the restart
analysis model.
Continuing an interrupted
run
The restart analysis continues directly from the specified step and
increment of the previous analysis. If the given step and increment do not
correspond to the end of the previous analysis (for example, if the analysis
was interrupted by a computer malfunction),
Abaqus
will try to finish the original step before trying to simulate any new steps.
In
Abaqus/Explicit
in cases where restart is being performed simply to continue a long step (which
might have been terminated because the time limit for the job was exceeded, for
example), you can restart the run by using the Recover job
type as shown in
Figure 1.
Figure 1. Recover job type.
Continuing
with additional steps
If the previous analysis completed successfully and, having viewed the
results, you want to add additional steps to the load history, the specified
step and increment should be the last step and last increment of the previous
analysis.
Changing an
analysis
Sometimes, having viewed the results of the previous analysis, you may want
to restart the analysis from an intermediate point and change the remaining
load history in some manner—for example, to add more output requests, to change
the loading, or to adjust the analysis controls. This can be necessary, for
example, when a step has exceeded its maximum number of increments. If an
analysis is restarted because the maximum number of increments has been
exceeded,
Abaqus/Standard
thinks that the analysis is partway through a step, tries to complete the step,
and promptly exceeds the maximum number of increments again.
In such situations you should indicate that the current step should be
terminated at the specified step and increment. The simulation may then
continue with the new steps. For example, if a step allowed only a maximum of
20 increments, which was less than the number necessary to complete the step, a
new step should be defined in which the entire step definition, including
applied loads and boundary conditions, is identical to that specified in the
original run with the following exceptions:
The number of increments should be increased.
The total time of the new step should be the total time of the original
step less the time completed in the first run. For example, if the time of the
step as originally specified was 100 seconds and the analysis ran out of
increments at a step time of 20 seconds, the duration of the step in the
restart analysis should be 80 seconds.
Any amplitude definitions specified in terms of step time need to be
respecified to reflect the new time scale of the step. Amplitude definitions
specified in terms of total time do not need to be changed, provided the
modifications given above are used.
The magnitudes of any loads or prescribed boundary conditions remain
unchanged since they are always total values in general analysis steps.
