Writing Restart Files
If you want to be able to restart an analysis, you must request restart
output. This output will be written to files that can be used to restart the
analysis. If you do not request that restart data be written, restart files
will not be created in
Abaqus/Standard,
while in
Abaqus/Explicit
a state file will be created with results at only the beginning and end of each
step.
In
Abaqus/Standard
these files are the restart
(job-name.res; file size
limited to 16 gigabytes), analysis database (.mdl and
.stt), part (.prt), output database
(.odb), and linear dynamics and substructure database
(.sim) files. In
Abaqus/Explicit
these files are the restart
(job-name.res; file size
limited to 16 gigabytes), analysis database (.abq,
.mdl, .pac, and
.stt), part (.prt), selected results
(.sel), and output database (.odb)
files. These files, collectively referred to as the restart files, allow an
analysis to be completed up to a certain point in a particular run and
restarted and continued in a subsequent run. The output database file only
needs to contain the model data; results data are not required and can be
suppressed.
You can control the amount of data written to the restart files, as
described below. The amount of data written to the restart file can be changed
from step to step if you include the restart request in each step definition.
Restart information is not written during the following linear perturbation
steps:
Controlling the Frequency of Output to the Restart Files
You can specify the frequency at which data will be written to the
Abaqus/Standard
restart file and the
Abaqus/Explicit
state files. The variables to be written cannot be specified; a complete set of
data is written each time. Therefore, the restart files can be quite large
unless you control the frequency with which restart information is written. If
restart information is requested for an
Abaqus/Standard
analysis at exact time intervals,
Abaqus/Standard
will obtain a solution each time data are written. In this case if the
frequency of output to the restart file is high, the number of increments and,
consequently, the computational cost of the analysis may increase considerably.
Specifying the Frequency of Output to the Abaqus/Standard Restart File in Increments
By default,
Abaqus/Standard
will write data to the restart file after each increment at which the increment
number is exactly divisible by a user-specified frequency value,
N, and at the end of each step of the analysis (regardless
of the increment number at that time). In a direct cyclic or a low-cycle
fatigue analysis
Abaqus/Standard
will write data to the restart file only at the end of a loading cycle;
therefore,
Abaqus/Standard
will write data to the restart file after each iteration (or cycle in a
low-cycle fatigue analysis) at which the iteration number (or cycle number in a
low-cycle fatigue analysis) is exactly divisible by N and
at the end of each step of the analysis.
Specifying the Frequency of Output to the Abaqus/Standard Restart File in Time Intervals
Abaqus/Standard
can divide the step into a user-specified number of time intervals,
n, and write the results at the end of each
interval, for a total of n points for the step. If
n is specified, by default data will be written to
the results file at the exact times calculated by dividing the step into
n equal intervals. Alternatively, you can choose to
write the information at the increment ending immediately after the time
dictated by each interval.
You can specify the frequency of restart output in time intervals only for
the procedures listed in
Table 1.
In addition, this capability is not supported for linear perturbation analyses.
Time Incrementation
If the output frequency is specified in terms of the number of intervals,
Abaqus/Standard
will adjust the time increments to ensure that data are written at the exact
time points specified. In some cases
Abaqus
may use a time increment smaller than the minimum time increment allowed in the
step in the increment directly before a time point. However,
Abaqus
will not violate the minimum time increment allowed for consolidation,
transient mass diffusion, transient heat transfer, transient couple
thermal-electrical, transient coupled temperature-displacement, and transient
coupled thermal-electrical-structural analyses. For these procedures if a time
increment smaller than the minimum time increment is required,
Abaqus
will use the minimum time increment allowed in the step and will write restart
data at the first increment after the time point.
When the output frequency is specified in terms of the number of
intervals, the number of increments necessary to complete the analysis might
increase, which might adversely affect performance.
Specifying the Frequency of Output to the Abaqus/Explicit State File
Abaqus/Explicit
will divide the step into a user-specified number of time intervals,
n, and write the results at the beginning of the
step and at the end of each interval, for a total of
n+1 points for the step, with the last point
matching the end of the step. By default, the results will be written to the
state file at the increment ending immediately after the time dictated by each
interval. Alternatively, you can choose to write the results at the exact times
calculated by dividing the step into n equal
intervals.
If a problem precludes the analysis from continuing to completion, such as
if an element becomes excessively distorted,
Abaqus/Explicit
will attempt to save the last completed increment in the state file.
Alternatively, you can specify the number of intervals as zero to turn off
all restart frame output. This setting can be used to reduce the disk usage if
there is no continuation after the current analysis.
Synchronizing Restart Information Written in a Co-Simulation
Restart output must be synchronized between co-simulation analyses for a
co-simulation restart to be successful. To achieve this synchronization, it is
recommended that you request that restart data are written at a specified
number of time intervals, n. In this case
Abaqus/Standard
and
Abaqus/Explicit
will write restart information at the co-simulation target time immediately
after the time dictated by each interval. If you specify the frequency of
output for restart data in increments, it is very difficult to synchronize the
writing of restart information, and the restart analysis may start from two
different time points, possibly leading to an imbalance.
Controlling the Precision of Output to the Abaqus/Explicit State File
By default,
Abaqus/Explicit
writes to the state file in double precision when the analysis is run in double
precision. Alternatively, you can choose to write data to the state file in
single precision if you want to reduce the size of the state file. This option
may cause noisy results between step boundaries or for the first step of a
restart analysis. If
Abaqus/Explicit
is run in single precision, this control parameter is ignored and single
precision is always used.
Overlaying Results in the Restart Files
For an
Abaqus/Standard
or
Abaqus/Explicit
analysis, you can specify that only one increment (or one iteration in the case
of a direct cyclic analysis) per step should be retained in the
Abaqus/Standard
restart file or
Abaqus/Explicit
state file, thus minimizing the size of the files. As the data are written,
they overlay the data from the previous increment (or iteration), if any,
written for the same step. You can specify whether or not the data should be
overlaid for each step individually. Since in
Abaqus/Explicit
the results are written by default only at the end of the step, it is
recommended to overlay the data in conjunction with specifying a number of time
intervals at which data are written; in this way the data in the restart file
are advanced as dictated by the number of intervals used.
To protect you from losing data if your system crashes, when
Abaqus/Standard
writes a frame from a given increment, it does not strictly overwrite the frame
from the last saved increment. Instead, it always keeps a reserve frame and
only frees a given saved frame for overwriting when the next frame is secured
on the file. This reserve frame is not deleted unless the space is required for
later increments. This process produces a bonus frame in the last step of an
analysis if overlaying is occurring in that step and if the analysis completes
successfully; users will observe that the penultimate restart frame is also
retained for the last step, even though overlay is being used.
The advantage of overlaying the restart data is that it minimizes the space
required to store the restart files.
Restarting an Analysis
You restart (continue) an analysis by specifying that the restart or state,
analysis database, and part files created by the original analysis be read into
the new analysis. The restart files must be saved upon completion of the first
job. In
Abaqus/Explicit
the package (.pac) file and the selected results
(.sel) file are also used for restarting an analysis and
must be saved upon completion of the first job. Since restart files can be very
large, sufficient disk space must be provided (in
Abaqus/Standard
the
analysis input file processor
estimates the space that is required for the restart file).
You can specify the point at which the analysis is continued in the new run,
as discussed below.
An
Abaqus/Standard
analysis cannot be restarted from the linear perturbation steps listed in
Writing Restart Files.
An
Abaqus/Explicit
analysis cannot be restarted from an anneal step.
In addition, if an
Abaqus/Standard
or
Abaqus/Explicit
analysis is terminated abruptly by an operating system command or due to a
power failure, it is unlikely that the job can be recovered or restarted. In
this situation, files that are open during the analysis process are not closed
properly, which may result in loss of data and incomplete files.
Identifying the Analysis to Be Restarted
In an
Abaqus/Standard
restart analysis you must specify the name of the restart file that contains
the specified step and increment, iteration (for a direct cyclic analysis), or
cycle (for a low-cycle fatigue analysis). In an
Abaqus/Explicit
restart analysis you must specify the name of the state file that contains the
specified step and interval.
Abaqus
issues an error message if the step and increment, iteration, cycle, or
interval number at which restart is requested do not exist in the specified
restart or state file.
Specifying the Restart Point
You can specify the point (step and increment, iteration, cycle, or
interval) in the previous analysis from which to restart. Truncating a step in
the previous analysis when you restart is discussed below.
Specifying the Restart Point for an Abaqus/Standard Analysis (Except When Restarting from a Direct Cyclic or a Low-Cycle Fatigue Analysis)
An
Abaqus/Standard
analysis restarted from any analysis other than a direct cyclic or a low-cycle
fatigue analysis will continue the analysis immediately after the
user-specified step and increment. If you do not specify a step or increment,
the analysis will restart at the last available step and increment found in the
restart file.
Specifying the Restart Point for an Abaqus/Standard Analysis Restarted from a Direct Cyclic Analysis
An
Abaqus/Standard
analysis restarted from a previous direct cyclic analysis can be restarted only
from the end of a loading cycle. In this case you should specify the step and
iteration number at which the new analysis will be resumed.
In a direct cyclic analysis that has not reached a stabilized cycle upon
restart, you can increase the number of iterations or Fourier terms, thus
allowing continuation of an analysis (see
Direct Cyclic Analysis).
Specifying the Restart Point for an Abaqus/Standard Analysis Restarted from a Low-Cycle Fatigue Analysis
An
Abaqus/Standard
analysis restarted from a previous low-cycle fatigue analysis can be restarted
only from the end of a loading cycle. In this case you should specify the step
and cycle number at which the new analysis will be resumed.
Specifying the Restart Point for an Abaqus/Explicit Analysis
An
Abaqus/Explicit
restart analysis will continue the analysis immediately after the
user-specified step and interval. You must specify the step from which an
Abaqus/Explicit
restart analysis will continue. If you do not specify an interval from which to
restart or that the current step should be terminated at a specified interval,
the analysis is restarted from the last interval available in the state file
for the specified step.
Continuing an Analysis without Changes
To continue an analysis without changes, only the steps subsequent to the
step at which restart is being made should be defined in the restart analysis.
All other information has been saved to the restart files. This feature cannot
be used for an
Abaqus
analysis that uses the co-simulation technique.
Continuing an Abaqus/Standard Analysis without Changes
In
Abaqus/Standard, 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), the data for the restart run may simply consist of the request to
read restart data from another analysis.
Continuing an Abaqus/Explicit Analysis without Changes
In
Abaqus/Explicit,
in cases where restart is being performed simply to continue a long step (which
might have been terminated because a CPU time
limit was exceeded, for example), do not use a restart analysis; instead, use a
recover analysis. In this case no data are needed (unless user subroutines are
being used).
Truncating a Step
You can truncate an analysis step prior to its completion when you restart
the analysis. For example, by default, if the previous analysis is an
Abaqus/Standard
procedure and you specify that the restart point is Step
p, the restart analysis will restart from the last
saved increment of Step p and continue the step to
completion. However, if you specify that the restart point is increment
n of Step p and that the
step should be terminated before restart, the restart analysis will restart
from increment n of Step
p, end Step p at that
point, and continue with newly defined steps. In this case the step from which
the analysis is being restarted will be truncated at the time of restart,
regardless of the step end time that had been given in the previous analysis.
Thus, the step is considered to be completed even though all of the loading may
not have been applied. Continuation of the analysis will be defined by history
data provided in the restart run.
When you truncate an analysis step in an
Abaqus/Explicit
restart analysis, you must specify the interval after which the analysis should
be restarted.
If the step from which the restart is being made completed normally, you can
truncate the step to restart within the step so that you can request additional
output, write to the restart file with a higher frequency, etc. In
Abaqus/Explicit
it may be necessary to truncate an analysis step when an unforeseen event
occurs within a step; for example, if contact surface definitions require
modification due to unforeseen displacements. If the step from which the
restart is being made completed normally and the restart is being made from the
last increment, iteration, or interval, truncating the analysis step will have
no effect.
If the restart is being made from a job that was truncated by the operating
system (for example, because of insufficient disk space, run-time limit
exceeded, etc.), you will usually not choose to truncate the analysis step, so
that the old step will first be completed before a new step—if any exists—is
started. If restart is being made from the end of a step that terminated
prematurely inside
Abaqus
(for example, because it ran out of increments or it failed to converge), you
must truncate the step and include a new step definition. If you do not
truncate the step,
Abaqus
will try to continue the old step upon restart and will terminate the analysis
in the same manner as before.
Amplitude References
Care should be taken if loads and boundary conditions refer to amplitude
curves (Amplitude Curves).
If the amplitude is given in terms of total time, the loads and boundary
conditions will continue to be applied according to the amplitude definition.
However, if the amplitude is given in terms of step time (default), the loads
and boundary conditions will be held constant at their values at the time the
step is terminated.
Temperatures, field variables, and mass flow rates applied in the old step
will remain in the new step if they are not redefined. If an amplitude curve
was not specified, these quantities will continue to be applied according to
the default amplitude for the procedure.
Automatic Stabilization in Abaqus/Standard
In
Abaqus/Standard
care should be exercised when automatic stabilization is active at the point at
which a step is truncated. This may happen either in the middle of quasi-static
procedures using automatic stabilization (see
Solving Nonlinear Problems)
or during contact analyses using automatic viscous damping (see
Adjusting Contact Controls in Abaqus/Standard).
In such cases viscous forces may be present, which will not be carried over to
the subsequent step, therefore causing convergence difficulties.
In the case of quasi-static procedures using automatic stabilization it is
recommended that the stabilization continue to be enforced during the following
step and that you specify the damping factor directly, using the last value
printed out by
Abaqus/Standard
in the message file. In the case of automatic viscous damping in a contact pair
when contact has not yet been fully established, it is recommended that the
damping be applied again, although there is no guarantee that the amount of
damping applied will be the same as in the original step.
Choosing the Initial Time Increment for an
Abaqus/Standard
Restart Analysis
In
Abaqus/Standard
take care in choosing the time period and initial time increment for the new
step if the previous step was truncated. In transient analyses the initial time
increment for the new step should be similar to the time increment that was
used at the point of restart in the old step. In quasi-static analyses choose
the initial time increment of the new step so that the increments in loads or
prescribed boundary conditions are similar to those at the point of restart in
the old step.
In a nonlinear analysis the increment of load applied in the first
increment of the restart run should be similar to that applied in the last
converged increment of the previous run. Let
-
= the load to be applied in the first increment of the restart run,
-
= the remaining load to be applied in the restart run,
-
= the initial time increment for the restart run, and
-
= the total step time for the first step of the restart run.
The following equation can then be used to determine the initial time
increment for the restart run:
Example
Suppose an
Abaqus/Standard job
stopped running because it reached the maximum number of increments specified
for the step. The original input file was as follows:
HEADING
…
STEP, INC=4
STATIC, DIRECT
0.1, 1.0
CLOAD
1, 2, 20.0
RESTART, WRITE, FREQUENCY=2
END STEP
This run ended at Step 1, increment 4 with a load of 8.0 applied. The
following input file could be used to restart this job and to complete the
loading:
HEADING
RESTART, READ, STEP=1, INC=4, END STEP
STEP, INC=120
STATIC, DIRECT
0.1, 0.6
CLOAD
1, 2, 20.0
END STEP
Notice that the concentrated load applied is the same as in the previous
step.
In this example assume that a load increment of 2.0 was applied in the
last converged increment of the previous run. Therefore, the initial time
increment for the restart run is chosen such that the load increment applied
during the first increment is also 2.0. The remaining load to be applied in the
restart run is 12.0 (20.0 total − 8.0 applied in the previous run).
Substitution into the equation for the initial time increment yields
= /6.
The step time for the first step of the restarted job,
,
is chosen to be 0.6 so that the total accumulated time is 1.0 when the applied
load is 20.0 (at the end of the step). Thus, the initial time increment for the
restart run, ,
is set equal to 0.1.
Supplying Additional Data in the Restart Analysis
It is possible to define steps subsequent to the step at which restart is
being made. It is also possible to supply new amplitude definitions, new
surfaces, new node sets, and new element sets during the restart analysis.
Existing sets cannot be modified.
In Abaqus/Standard additional surfaces defined in the model part of a restart analysis have the
restriction that they can be referenced only from surface-based loading definitions or
output requests for user-defined surface sections (see Output to the Data and Results Files).
Example
For example, suppose a one-step
Abaqus/Explicit job
stopped prior to completion because a CPU time
limit was exceeded and you have decided that a second step should be added with
new boundary condition definitions. The following input file could be used to
restart this job, complete the remaining part of Step 1, and complete Step 2:
HEADING
RESTART, READ, STEP=1
**
** This defines Step 2
**
STEP
DYNAMIC, EXPLICIT
, .003
BOUNDARY, OP=NEW
…
END STEP
Continuation of Optional History Data in Restart Analyses
The rules governing the continuation of optional analysis history
data—loading, boundary conditions, output controls, and auxiliary controls (see
Abaqus Model Definition)—are
the same for the steps defined in the restart analysis and the original
analysis. For a discussion of the rules governing the continuation of optional
history data, see
Defining an Analysis.
Prescribing Predefined Fields in the Restart Analysis
It is possible to prescribe predefined fields (see
Predefined Fields)
in the restart analysis.
To specify predefined temperatures or field variables in an
Abaqus/Standard restart
analysis, the corresponding predefined field must have been specified in the
original analysis as initial temperatures or field variables (Initial Conditions)
or as predefined temperatures or field variables (Predefined Fields).
Restarting with User Subroutines
User subroutines are not written to the
Abaqus/Standard
restart file or to the
Abaqus/Explicit
state file. Therefore, if the original analysis contained any user subroutines,
these subroutines must be included again in the restart run or when recovering
additional results output from restart data (see
Recovering Additional Results Output from Restart Data in Abaqus/Standard).
These subroutines can be modified on restart; however, modifications should be
made with caution because they may invalidate the solution from which the
restart is being made.
Simultaneously Reading and Writing a Restart File
You can continue a previous analysis as a restart analysis and write the
results from the restart analysis to a new restart file or state file. For
example, if the previous analysis is an
Abaqus/Explicit
procedure and in the current analysis you specify that the restart point is
Step p and the restart output frequency is
n, the analysis will be restarted from the last
saved interval of Step p and restart states will be
written in subsequent steps based on the new value of
n.
To discontinue the writing of a restart file in
Abaqus/Standard
when you are restarting a previous analysis, specify a restart output frequency
of 0; if you do not specify a frequency, the file will continue to be written
at the frequency defined for the previous analysis.
The New Restart File
Restart files can be very large for large models or for jobs involving many
restart increments (unless you choose to overlay the restart data—see
Overlaying Results in the Restart Files).
Therefore, the previous restart file is not copied to the beginning of the new
restart file when a job is restarted: only the data at restart increments
requested in the current run are saved to the new restart file. However, if an
eigenfrequency extraction step (Natural Frequency Extraction)
is restarted and additional eigenvalues are requested, the new restart file
will contain those eigenvalues that converged during the first run as well as
the additional eigenvalues.
Example: Abaqus/Standard
Suppose an
Abaqus/Standard job
stopped running because it ran out of disk space. The last complete information
for an increment in the restart file is from Step 2, increment 4. The following
two-line input file could be used to restart this job and continue writing the
restart file:
HEADING
RESTART, READ, STEP=2, INC=4, WRITE
Example: Abaqus/Explicit
Suppose you stopped an
Abaqus/Explicit job
because too much output was being generated. The last information in the state
file is from Step 2, Interval 4 at a time of .004. Step 2 has a time period of
.010 and restart results were requested at 10 intervals. The following input
file could be used to restart this job and redefine the remainder of the step
with reduced output requests:
HEADING
RESTART, READ, END STEP, STEP=2, INTERVAL=4
STEP
DYNAMIC, EXPLICIT
, .006
RESTART, WRITE, NUMBER INTERVAL=2
END STEP
Continuation of Output upon Restart
When you restart an analysis,
Abaqus
creates a new output database file
(job-name.odb) and a new
results file (job-name.fil) and
writes output data to those files according to the criteria described below.
Output Database (.odb) Files
The
Abaqus
output database file
(job-name.odb) contains results
that can be used for postprocessing.
By default, the output database file is not made continuous across restarts;
Abaqus
creates a new output database file each time a job is run.
Results (.fil) Files
The
Abaqus
results file created in
Abaqus/Standard
and
Abaqus/Explicit
(job-name.fil) contains
user-specified results that can be used for postprocessing in external
postprocessing packages. In
Abaqus/Explicit
results are also written to the selected results file
(job-name.sel), which is then
converted to the results file for postprocessing. See
About Output
for details.
Upon restart
Abaqus/Standard
will copy the information from the old results file into the results file for
the new job up to the restart point and begin writing the new results to the
new file following that point.
Abaqus/Explicit
will copy the information from the old selected results file into the selected
results file for the new job up to the restart point and begin writing the new
results to the new file following that point.
If the old results file is not provided,
Abaqus/Standard
will continue the analysis, writing the results of the restart analysis only to
the new results file. Therefore, you will have segments of the analysis results
in different files, which should be avoided in most cases since postprocessing
programs assume that the results are in a single continuous file. You can merge
such segmented results files, if necessary, by using the
abaqus append
execution procedure (Joining Results (.fil) Files).
Restart Compatibility
A restart analysis in Abaqus/Standard can use the restart files generated from the same maintenance delivery of the same
general release. Restart may not be compatible between general releases and hotfix releases
within the same general release. In Abaqus/Explicit the original analysis and the restart analysis must use precisely the same release.
A restart analysis in
Abaqus
and a recover analysis in
Abaqus/Explicit
must be run on a computer that is binary compatible with the computer used to
generate the restart files. You should only use restart files generated from
the same maintenance delivery of a general release for a restart analysis.
|