김경종
187 lines
16 KiB
Markdown
187 lines
16 KiB
Markdown
<!-- source-page: 631 -->
|
||
|
||
# 9. Analysis Continuation Techniques
|
||
|
||
Restarting an analysis 9.1
|
||
|
||
Importing and transferring results 9.2
|
||
|
||
<!-- source-page: 632 -->
|
||
|
||
<!-- source-page: 633 -->
|
||
|
||
# 9.1 Restarting an analysis
|
||
|
||
• “Restarting an analysis,” Section 9.1.1
|
||
|
||
<!-- source-page: 634 -->
|
||
|
||
<!-- source-page: 635 -->
|
||
|
||
# 9.1.1 RESTARTING AN ANALYSIS
|
||
|
||
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Output,” Section 4.1.1
|
||
• \*RESTART
|
||
• “Restarting an analysis,” Section 19.6 of the Abaqus/CAE User’s Guide
|
||
|
||
# Overview
|
||
|
||
When you run an analysis, you can write the model definition and state to the files required for restart. Scenarios for using the restart capability include:
|
||
|
||
• Continuing an interrupted run: If an analysis is interrupted by a computer malfunction, the Abaqus restart analysis capability allows the analysis to complete as originally defined.
|
||
• Continuing with additional steps: After viewing results from a successful analysis, you may decide to append steps to the load history.
|
||
• 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 data in some manner. In addition, you may want to add additional steps to the load history if the previous analysis completed successfully.
|
||
|
||
“Output,” Section 4.1.1, describes the process of obtaining results output from an Abaqus/Standard restart file.
|
||
|
||
# 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 and Abaqus/CFD 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. In Abaqus/CFD these files are the restart and analysis database (job-name.sim) 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.
|
||
|
||
<!-- source-page: 636 -->
|
||
|
||
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:
|
||
|
||
• “Static stress analysis,” Section 6.2.2 (perturbation)
|
||
• “Eigenvalue buckling prediction,” Section 6.2.3
|
||
• “Direct-solution steady-state dynamic analysis,” Section 6.3.4
|
||
• “Complex eigenvalue extraction,” Section 6.3.6
|
||
• “Transient modal dynamic analysis,” Section 6.3.7
|
||
• “Mode-based steady-state dynamic analysis,” Section 6.3.8
|
||
• “Subspace-based steady-state dynamic analysis,” Section 6.3.9
|
||
• “Response spectrum analysis,” Section 6.3.10
|
||
• “Random response analysis,” Section 6.3.11
|
||
• “Eddy current analysis,” Section 6.7.5
|
||
|
||
Input File Usage: Use the following option to request that restart data be written for an analysis: \*RESTART, WRITE
|
||
|
||
The \*RESTART, WRITE option can be used as either model data or history data.
|
||
|
||
Abaqus/CAE Usage: Step module: Output→Restart Requests
|
||
|
||
In Abaqus/CAE restart requests are always associated with a particular step; you cannot define a restart request for the entire analysis. Restart requests are created by default for every step; restart requests for Abaqus/Standard and Abaqus/CFD steps have a default frequency of 0, while restart requests for Abaqus/Explicit steps have a default number of intervals of 1.
|
||
|
||
# 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 and Abaqus/CFD 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,
|
||
|
||
<!-- source-page: 637 -->
|
||
|
||
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.
|
||
|
||
Input File Usage: \*RESTART, WRITE, FREQUENCY=N By default, N=1.
|
||
|
||
Abaqus/CAE Usage: Step module: Output→Restart Requests: enter N in the Frequency column for each step By default, N=0 (no restart information is written).
|
||
|
||
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 9.1.1–1. In addition, this capability is not supported for linear perturbation analyses.
|
||
|
||
Input File Usage: Use the following option to request results at the exact time intervals: \*RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=YES
|
||
|
||
Use the following option to request results at the increments ending immediately after each time interval:
|
||
|
||
\*RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=NO
|
||
|
||
Abaqus/CAE Usage: Step module: Output→Restart Requests: enter n in the Intervals column; toggle on the Time Marks column for each step if you want the results written at the exact time intervals
|
||
|
||
Table 9.1.1–1 List of Abaqus/Standard procedures that support restart at time intervals.
|
||
|
||
<table><tr><td>Procedure</td><td>Time incrementation</td><td>Restart at exact time intervals</td><td>Restart at approximate time intervals</td></tr><tr><td rowspan="2">“Static stress analysis,” Section 6.2.2 (except if the Riks method is used)</td><td>Automatic</td><td>√</td><td>√</td></tr><tr><td>Fixed</td><td>—</td><td>√</td></tr><tr><td rowspan="2">“Implicit dynamic analysis using direct integration,” Section 6.3.2</td><td>Automatic</td><td>√</td><td>√</td></tr><tr><td>Fixed</td><td>—</td><td>√</td></tr></table>
|
||
|
||
<!-- source-page: 638 -->
|
||
|
||
<table><tr><td>Procedure</td><td>Time incrementation</td><td>Restart at exact time intervals</td><td>Restart at approximate time intervals</td></tr><tr><td rowspan="2">“Uncoupled heat transfer analysis,” Section 6.5.2 (except if you specify that the analysis end when steady state is reached)</td><td>Automatic</td><td>√</td><td>√</td></tr><tr><td>Fixed</td><td>—</td><td>√</td></tr><tr><td rowspan="2">“Mass diffusion analysis,” Section 6.9.1 (except if you specify that the analysis end when steady state is reached)</td><td>Automatic</td><td>√</td><td>√</td></tr><tr><td>Fixed</td><td>—</td><td>√</td></tr><tr><td rowspan="2">“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 (except if you specify that the analysis end when steady state is reached)</td><td>Automatic</td><td>√</td><td>√</td></tr><tr><td>Fixed</td><td>—</td><td>√</td></tr><tr><td rowspan="2">“Fully coupled thermal-stress analysis,” Section 6.5.3</td><td>Automatic</td><td>√</td><td>√</td></tr><tr><td>Fixed</td><td>—</td><td>√</td></tr><tr><td rowspan="2">“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4</td><td>Automatic</td><td>√</td><td>√</td></tr><tr><td>Fixed</td><td>—</td><td>√</td></tr><tr><td rowspan="2">“Coupled thermal-electrical analysis,” Section 6.7.3 (except if you specify that the analysis end when steady state is reached)</td><td>Automatic</td><td>√</td><td>√</td></tr><tr><td>Fixed</td><td>—</td><td>√</td></tr><tr><td rowspan="2">“Steady-state transport analysis,” Section 6.4.1</td><td>Automatic</td><td>√</td><td>√</td></tr><tr><td>Fixed</td><td>—</td><td>√</td></tr><tr><td>“Subspace-based steady-state dynamic analysis,” Section 6.3.9</td><td>Fixed</td><td>—</td><td>√</td></tr><tr><td rowspan="2">“Quasi-static analysis,” Section 6.2.5</td><td>Automatic</td><td>√</td><td>√</td></tr><tr><td>Fixed</td><td>—</td><td>√</td></tr></table>
|
||
|
||
# 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,
|
||
|
||
<!-- source-page: 639 -->
|
||
|
||
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.
|
||
|
||
Input File Usage: Use the following option to request results at the increments ending immediately after each time interval:
|
||
|
||
\*RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=NO
|
||
|
||
Use the following option to request results at the exact time intervals:
|
||
|
||
\*RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=YES
|
||
|
||
By default, n=1.
|
||
|
||
Use the following option to turn off all restart frame output:
|
||
|
||
\*RESTART, WRITE, NUMBER INTERVAL=0
|
||
|
||
Abaqus/CAE Usage: Step module: Output→Restart Requests: enter n in the Intervals column; toggle on the Time Marks column for each step if you want the results written at the exact time intervals By default, n=1.
|
||
|
||
Turning off all restart frame output is not supported in Abaqus/CAE.
|
||
|
||
# Specifying the frequency of output to the Abaqus/CFD state file in increments
|
||
|
||
Abaqus/CFD 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).
|
||
|
||
Input File Usage: \*RESTART, WRITE, FREQUENCY=N
|
||
|
||
By default, N=1.
|
||
|
||
<!-- source-page: 640 -->
|
||
|
||
Abaqus/CAE Usage: Step module: Output→Restart Requests: enter N in the Frequency column for each step By default, N=0 (no restart information is written).
|
||
|
||
Specifying the frequency of output to the Abaqus/CFD state file in time intervals
|
||
|
||
Abaqus/CFD 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. By default, the results will be written to the state file at the increment ending immediately after the time dictated by each interval.
|
||
|
||
If a problem precludes the analysis from continuing to completion, such as if the solution does not converge, Abaqus/CFD will attempt to save the last completed increment in the state file.
|
||
|
||
Input File Usage: \*RESTART, WRITE, NUMBER INTERVAL=n
|
||
|
||
Abaqus/CAE Usage: Step module: Output→Restart Requests: enter n in the Intervals column By default, n=0.
|
||
|
||
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, Abaqus/Explicit, and Abaqus/CFD 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.
|
||
|
||
Input File Usage: Use the following option to synchronize restart information written in a cosimulation:
|
||
|
||
\*RESTART, WRITE, NUMBER INTERVAL=n
|
||
|
||
When using the NUMBER INTERVAL parameter for a co-simulation, the TIME MARKS parameter on the \*RESTART option is always set to NO.
|
||
|
||
Abaqus/CAE Usage: Step module: Output→Restart Requests: enter n in the Intervals column
|
||
|
||
# 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.
|
||
|
||
Input File Usage: \*RESTART, WRITE, SINGLE
|
||
|
||
Abaqus/CAE Usage: Single precision state file output is not supported by Abaqus/CAE.
|