The ABAQUS FAQ
2. Jobs
Q2.1 : How do I run small jobs?
Use the following commandabaqus job=job-id interactive
Example : abaqus job=plate inter
Q2.2 : How do I go about running many small jobs?
Create a batch file (say aba-multrun.bat) with one line per analysis as shown below :abaqus job=analysis-a interactive abaqus job=analysis-b interactive abaqus job=analysis-c interactive abaqus job=analysis-d interactiveThen make the file an executable using the following unix command :
chmod u+x aba-multrun.batThen type aba-multrun to execute the ABAQUS jobs one at a time while you are logged ON. This is only suitable for small jobs which only take a few minutes to run. These jobs will run one at a time and in the sequence in which these appear in the batch file.
This is preferable to submitting all the jobs at the same time (for example typing the above commands directly at the terminal without the interactive parameter). This will put a strain on the server and its resources and inconvenience the other users as well.
For medium to large jobs use the batch command available in the CUED teaching system.
If ABAQUS is installed on a PC (Windows XP O/S) then the above batch file requires a modification. Enclose the lines with a round brackets. in the absence of this bracket only the very first job in the file will be run.
( abaqus job=analysis-a interactive abaqus job=analysis-b interactive abaqus job=analysis-c interactive abaqus job=analysis-d interactive )
Q2.3 : How do I run large jobs?
Q2.4 : How do I run ABAQUS/CAE?
Using the following command :abaqus cae
Q2.5 : How do I run ABAQUS/Viewer?
Using the following command :abaqus viewer
abaqus viewerdatabase=cantilever
Example : abaqus viewer database=cantilever
Q2.6 : How do I get copies of the ABAQUS examples input data files (*.inp)?
There are 2 options. Cut and paste directly from the screen once from the on-line documentation of the Input Files. The other option is to use the fetch command along with the name of the analysis-ID. First find the name of the input file from the Examples manual (available on-line). This will copy the 1010101.inp file to the current directory.For the Laminated Composite Plate failure example (Example 1.1.13 in version 6.3) the input files have the starting name damagefailcomplate. There are a total of ten files listed. Here * (wildcard character) can be used to complete the file name in the fetch command. abaqus fetch command.
Example : abaqus fetch job=damagefailcomplate*
This will fetch the following files to the current directory :
inflating: damagefailcomplate_cps4.f inflating: damagefailcomplate_cps4.inp inflating: damagefailcomplate_cps4r.f inflating: damagefailcomplate_cps4r.inp inflating: damagefailcomplate_element.inp inflating: damagefailcomplate_node.inp inflating: damagefailcomplate_s4.f inflating: damagefailcomplate_s4.inp inflating: damagefailcomplate_s4r.f inflating: damagefailcomplate_s4r.inp
Q2.7 : How do I run a ABAQUS job which uses a user subroutine?
Using the following command :abaqus job=job-id user= < subroutine-filename >
For the Linux Teaching System Computers give the extension .f and for PCs give the extension .for.
The user subroutine has to be in a separate file (say my_material.f).
Example : abq681 j=plate user=my_material
If there are more than 1 user subroutines then all the subroutines must be included in a single file.
If using CAE then in the Job Create a Job and then click on the General tab and click on the browse button for user subroutine and choose the file containing the user subroutine and Click on OK in the browse window and also in the dialog box. Then submit the job.
Q2.8 : How do I run a user written post processing program which accesses the *.fil file?
Using the following command :abaqus make job=This will compile the user program in a file called disp1.f and then create an executable called cantilever.x. Type abaqus cantilever.x to run this program.job-id user=name-of-file Example : abaqus make job=cantilever user=disp1
Q2.9 : How do I find out about the different execution procedures that are available with ABAQUS?
Type abaqus help and this will list all the abaqus execution procedures. These are listed below :
Execution Procedure for ABAQUS/Standard and ABAQUS/Explicit
abaqus job=job-name [ analysis | datacheck | continue | help | recover |
convert={restart|select|all} |
information={environment|local|memory|release|status} ]
[ input=input-file ] [ user=source-file ]
[ oldjob=oldjob-name ] [ fil={append|new} ]
[ globalmodel=results file-name ] [ double ]
[ memory=memory-size ] [ buffer=buffer-size ]
[ interactive | background | queue=queue-name ]
[ cpus=number-of-cpus ] [scratch=scratch-dir]
[ subcomplex=subcomplex-name]
Note: subcomplex is only valid on the Convex Exemplar
Execution Procedure for ABAQUS/Abares
abaqus abares job=job-name [ restart=restart-name ]
[ beginstep=step-number ] [ endstep=step-number ]
[ increment={all|endstep|final|none|integer-list} ]
Execution Procedure for ASCII translation of results (.fil) files
abaqus ascfil job=job-name [ input=input-file ]
Execution Procedure for on-line documentation
abaqus doc
Execution Procedure for ABAQUS/Append
abaqus append job=job-name oldjob=oldjob-name input=input-file
Execution Procedure for ABAQUS/Fetch
abaqus fetch job=job-name [ input=input-file ]
Execution Procedure for ABAQUS/Findkeyword
abaqus findkeyword [ job=job-name ] [ maximum=maximum-matches ]
Execution Procedure for ABAQUS/Make
abaqus make job=job-name [ user={source-file|object-file} ]
Execution procedure for suspending or resuming analysis jobs
abaqus [ suspend | resume ] job=job-name
Execution procedure for fixed format translator
abaqus free job=job-name input=input-file
Execution Procedure for input file upgrade utility
abaqus upgrade job=new-input-file input=old-input-file
Execution Procedure for output database file upgrade utility
abaqus upgrade job=new-output-database-file odb=old-output-database-file
Execution Procedure for the movie player utility
abaqus movieplayer [ movie=animation-file ]
Execution Procedure for ABAQUS Verification
abaqus verify [ -all | -std | -user_std | -exp | -user_exp
-cae | -viewer | -design | -make | -param
-scripting | -adams | -cmold | -moldflow
-catia | -ideas | -parasolid | -proe
-log ]
Q2.10 : How do I find what the current settings are for the environment variables?
Type abaqus info=environment and this will list all the current setting of the ABAQUS environmental variables.memory, local, release, status are other options on which you can get more information on.
For ABAQUS jobs you have run look for *.com file. For the current session in #the Teaching System use the printenv command.
For PCs type "set" in a MS-DOS command window at the DOS prompt (>).
Q2.11 : How do I change the current settings of the environment variables?
Create a file called abaqus_v6.env in the directory from which ABAQUS is run which contains lines of environment variables you want to change set equal to new values. However make sure that the computer on which you are running ABAQUS can support the changes. For example you can increase the memory used by ABAQUS. But you cannot increase this beyond what is available in the computer.Example : Include the following lines in the abaqus_v6.env file to increase the size of pre_memory and the standard_memory used by ABAQUS.
For earlier versions of ABAQUS :
pre_memory="400 mb" standard_memory="500 mb"
If running ABAQUS on a PC then make these to the system copy which will be in the ABAQUS installation directory :
C:\ABAQUS\6.8-1\site\abaqus_v6.env
Q2.12 :Can one run long ABAQUS jobs in the Teaching System Computers?
Q2.13 : When re-running a ABAQUS job getting the old files existing message. Is it possible to over-ride it without having to type Y?
This could also be a problem if ABAQUS is run in an optimisation loop many times automatically.This can be done by adding the following line to the abaqus_v6.env in the directory from which ABAQUS is run (for example).
ask_delete=NO
If running ABAQUS on a PC then make this change to the system copy which will be in the ABAQUS installation directory :
C:\ABAQUS\6.8-1\site\abaqus_v6.env
This needs to be used with care. Accidentally typing the name of a previously carried out analysis (which may have been a long run) which you didn't want to be deleted/overwritten can easily be lost with the above setting (as there is no safety net).
When not required change the setting / or comment it out / or delete it.
# comment it out # # ask_delete=NO # Reset it ask_delete=YES
Q2.14 :How do I stop a ABAQUS analysis job I had submitted?
From a command prompt window (DOS Window) from the same directory from which the job was submitted. Re-type job submission command but this time add suspend to suspend the job execution.ABAQUS job=plate suspend
This allows you to review matters. If you then decide then you want to terminate the job Re-type the job submission command but use the option terminate instead.
ABAQUS job=plate terminate
A run can be terminated using terminate option without having to suspend the job in the first place. A sup ended job can be continued by using the option resume.
ABAQUS job=plate resume
Q2.15 : How do I stop and re-start an analysis job?
Input file for the first run dynam.inp Include the line*RESTART, WRITE, FREQ=1in the second step of this input file and this will write the results of every increment (FREQ = 1) to the re-start file.
The job is run from the command line as follows :
abaqus j=dynamIn this example the 2nd step is not completed.
Lets assume that in the re-started run the analysis is to be continued from the end 10th increment of the second step.
This is done by including the following line after the *HEADING statement.
*RESTART, READ, STEP=2, INCREMENT=1, END STEP, WRITEFailing to include the END STEP parameter would result in the re-started run repeating the second step exactly and failing to complete in the same way as the first run.
Note that since this is a re-start run all the model data part of the input (F.E.Mesh data material properties etc) is omitted. The next statement after the *RESTART statement consists of a *STEP statement.
Input file for the re-started run dynamr.inp
The job is submitted from the command line as follows :
abaqus oldjob=dynam j=dynamr
The following extract taken from dynamr.dat shows that the results are read from the restart file up to the 10th increment and the analysis continuing with the next step (STEP 3).
*HEADING
BISHOP AND DRUCKER -- SMALL DISPLACEMENT ANALYSIS B21
STEP 1 INCREMENT 1 HAS BEEN FOUND ON THE RESTART FILE
STEP 2 INCREMENT 1 HAS BEEN FOUND ON THE RESTART FILE
STEP 2 INCREMENT 2 HAS BEEN FOUND ON THE RESTART FILE
....
STEP 2 INCREMENT 8 HAS BEEN FOUND ON THE RESTART FILE
STEP 2 INCREMENT 9 HAS BEEN FOUND ON THE RESTART FILE
STEP 2 INCREMENT 10 HAS BEEN FOUND ON THE RESTART FILE
The analysis continuing wth the next step (STEP 3). Following is the
extract from the status file : dynamr.sta
Abaqus/Standard 6.9-1 DATE 01-Sep-2009 TIME 15:31:01
SUMMARY OF JOB INFORMATION:
MONITOR NODE: 11 DOF: 2
STEP INC ATT SEVERE EQUIL TOTAL TOTAL STEP INC OF DOF IF
DISCON ITERS ITERS TIME/ TIME/LPF TIME/LPF MONITOR RIKS
ITERS FREQ
3 1 1 0 1 1 1.11 0.0100 0.01000 19.3
3 2 1 0 1 1 1.12 0.0200 0.01000 10.1
3 3 1 0 1 1 1.13 0.0300 0.01000 0.116
3 4 1 0 1 1 1.14 0.0400 0.01000 -10.7
3 5 1 0 1 1 1.15 0.0500 0.01000 -20.5
3 6 1 0 1 1 1.16 0.0600 0.01000 -26.7
3 7 1 0 1 1 1.17 0.0700 0.01000 -29.3
.....
3 97 1 0 1 1 2.07 0.970 0.01000 -11.6
3 98 1 0 1 1 2.08 0.980 0.01000 -1.12
3 99 1 0 1 1 2.09 0.990 0.01000 9.46
3 100 1 0 1 1 2.10 1.00 0.01000 18.8
THE ANALYSIS HAS COMPLETED SUCCESSFULLY
If the ODB files from the first run and the re-started run needs to be
combined into a single ODB file for post-processing purposes, this is
achieved by typing the following line from the command line :
Execution procedure for joining output database (.odb) files from restarted analyses
abaqus restartjoin originalodb=odb-file-name restartodb=odb-file-name [copyoriginal].
|
|
| | Computing Help |[Finite Elements] | [Engineering Packages] |