add *imperfection into .inp file directly, using a text editor 2

[kkbabak]

hello every one
i m working to add buckling analysis results (buckling modes) in my main general analysis step as initial geometric imperfection.

whenever i add *imperfection command in abaqus cae (graphic interface) the Intended buckling mode would be added to static analysis as expected but in i need to add the *imperfection command in .inp file directly from matlab environment and despite of right position of *imperfection in .inp file, the abaqus ignore the *imperfection and the analysis would continue without implementing the imperfected geometry to the end.

How could I add *IMPERFECTION to my .inp file directly using a text editor or matlab ?
Thank you.

 

[TGS4]

Use a text editor. The input file is a text file.

 

[kkbabak]

i know!
as i explained,when i use a text editor and add *imperfection command in .inp file,the abaqus ignore it and the job complete without adding the imperfected shape to main analysis.
but when i import the .inp file in abaqus cae and add the *imperfection command, it works!

 

[Mustaine3]

I don't believe that. Maybe you still submit the job from /CAE and not the modified .inp on your hard disk.

 

[kkbabak]

thanks for respond.
this is my .inp file. maybe the place of *imperfection command in inp structure is not true.
the second command line of *imperfection as well as nodes are ignored here.


*Heading
** Job name: main-base Model name: shahed-main
** Generated by: Abaqus/CAE 6.13-4
*Preprint, echo=NO, model=NO, history=NO, contact=NO
**
** PARTS
**
*Part, name=MAIN-1
*Node
*Element, type=S3
*Elset, elset=ALLP, generate
** Section: sec
*Shell Section, elset=ALLP, material=S1MAT
*End Part
*IMPERFECTION, FILE=buck, STEP=1 *********************************
**
**
** ASSEMBLY
**
*Assembly, name=Assembly
**
*Instance, name=MAIN-1, part=MAIN-1
*End Instance
**
*Elset, elset=all, instance=MAIN-1, generate
*Elset, elset=peeqset, instance=MAIN-1
*Nset, nset=bot, instance=MAIN-1
*Nset, nset=botnodes, instance=MAIN-1
*Nset, nset=top, instance=MAIN-1
*Nset, nset=topnodes, instance=MAIN-1
*Surface, type=NODE, name=botnodes_CNS_, internal
botnodes, 1.
*Surface, type=NODE, name=topnodes_CNS_, internal
topnodes, 1.
** Constraint: BOT
*Coupling, constraint name=BOT, ref node=bot, surface=botnodes_CNS_
*Kinematic
** Constraint: TOP
*Coupling, constraint name=TOP, ref node=top, surface=topnodes_CNS_
*Kinematic
*End Assembly
*Amplitude, name=AMP-1
**
** MATERIALS
**
*Material, name=S1MAT
*Elastic
201000., 0.3
*Plastic, hardening=COMBINED, datatype=PARAMETERS, number backstresses=4
185.,22000., 300., 1600., 120., 6000., 250., 600.
30.,
**
** BOUNDARY CONDITIONS
**
** Name: bot Type: Displacement/Rotation
*Boundary
bot, 1, 1
bot, 2, 2
bot, 3, 3
bot, 4, 4
bot, 5, 5
bot, 6, 6
** Name: top Type: Displacement/Rotation
*Boundary
top, 3, 3
top, 4, 4
top, 5, 5
top, 6, 6
** ----------------------------------------------------------------
**
** STEP: Step-1
**
*Step, name=Step-1, nlgeom=YES, inc=1000000000
*Static
0.005, 192., 4.8e-13, 0.05
**
** BOUNDARY CONDITIONS
**
** Name: topu Type: Displacement/Rotation
*Boundary, amplitude=AMP-1
top, 1, 1, 1.
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
*Print, solve=NO
**
** FIELD OUTPUT: F-Output-1
**
*Output, field
*Node Output
RF, U
*Element Output, directions=YES
E, NFORC, PE, PEEQ, S
**
** HISTORY OUTPUT: allpd
**
*Output, history
*Energy Output, elset=all
ALLPD,
**
** HISTORY OUTPUT: rfbot
**
*Node Output, nset=bot
RF1,
**
** HISTORY OUTPUT: topu
**
*Node Output, nset=top
U1,
*NODE PRINT, GLOBAL=NO, FREQUENCY=1,NSET=top,TOTALS=NO,SUMMARY=NO
U1
*EL PRINT, POSITION=INTEGRATION POINTS,ELSET=peeqset, FREQUENCY=10,TOTALS=NO,SUMMARY=NO
Peeq
*NODE PRINT, GLOBAL=NO, FREQUENCY=1,NSET=bot,TOTALS=NO,SUMMARY=NO
rf1
*End Step

 

[TGS4]

How are you submitting your job? If from inside cae, then cae will overwrite the input file. You need to submit from the command line.

 

[kkbabak]

thank you TGS4! you are right!
every time i submitted .inp file from cae, the abaquswould overwrite the .inp file!
i submitted it from command line and the buckling mode added to main analysis
thankyou