*IMPERFECTION command Help Please! 1

[AK1984]

Hello everyone,

I am trying to use the *IMPERFECTION command to introduce geometric imperfections from an Eigenvalue-buckling-analysis into a static analysis step.

I followed the ABAQUS documentation. I have done the following:

1- I used the *NODE FILE command in the .inp input file of the Eigenvalue-buckling-analysis step.

2- I got the .fil result file

3- I used the *IMPERFECTION command in the .inp input file of the Static-analysis step (I tried placing the command in different locations within the .inp file):

*IMPERFECTION, FILE=Eigen1, STEP=Step-1
1, 0.5

4- I get this error message:

keyword *IMPERFECTION, file "Static.inp", line 5301: The keyword is misplaced. It can be suboption for the following keyword(s)/level(s): model

Please Help,

Best Regards,
Ahmed

 

[Rocketeer3k]

Are you using the keyword editor? It makes it a littles easier. Please copy paste your keywords for the file in which you want to have imperfections so we can take a look.

If been there too, it takes a little trial and error. As with so many thigs in abaqus, a good reference example is nowhere to be found.

 

[beyondemon]

Make sure that you are defining the imperfection in model level.

Mohammad M. Shahbazi

http://omranafzar.com/en

 

[AK1984]

Thanks guys for response,

@Rockteer3k : I am already using text editor. I have been doing trial and error for 3 days now and it all ended up to this error. I will post the keywords shortley after I minimize the file a little bit. Thanks.


@beyondemon : This is the issue, I don't know what does defining the imperfection in the "MODEL LEVEL" means. Please inform me if you know how. Thank you very much.

 

[beyondemon]

An ABAQUS model has several levels such as Part level, Instance level, Model level, and Analysis level. The imperfection goes to model level where boundary and initial conditions are defined. Therefore, you just need to move the imperfection to somewhere besides initial and boundary conditions.

Mohammad M. Shahbazi

http://omranafzar.com/en

 

[AK1984]

Thanks Mohammad,

That was part of the problem that I fixed, Also, I noticed that I had the name of the step in the *Imperfection command wrong, so it had to be modified.

Also, I should note that I couldn't run the two steps in one .inp file (as discussed in abaqus documentation).

it only worked when I separated the two steps in two different .inp files.


Thank you all very much for your help.

Ahmed

 

[ArcadiaSolarSail]

Hi all i have the same problem of the other collegue, where is located the model level?? I cant find it in the inp file.

*Heading
** Job name: Carico_buckling_lin Model name: Model-1
** Generated by: Abaqus/CAE 6.10-1
*Preprint, echo=NO, model=YES, history=NO, contact=NO
**
** PARTS
**
*Part, name=Boom
*Node
1, -9.98489094, 0.349999994, 1000.
.........
*Elements
..........
29997, 30496, 30497, 30558, 30557
29998, 30497, 30498, 30559, 30558
29999, 30498, 30499, 30560, 30559
30000, 30499, 30500, 30561, 30560
.......
*Nset, nset=_PickedSet26, internal, generate
1, 30561, 1
*Elset, elset=_PickedSet26, internal, generate
1, 30000, 1
*Nset, nset=Fixed_End, generate
1, 61, 1
*Elset, elset=Fixed_End, generate
1, 60, 1
*Nset, nset=Load_end, generate
30501, 30561, 1
*Elset, elset=Load_end, generate
29941, 30000, 1
** Section: Section-1
*Shell General Section, elset=_PickedSet26, density=1.7e-06
6102., 5878., 6102., 0., 0., 3113., 0., 0.
0., 23.3, 0., 0., 0., 22.1, 23.3, 0.
0., 0., 0., 0., 22.7,
*End Part
**
**
** ASSEMBLY
**
*Assembly, name=Assembly
**
*Instance, name=Boom-1, part=Boom
*End Instance
**
*Node
1, 0., 0., 0.
*Nset, nset="Attachment Points-1-Set-1"
1,
*Nset, nset=_PickedSet82, internal, instance=Boom-1, generate
30501, 30561, 1
*Elset, elset=_PickedSet82, internal, instance=Boom-1, generate
29941, 30000, 1
*Nset, nset=_PickedSet83, internal
1,
*Nset, nset=_PickedSet84, internal, instance=Boom-1, generate
1, 61, 1
*Elset, elset=_PickedSet84, internal, instance=Boom-1, generate
1, 60, 1
*Nset, nset=_PickedSet85, internal, instance=Boom-1, generate
30501, 30561, 1
*Elset, elset=_PickedSet85, internal, instance=Boom-1, generate
29941, 30000, 1
*Nset, nset=_PickedSet88, internal
1,
*Nset, nset=_PickedSet89, internal, instance=Boom-1, generate
1, 61, 1
*Elset, elset=_PickedSet89, internal, instance=Boom-1, generate
1, 60, 1
*Nset, nset=_PickedSet90, internal, instance=Boom-1, generate
30501, 30561, 1
*Elset, elset=_PickedSet90, internal, instance=Boom-1, generate
29941, 30000, 1
*Nset, nset=_PickedSet91, internal
1,
*Nset, nset=_PickedSet92, internal, instance=Boom-1, generate
30501, 30561, 1
*Elset, elset=_PickedSet92, internal, instance=Boom-1, generate
29941, 30000, 1
*Nset, nset=_PickedSet93, internal, instance=Boom-1, generate
1, 61, 1
*Elset, elset=_PickedSet93, internal, instance=Boom-1, generate
1, 60, 1
*Elset, elset=_BoomSup_SNEG, internal, instance=Boom-1, generate
1, 30000, 1
*Surface, type=ELEMENT, name=BoomSup
_BoomSup_SNEG, SNEG
*Elset, elset=_BoomOP_SPOS, internal, instance=Boom-1, generate
1, 30000, 1
*Surface, type=ELEMENT, name=BoomOP
_BoomOP_SPOS, SPOS
*Surface, type=NODE, name=_PickedSet82_CNS_, internal
_PickedSet82, 1.
** Constraint: Caricodipunta
*MPC
BEAM, _PickedSet82, _PickedSet83
*End Assembly
*Amplitude, name=spostamento_smooth, definition=SMOOTH STEP
0., 0., 0.5, 0.5, 1., 1.
**
** MATERIALS
**
*Material, name="T300 Epoxy 913 tow"
*Damping
*Density
1.7e-06,
*Elastic, type=LAMINA
159520.,11660., 0.27, 3813., 3813., 3961.
**
** INTERACTION PROPERTIES
**
*Surface Interaction, name=Proprietà_contatto
1.,
*Friction
0.,
** ----------------------------------------------------------------
**
** STEP: Axial_disp
**
*Step, name=Axial_disp, nlgeom=YES, inc=500
*Static
0.01, 1., 1e-05, 1.
**
** BOUNDARY CONDITIONS
**
** Name: Spostamento_Assiale Type: Displacement/Rotation
*Boundary
"Attachment Points-1-Set-1", 3, 3, 10.
** Name: Vincolo_base_spostamento_assiale Type: Displacement/Rotation
*Boundary
_PickedSet93, 1, 1
_PickedSet93, 2, 2
_PickedSet93, 3, 3
_PickedSet93, 6, 6
** Name: Vincolo_spostamento_assiale Type: Displacement/Rotation
*Boundary
_PickedSet92, 1, 1
_PickedSet92, 2, 2
_PickedSet92, 4, 4
_PickedSet92, 5, 5
_PickedSet92, 6, 6
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-3
**
*Output, field
*Node Output
CF, RF, U
*Element Output, directions=YES
S,
*Output, history, frequency=0
*End Step
** ----------------------------------------------------------------
**
** STEP: Buckle_LIN
**
*Step, name=Buckle_LIN, perturbation
*Buckle
5, , 10, 30
**
** BOUNDARY CONDITIONS
**
** Name: Spostamento_Assiale Type: Displacement/Rotation
*Boundary, op=NEW, load case=1
** Name: Vincolo_base Type: Displacement/Rotation
*Boundary, op=NEW, load case=1
_PickedSet84, 1, 1
_PickedSet84, 2, 2
_PickedSet84, 3, 3
_PickedSet84, 6, 6
*Boundary, op=NEW, load case=2
_PickedSet84, 1, 1
_PickedSet84, 2, 2
_PickedSet84, 3, 3
_PickedSet84, 6, 6
** Name: Vincolo_base_spostamento_assiale Type: Displacement/Rotation
*Boundary, op=NEW, load case=1
** Name: Vincolo_carico Type: Displacement/Rotation
*Boundary, op=NEW, load case=1
_PickedSet85, 1, 1
_PickedSet85, 2, 2
_PickedSet85, 4, 4
_PickedSet85, 5, 5
_PickedSet85, 6, 6
*Boundary, op=NEW, load case=2
_PickedSet85, 1, 1
_PickedSet85, 2, 2
_PickedSet85, 4, 4
_PickedSet85, 5, 5
_PickedSet85, 6, 6
** Name: Vincolo_spostamento_assiale Type: Displacement/Rotation
*Boundary, op=NEW, load case=1
**
** LOADS
**
** Name: Carico Type: Concentrated force
*Cload
_PickedSet88, 3, 1.
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field
*Node Output
U,
*Element Output, directions=YES
ALPHA, CS11, CTSHR, E, EE, ER, IE, LE, MISESMAX, NE, PE, PEEQ, PEEQMAX, PEEQT, PEMAG, PEQC
PS, S, SALPHA, SE, SEE, SEP, SEPE, SPE, SSAVG, THE, TRIAX, TSHR, VE, VEEQ, VS
*End Step
** ----------------------------------------------------------------
**
** STEP: Ricks
**
*Step, name=Ricks, nlgeom=YES, inc=500
*Static, riks
0.1, 1., 1e-05, 200., 2.,
**
** BOUNDARY CONDITIONS
**
** Name: Spostamento_Assiale Type: Displacement/Rotation
*Boundary, op=NEW
** Name: Vincolo_Ricks Type: Displacement/Rotation
*Boundary, op=NEW
_PickedSet89, 1, 1
_PickedSet89, 2, 2
_PickedSet89, 3, 3
_PickedSet89, 6, 6
** Name: Vincolo_base_spostamento_assiale Type: Displacement/Rotation
*Boundary, op=NEW
** Name: Vincolo_carico_Ricks Type: Displacement/Rotation
*Boundary, op=NEW
_PickedSet90, 1, 1
_PickedSet90, 2, 2
_PickedSet90, 4, 4
_PickedSet90, 5, 5
_PickedSet90, 6, 6
** Name: Vincolo_spostamento_assiale Type: Displacement/Rotation
*Boundary, op=NEW
**
** LOADS
**
** Name: Carico_Ricks Type: Concentrated force
*Cload
_PickedSet91, 3, 3.
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-3
**
*Output, field
*Node Output
CF, RF, U
*Element Output, directions=YES
S,
**
** FIELD OUTPUT: F-Output-2
**
*Node Output
U,
*Element Output, directions=YES
S,
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step

 

[AK1984]

You should add it before the STEP as below

*IMPERFECTION
....
....
....
**
** STEP: Axial_disp
**
*Step, name=Axial_disp, nlgeom=YES, inc=500

I also recommend you do the buckling analysis in a separate INP file


Best Regards,
Ahmed