Using *IMPORT to transfer final state from an Abaqus Standard model to an Abaqus Explicit Model 2

[luc46552]

Hello,

I was wondering if anyone here has ever used the *IMPORT command in an input file to create a job that runs a dynamic-explicit step in a new model from the final state in a standard model. I have not created a job using an input file before, so I may be making some basic mistakes. Currently, I can get the job to run, but is returns several errors:

- "TRANSLATION/ROTATION DATA MUST FOLLOW ELEMENT SET NAMES IN THE DATA LINES OF THE *IMPORT OPTION"
- "THERE ARE NO ELEMENT SET DATA SPECIFIED FOR THE *IMPORT OPTION"

I'm having difficulty finding any examples on how to format the *IMPORT command for transferring an assembly from one model to another. I have read several versions of the "Transferring Results Between Abaqus/Explicit and Abaqus/Standard" in the user's manual, and it has gotten me this far, but I can't seem to figure out what is causing these errors. Here is what I have for the input file so far (it's pretty short):

*HEADING
*PREPRINT, ECHO=NO, MODEL=NO, HISTORY=NO, CONTACT=NO
**
*ASSEMBLY,NAME = CobraWeave
**
*INSTANCE,
LIBRARY=CobraWeaveStandard,
INSTANCE=Large Stick-1-lin-1-1,
INSTANCE=Large Stick-1-lin-1-2,
INSTANCE=Large Stick-1-lin-1-3,
INSTANCE=Large Stick-2-lin-1-1,
INSTANCE=Large Stick-2-lin-1-2,
INSTANCE=Large Stick-2-lin-1-3,
INSTANCE=Large Stick-Trigger-1,
INSTANCE=Large Stick-Trigger-2
**
*IMPORT, UPDATE=NO
**
*END INSTANCE
**
*END ASSEMBLY
**
*STEP, NAME="Release of Contact", NLGEOM=YES
*DYNAMIC, EXPLICIT
*BULK VISCOSITY
0.06, 1.2
*END STEP

In the data file, it displays the following warning regarding the instances, I'm not sure if it's significant:

- "in keyword *INSTANCE, file "CobaWeaveExplicit.inp", line 12: Repeated parameter: instance. New definition of "Large Stick-1-lin-1-2" overrides previous setting."

 

[Erik Panos Kostson]

This link shows how to do what you want. Look at the last example and repeat that process for every instance in your assembly.

http://bobcat.nus.edu.sg:2080/English/SIMACAEANLRefMap/simaanl-c-exptostd.htm

 

[FEA way]

Did you read the chapter regarding *IMPORT in Keywords Reference Guide ? It's important to see this guide before doing changes in INP file as it contains the necessary information about syntax. In this case you should add a line below *IMPORT with the names of element sets to be imported. The errors you get concern this part of import analysis definition.

 

[Erik Panos Kostson]

Below is a small example (not really good syntax perhaps but it works).
Frame structure which runs on the static solver with a pretension force. This is then used as initial condition in an explicit run, which has an additional transverse force. So first is the imex (static), and then the imexex (explicit).
I have them as two separate files which run from command prompt.

*Heading
** Job name: imex Model name: Model-1
*Preprint, echo=NO, model=NO, history=NO, contact=NO
**
** PARTS
**
*Part, name=Part-1
*Node
      1,  0.,           1.,           0.
	  2,  1.,           0.,           0.
*Element, type=B31
1, 1, 2

*Elset, elset=Set-1
 1
** Section: Section-1  Profile: Profile-1
*Beam Section, elset=Set-1, material=Material-1, temperature=GRADIENTS, section=RECT
0.05, 0.05
0,0,-1
*End Part
*Part, name=Part-2
*Node
      1,  0.,          -1.,           0.
	  2,  1.,           0.,           0.
*Element, type=B31
1, 1, 2
*Elset, elset=Set-10
 1
** Section: Section-2  Profile: Profile-2
*Beam Section, elset=Set-10, material=Material-1, temperature=GRADIENTS, section=RECT
0.05, 0.05
0,0,-1
*End Part
**  
**
** ASSEMBLY
**
*Assembly, name=Assembly
**  
*Instance, name=Part-1-1, part=Part-1
*End Instance
*Instance, name=Part-2-1, part=Part-2
*End Instance
**  
*Nset, nset=Set-1, instance=Part-1-1
 1,
*Nset, nset=Set-2, instance=Part-1-1
 2,
*Nset, nset=Set-11, instance=Part-2-1
 1,
*Nset, nset=Set-22, instance=Part-2-1
 2,
*Surface, type=NODE, name=SET-2_CNS_, internal
SET-2, 1.
*Surface, type=NODE, name=SET-22_CNS_, internal
SET-22, 1.
** Constraint: Constraint-1
*Tie, name=Constraint-1, adjust=yes
SET-22_CNS_, SET-2_CNS_
*End Assembly
** 
** MATERIALS
** 
*Material, name=Material-1
*Density
7800.,
*Elastic
 2e+11, 0.3
** ----------------------------------------------------------------
** 
** STEP: Step-1
** 
*Step, name=Step-1, nlgeom=NO
*Static
1., 1., 1e-05, 1.
** 
** BOUNDARY CONDITIONS
** 
** Name: BC-1 Type: Symmetry/Antisymmetry/Encastre
*Boundary
Set-1, ENCASTRE
*Boundary
Set-11, ENCASTRE
** 
** LOADS
** 
** Name: Load-1   Type: Concentrated force
*Cload
Set-2, 1, 1000.
** 
** OUTPUT REQUESTS
** 
*Restart, write, frequency=1
** 
** FIELD OUTPUT: F-Output-1
** 
*Output, field, variable=PRESELECT
** 
** HISTORY OUTPUT: H-Output-1
** 
*Output, history, variable=PRESELECT
*End Step

*Heading
** Job name: imexex Model name: Model-1
*Preprint, echo=NO, model=NO, history=NO, contact=NO
** ASSEMBLY
**
*Assembly, name=Assembly
**  
*Instance, instance=Part-1-1, LIBRARY=imex
*IMPORT, STEP=1, INCREMENT=1, STATE=YES, UPDATE=NO
*End Instance
*Instance, instance=Part-2-1, LIBRARY=imex
*IMPORT, STEP=1, INCREMENT=1, STATE=YES, UPDATE=NO
*End Instance
**
*Nset, nset=Set-100, instance=Part-1-1
 1,
*Nset, nset=Set-200, instance=Part-1-1
 2,
*Nset, nset=Set-110, instance=Part-2-1
 1,
*Nset, nset=Set-220, instance=Part-2-1
 2,
*Surface, type=NODE, name=SET-2_CNS_, internal
SET-200, 1.
*Surface, type=NODE, name=SET-22_CNS_, internal
SET-220, 1.
** Constraint: Constraint-1
*Tie, name=Constraint-1, adjust=yes
SET-22_CNS_, SET-2_CNS_
*End Assembly
**
** BOUNDARY CONDITIONS
** 
** Name: BC-1 Type: Symmetry/Antisymmetry/Encastre
*Boundary
Set-100, ENCASTRE
*Boundary
Set-110, ENCASTRE
**  
** ----------------------------------------------------------------
** 
** STEP: Step-1
** 
*Step
*Dynamic,explicit
,2.0E-1
** 
** LOADS
** 
** Name: Load-1   Type: Concentrated force
*Cload
Set-200, 1, 1000.
*Cload
Set-200, 2, 1000.
** 
** OUTPUT REQUESTS
** 
*End Step