*IMPORT

Import information from a previous Abaqus/Explicit or Abaqus/Standard analysis.

This option is used to define the time in a previous Abaqus/Standard or Abaqus/Explicit analysis at which the specified node and element information is imported. The IMPORT option must be used in conjunction with the INSTANCE option when importing a part instance from a previous analysis. In an Abaqus/Explicit import analysis you can define new positions for the imported elements and import an element set more than once, which requires renaming the element set.

Related Topics
*INSTANCE
In Other Guides
About transferring results between Abaqus analyses

ProductsAbaqus/StandardAbaqus/ExplicitAbaqus/CAE

TypeModel data

LevelPart instance

Abaqus/CAESupported for use in conjunction with part instances; importing selected part instances stored in an output database is supported using the File menu and importing the initial state of part instances is supported in the Load module.

Required parameters

UPDATE

Set UPDATE=NO to continue the analysis without resetting the reference configuration.

Set UPDATE=YES to continue the analysis by resetting the reference configuration to be the imported configuration. In this case displacement and strain values are calculated from the new reference configuration.

Required parameters if the imported element sets are to be renamed (Abaqus/Explicit only; not applicable for import of part instances)

EOFFSET

Set this parameter equal to an integer that specifies the offset to be used to renumber the elements in the renamed element sets.

NOFFSET

Set this parameter equal to an integer that specifies the offset to be used to renumber the nodes to be imported for the renamed element sets.

RENAME

Include this parameter to specify new labels for the element sets to be imported from the previous analysis.

Optional, mutually exclusive parameters

INCREMENT

When importing an analysis from Abaqus/Standard into Abaqus/Explicit or from one Abaqus/Standard analysis into another Abaqus/Standard analysis, set this parameter equal to the increment of the specified step on the Abaqus/Standard restart file from which the analysis is to be imported. If this parameter is omitted, the analysis is imported from the last available increment of the specified step.

INTERVAL

When importing an analysis from Abaqus/Explicit into Abaqus/Standard or from one Abaqus/Explicit analysis into another Abaqus/Explicit analysis, set this parameter equal to the interval of the specified step on the Abaqus/Explicit state file from which the analysis is to be imported. If this parameter is omitted, the analysis is imported from the last available interval of the specified step.

ITERATION

This parameter is relevant only when the results are imported from a previous direct cyclic Abaqus/Standard analysis.

When importing an analysis from Abaqus/Standard into Abaqus/Explicit or from one Abaqus/Standard analysis into another Abaqus/Standard analysis, set this parameter equal to the iteration number of the specified step on the Abaqus/Standard restart file from which the analysis is to be imported. Since restart information can be written only at the end of an iteration in a direct cyclic analysis, the INCREMENT parameter is irrelevant and is ignored if the ITERATION parameter is specified. If this parameter is omitted, the analysis is imported from the last available iteration of the specified step.

Optional parameters

STATE

Set STATE=YES (default) to import the current material state of the elements at the specified step and the specified interval, increment, or iteration.

Set STATE=NO if no material state is to be imported. In this case the elements will start with no initial state or with the state as defined by the INITIAL CONDITIONS option.

STEP

Set this parameter equal to the step on the Abaqus/Explicit state file or on the Abaqus/Standard restart file from which the analysis is being imported. If this parameter is omitted, the analysis is imported from the last available step on the state file or the restart file at the specified increment, interval, or iteration.

Data lines to specify the element sets to be imported and optionally repositioned

First line if the element sets are not renamed

  1. List of element sets that are to be imported. Specify only element set names that are used in the previous Abaqus/Explicit or Abaqus/Standard analysis.

Repeat this data line as often as necessary to define the element sets to be imported. Up to 16 element sets can be listed per data line.

First line if the element sets are to be renamed (Abaqus/Explicit only)

  1. The old name of the element set to be imported. Specify only old element set names that are used in the previous Abaqus/Explicit or Abaqus/Standard analysis.

  2. The new name of the element set in the import analysis.

Repeat this data line as often as necessary to specify the old and new names of the element sets to be imported.

Subsequent line to translate the imported element sets (optional if rotation is not specified; Abaqus/Explicit only)

  1. Value of the translation to be applied in the X-direction.

  2. Value of the translation to be applied in the Y-direction.

  3. Value of the translation to be applied in the Z-direction.

Enter values of zero to apply a pure rotation.

Subsequent line to rotate the imported element sets (optional; Abaqus/Explicit only)

  1. X-coordinate of point a on the axis of rotation (see Figure 1).

  2. Y-coordinate of point a on the axis of rotation.

  3. Z-coordinate of point a on the axis of rotation.

  4. X-coordinate of point b on the axis of rotation.

  5. Y-coordinate of point b on the axis of rotation.

  6. Z-coordinate of point b on the axis of rotation.

  7. Angle of rotation about the axis a–b, in degrees.

If both translation and rotation are specified, translation is applied before rotation.

Figure 1. Rotation of an element set.

There are no data lines for importing a part instance