김경종
21 KiB
9.2 Importing and transferring results
• “Transferring results between Abaqus analyses: overview,” Section 9.2.1
• “Transferring results between Abaqus/Explicit and Abaqus/Standard,” Section 9.2.2
• “Transferring results from one Abaqus/Standard analysis to another,” Section 9.2.3
• “Transferring results from one Abaqus/Explicit analysis to another,” Section 9.2.4
9.2.1 TRANSFERRING RESULTS BETWEEN Abaqus ANALYSES: OVERVIEW
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Transferring results between Abaqus/Explicit and Abaqus/Standard,” Section 9.2.2
• “Transferring results from one Abaqus/Standard analysis to another,” Section 9.2.3
• “Transferring results from one Abaqus/Explicit analysis to another,” Section 9.2.4
• *IMPORT
• *IMPORT ELSET
• *IMPORT NSET
• *IMPORT CONTROLS
• *INSTANCE
• “Transferring results between Abaqus analyses,” Section 16.6 of the Abaqus/CAE User’s Guide
Overview
Abaqus provides the capability to import a deformed mesh and its associated material state from Abaqus/Standard into Abaqus/Explicit and vice versa. This capability is particularly useful in manufacturing problems; for example, the entire sheet metal forming process (which requires an initial preloading, forming, and subsequent springback) can be analyzed. In this case the initial preloading can be simulated with Abaqus/Standard using a static procedure and the subsequent forming process can be simulated with Abaqus/Explicit. Finally, the springback analysis can be performed with Abaqus/Standard.
Abaqus also provides the capability to transfer desired results and model information from an Abaqus/Standard analysis to a new Abaqus/Standard analysis or from an Abaqus/Explicit analysis to a new Abaqus/Explicit analysis, where additional model definitions may be specified before the analysis is continued. For example, during an assembly process an analyst may first be interested in the local behavior of a particular component but later is concerned with the behavior of the assembled product. In this case the local behavior can first be analyzed in an Abaqus/Standard or Abaqus/Explicit analysis. Subsequently, the model information and results from this analysis can be transferred to a second Abaqus/Standard or Abaqus/Explicit analysis, where additional model definitions for the other components can be specified, and the behavior of the entire product can then be analyzed.
For this capability to work, the same release of Abaqus/Explicit and Abaqus/Standard must be run on computers that are binary compatible. In addition, transfer of model and results can only be requested from one previous analysis; transfer from multiple analyses is not supported.
Saving the analysis results
The restart files from the original analysis contain the analysis results that are transferred from Abaqus/Standard or Abaqus/Explicit. Obtaining restart files is described in more detail in “Writing restart files” in “Restarting an analysis,” Section 9.1.1; brief summaries are provided below. By default, Abaqus/Standard does not write any restart information and Abaqus/Explicit writes results at the beginning and end of each step.
Saving results from Abaqus/Standard
If the results are to be imported from an Abaqus/Standard analysis, the results from the original Abaqus/Standard job must be written to the restart (.res), analysis database (.mdl and .stt), part (.prt), and output database (.odb) files.
You can specify the increments at which restart information will be written. Restart information is always written at the end of a step in addition to the requested increments whenever you request restart data in Abaqus/Standard.
Input File Usage: *RESTART, WRITE, FREQUENCY=n
Abaqus/CAE Usage: Step module: Output→Restart Requests: enter n in the Frequency column for each step
Saving results from Abaqus/Explicit
If the results are to be imported from an Abaqus/Explicit analysis, the results from the original Abaqus/Explicit job must be written to the state (.abq) file at the time when transfer of the state of the deformed body is required. The state (.abq), restart (.res), analysis database (.stt), package (.pac), part (.prt), and output database (.odb) files will be used for importing the results from Abaqus/Explicit.
You can specify whether the results are to be written at the exact time dictated by the specified time interval, n, during a step of an Abaqus/Explicit analysis or at the increment ending after the time dictated by the specified time interval. Results are always written at the end of a step, so it is not necessary to request results at the exact time intervals if results will be read only from the end of a step.
Input File Usage: Use the following option to request results at the increments ending immediately after each time interval:
*RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=NO
Use the following option to request results at the exact time intervals:
*RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=YES
Abaqus/CAE Usage: Step module: Output→Restart Requests: enter n in the Number Interval column; click to check the Time Marks column for each step if you want the results written at the exact time intervals
The import capability is used to transfer model data and results from one analysis to another. The following sections describe how to specify the import request. You can import element sets from models that are not defined as assemblies of part instances, or you can import part instances from models that are defined as assemblies of part instances. In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
Although elements of different types, (such as C3D4, C3D6, C3D8R, etc.) can be specified in the same element set used in a section definition, the maximum number of element types is limited to three if the model is to be used in an import analysis.
Specifying the transfer of model data and results for models that are not defined as assemblies of part instances
You can import element sets from a previous analysis to specify the transfer of model data and results for models that are not defined as assemblies of part instances. This import capability is illustrated in “Springback of two-dimensional draw bending,” Section 1.5.1 of the Abaqus Example Problems Guide, and “Axisymmetric forming of a circular cup,” Section 1.3.7 of the Abaqus Example Problems Guide.
Each element set to be imported must have been defined in the original analysis. You can import any element set, including nested element sets and those with overlapping elements. An imported element set can also be a subset of another imported element set. The elements in these sets as well as the element set definitions are imported. Even though an element may be included in multiple imported elements sets, each element is imported only once in the import analysis. You cannot use element sets that are internal to the original analysis.
Input File Usage:
Use the following option to import element sets from a previous analysis:
*IMPORT
list of element sets that are to be imported
For example, the following input imports the element set definitions for BLANK1 and BLANK2 in addition to the elements and element set definition for BLANK:
Original analysis
*SHELL SECTION, MATERIAL=STEEL1, ELSET=BLANK1
.00082, 5
*SHELL SECTION, MATERIAL=STEEL2, ELSET=BLANK2
.00082, 5
*ELSET, ELSET=BLANK
BLANK1, BLANK2
Import analysis
*IMPORT
BLANK
To prevent any ambiguity regarding element and node definitions, the *IMPORT option must be specified before any options that define additional model data in the input file.
Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
Repositioning elements in the model in an Abaqus/Explicit analysis
In an Abaqus/Explicit analysis you can reposition elements in the element sets from their original positions in the previous analysis to new positions in the import analysis. The new position is determined by a translation and/or rotation of the original position relative to the origin of the global coordinate system. The positioning data apply to all elements in the list of imported element sets. Element sets that require different positioning data need to be grouped separately during import.
Input File Usage: Use the following option to reposition imported element sets from a previous analysis:
*IMPORT
list of element sets that are to be imported and relocated positioning data
Multiple *IMPORT options need to be defined for elements sets that require different positioning data.
Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
Importing model data and results of element sets multiple times in an Abaqus/Explicit analysis
You can import model data and results of element sets from a previous analysis to an Abaqus/Explicit analysis multiple times. You must define a new name and a new position for an element set that has been imported more than once. You specify the old element set name used in the previous analysis followed by the new element set name to be used in the import analysis. The old element set name must have been defined in the previous analysis and use of internal sets is not supported.
New elements and nodes are generated with new element and node numbers for the renamed element sets. You specify element and node offsets; the new numbers are obtained by adding the offsets to the old numbers used in the previous analysis. It is your responsibility to select appropriate element and node offsets to preserve uniqueness of element and node numbering in the model.
The new position is determined as described in “Repositioning elements in the model in an Abaqus/Explicit analysis.” To prevent multiple elements in the model occupying identical positions, an old element set name must not appear more than once in the list of imported element sets for each import definition. Element sets that require renaming must be grouped separately during import from those that do not require renaming.
Input File Usage: Use the following option to rename and reposition element sets to be imported from a previous analysis:
*IMPORT, RENAME, EOFFSET=element-offset, NOFFSET=node-offset
old_name_elem_set1, new_name_elem_set1 old_name_elem_set2, new_name_elem_set2
positioning data
Separate *IMPORT options need to be defined for element sets that require renaming and/or employ different positioning data, as shown in the following example:
*IMPORT, UPDATE=NO
ASSEMBLY_QUADRANT_1_LOWER,
ASSEMBLY_QUADRANT_1_UPPER,
*IMPORT, UPDATE=NO, RENAME, OFFSET=80, NOFFSET=97
ASSEMBLY_QUADRANT_1_LOWER, ASSEMBLY_QUADRANT_2_LOWER
ASSEMBLY_QUADRANT_1_UPPER, ASSEMBLY_QUADRANT_2_UPPER
0., 0., 0.,
0., 0., 0., 0., 0., 1., 90.,
Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
Importing element set and node set definitions
All element set and node set definitions associated with the imported elements are imported by default. For models that are not defined as assemblies of part instances, you can also selectively import only specified element set or node set definitions. This capability provides a convenient way of selectively reusing the element or node sets defined in the original analysis. However, any members of such sets that do not belong to the imported elements are removed from the specified sets.
For example, suppose three element sets—SHELL3D, MEMB, and ALL—are defined in the original analysis. Element set ALL contains all of the elements in element sets SHELL3D and MEMB, as well as other elements. You choose to import only the element sets SHELL3D and MEMB (i.e., the elements in these sets as well as the element set definitions). In addition, you selectively import the element set definition ALL (but not the elements in this set). If element 100 belongs to element set ALL but not to either element set SHELL3D or element set MEMB, it will not be imported and will be removed from the list of elements belonging to element set ALL. The imported element set definitions are processed before any node or element definitions; therefore, even if element 100 is subsequently redefined in the import analysis, it will not belong to element set ALL (unless it is explicitly assigned to element set ALL in the import analysis).
Only node and element sets defined in the original or previous import analysis are available for importing. New sets defined during a restart run cannot be imported.
Input File Usage: Use either or both of the following options immediately following the *IMPORT option to import selected element or node set definitions:
*IMPORT ELSET
*IMPORT NSET
For models that are defined as assemblies of part instances, you cannot selectively import element and node set definitions. All element and node set definitions are imported automatically.
Abaqus/CAE Usage:
In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. You cannot selectively import element and node set definitions in Abaqus/CAE. All element and node set definitions are imported automatically.
Importing element sets and node sets multiple times in an Abaqus/Explicit analysis
You can import element sets and node sets from a previous analysis to an Abaqus/Explicit analysis multiple times. You must define a new name for an element set or a node set that has been imported more than once. You specify the old element or node set name used in the previous analysis followed by the new element or node set name to be used in the import analysis. The old set name must have been defined in the previous analysis and use of internal sets is not supported.
New elements and nodes are generated with new element and node numbers for the renamed sets using the offsets that you specified for import; the new numbers are obtained by adding the offsets to the old numbers used in the previous analysis.
Element sets and node sets that require renaming must be grouped separately during import from those that do not require renaming.
Input File Usage:
Use the following options to rename element sets and node sets to be imported from a previous analysis:
*IMPORT ELSET, RENAME *IMPORT NSET, RENAME
The *IMPORT ELSET and *IMPORT NSET options must immediately follow an *IMPORT option with the RENAME, EOFFSET, and NOFFSET parameters specified. The offset values to be used are given by the parameter values of EOFFSET and NOFFSET of the *IMPORT option immediately preceding the *IMPORT ELSET and *IMPORT NSET options.
Abaqus/CAE Usage:
In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
Specifying the transfer of model data and results for models that are defined as assemblies of part instances
You can import part instances from a previous analysis to specify the transfer of model data and results for models that are defined as assemblies of part instances. If you import more than one part instance, the part instances must be from the same output database (.odb) file and all import parameters must be the same for each imported part instance. Each instance name that you specify must be the same as the instance name in the original analysis. Only sets that are defined within the imported instance will be imported. Sets defined at the assembly level must be redefined in the import analysis. New set definitions and surface definitions can be added upon import. You cannot assign new sections, material orientations, normals, or beam orientations to the imported part instance.
Input File Usage: Use the following options to import a part instance from a previous analysis:
*INSTANCE, INSTANCE=instance-name
Additional set and surface definitions (optional)
*IMPORT
*END INSTANCE
Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: select the instances to which the initial state should be assigned
Repositioning part instances in the model in an Abaqus/Explicit analysis
You can import a part instance in an Abaqus/Explicit analysis and specify a new position for the part instance in the imported model. The new position is determined by a translation and/or rotation of the original position relative to the origin of the assembly (global) coordinate system.
Input File Usage: Use the following options to import and reposition a part instance from a previous analysis:
*INSTANCE, INSTANCE=instance-name
positioning data
Additional set and surface definitions (optional)
*IMPORT
*END INSTANCE
Abaqus/CAE Usage: Repositioning part instances in the model is not supported in Abaqus/CAE.
Importing part instances in the model multiple times in an Abaqus/Explicit analysis
In an Abaqus/Explicit analysis you can import a part instance from a previous analysis more than once. A part instance must be instanced separately in the assembly each time it is imported. In each instance, you must define a new name and a new position for a part instance that has been imported more than once. You specify the old name of the part instance in the previous analysis and a new name for the part instance.
The new position is determined by a translation and/or rotation of the original position relative to the origin of the assembly (global) coordinate system. Sets defined within the part instance will be imported and repositioned. Sets defined at the assembly level must be redefined in the import analysis. New set definitions and surface definitions can be added upon import. You cannot assign new sections, material orientations, normals, or beam orientations to the imported part instance. If you import more than one part instance, the part instances must be from the same output database (.odb) file and all import parameters must be the same for each imported part instance.
Input File Usage: Use the following options to import a part instance more than once from a previous analysis:
*INSTANCE, NAME=new instance-name, INSTANCE=old instance-name
positioning data
Additional set and surface definitions (optional)
*IMPORT
*END INSTANCE
Abaqus/CAE Usage: Importing part instances in the model multiple times is not supported in Abaqus/CAE.
Identifying the analysis from which the data will be obtained
You must specify the name of the job from which the model and results data will be obtained.
Input File Usage:
For all models you can enter the following input on the command line:
abaqus job=job-name oldjob=oldjob-name
If the oldjob parameter is omitted, Abaqus will prompt for the job name (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2) even if the current job is an Abaqus/Explicit analysis that uses the recover option to restart from the last available step and increment in the state file.
Alternatively, for models defined as assemblies of part instances, you can use the following option:
*INSTANCE, LIBRARY=oldjob-name
If you import more than one part instance, the oldjob-name specified by the LIBRARY parameter must be the same for each imported part instance.
If the job name is specified on the command line using the oldjob option, the command line specification will take precedence over the LIBRARY parameter.
Abaqus/CAE Usage:
In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: Job name: output-database-name
Importing model data
Element property definitions of imported elements can be redefined only if the reference configuration is updated (see “Updating the reference configuration”) and the material state is not imported (see “Importing the material state”). In this case the material orientation definitions (“Orientations,” Section 2.2.5), hourglass stiffness but not hourglass control definitions, and transverse shear stiffness definitions (in the case of shell elements) of the imported elements can also be redefined.
For other reference configuration and material state combinations, the information required to define the section for each imported element will be imported from the original analysis. Material orientations cannot be redefined in the import analysis; orientation names cannot be reused in the import analysis. For imported elements, the material orientations will be transferred from the original