Recovering Results from a Substructure

The abaqus substructurerecover utility recovers results within a substructure using the modal recovery matrices.

Results recovery is performed for static or dynamic time-domain or frequency-domain solutions obtained from Abaqus/Standard and from the following workflows:

  • Abaqus-ADAMS flexible body dynamics
  • Abaqus-EXCITE flexible body dynamics
  • Abaqus-Simpack flexible body dynamics

This page discusses:

 

See Also
Generating Substructures
Using Substructures

Using the Utility

The following procedure summarizes the typical usage of the abaqus substructurerecover utility:

  1. Run an Abaqus/Standard substructure generation analysis to generate the following items:
    • Substructure
    • Flexible body
    • Recovery matrices for the nodal and element results
    • Model data ODB file
  2. Do one of the following:
  3. Run the abaqus substructurerecover utility to recover results within the substructure, specifying the substructure name that defines the substructure SIM and model data ODB files and specifying the file that contains the solution for all the substructure degrees of freedom.

Command Summary

abaqus substructurerecoverjobjob-namesubstructuresubstructure-nameinputinput-file-nameformat{OP4INP4MDFASCSIM}eigenproblemminframevaluevaluemaxframevaluevalueresultsformat{ODBSIMBOTH}outputvariables-listnsetnode-set-nameselsetelement-set-names

Command Line Options

job

This option specifies the name of the output database file: job-name.odb. It also defines the input-file-name if the input option is not specified.

substructure
This option specifies the name of the substructure ("Z-name") that defines the substructure SIM and model data ODB files.
input
This option specifies the name of the input file that contains the solution for all the substructure degrees of freedom. If the option is omitted, the default value is job-name.

The contents and format of the solution input file are specific to the product used to obtain the solution.

The solution input file name may include one of the following supported file extensions: .op4, .inp4, .mdf, .asc, and .sim.

format
This option specifies the format of the solution input file. The following formats are supported: OP4, INP4, MDF, ASC, and SIM. If this option is omitted, the format is determined by the extension of the input-file-name. If the input option is omitted, the default format is SIM.
eigenproblem
This option specifies recovering the eigenmodes of an unsupported substructure. This calculation does not require input of the dynamic solution. This option is mutually exclusive with the input and format options.
minframevalue
This option specifies the lower boundary of the time or frequency range for results recovery. By default, the minimal available time or frequency value is used.
maxframevalue
This option specifies the upper boundary of the time or frequency range for results recovery. By default, the maximal available time or frequency value is used.
resultsformat
This option specifies the results output format: ODB, SIM, or BOTH. The default value is ODB.
output
This option specifies a list of output variables to recover. Variables in the list are separated by commas and/or spaces. If spaces are used, the list must be enclosed in quotes. This option is supported only for resultsformat=ODB.

Supported output requests:

  • U (displacement)
  • V (velocity)
  • A (acceleration)
  • S (stress)
  • E (strain)
  • MISES (Mises stress)
  • SP (principal stress)
  • EP (principal strain)
  • SPAM (principal absolute maximum stress)
  • EPAM (principal absolute maximum strain)
Principal stresses and strains and Mises stress are applicable only to element recovery averaged at nodes in the Abaqus substructure generation.
nset
This option specifies the node set names for results output. The node sets are defined in the Abaqus substructure generation model. Multiple node set names must be separated by commas. By default, results are recovered at all nodes associated with recovery matrices.
elset
This option specifies the element set names for results output. The element sets are defined in the Abaqus substructure generation model. Multiple element set names must be separated by commas. By default, results are recovered at all elements associated with recovery matrices.

Examples

The following examples illustrate different methods of recovering results from a substructure using the abaqus substructurerecover utility.

Recovering Results within a Substructure in an Abaqus-Simpack Flexible Body Dynamics Workflow

In an Abaqus-Simpack flexible body dynamics workflow, you may have the substructure generalized solution in a file with a .txt extension. In this case you can use the .txt file as input; however, you must use format=ASC as shown in the example below: 

abaqus substructurerecover job=recover2 substructure=substr_Z1 input=solutions.txt 
format=ASC resultsformat=SIM nset=NSET1,NSET2

Alternatively, you can rename the solutions.txt file to solutions.asc and omit the format argument.

Results are recovered for node sets NSET1 and NSET2 defined in the substructure generation finite element model. The recovered results are saved in a file named recover2.odb.

Recovering Results within a Substructure in an Abaqus-ADAMS Flexible Body Dynamics Workflow

Use the following command to recover results within a substructure in an Abaqus-ADAMS flexible body dynamics workflow: 

abaqus substructurerecover job=recover1 substructure=substr_Z1 input=solutions.mdf 
minframevalue=0.001 maxframevalue=0.01

Results are recovered in the time range from 0.001 to 0.01. The recovered results are saved in a file named recover1.odb.

Recovering Results within a Substructure in an Abaqus-EXCITE Flexible Body Dynamics Workflow

Use the following command to recover results within a substructure in an Abaqus-EXCITE flexible body dynamics workflow: 

abaqus substructurerecover job=recover3 substructure=substr_Z1 input=solutions.inp4 
output=U,MISES,SPAM

Results are recovered only for output variables U, MISES, and SPAM. The recovered results are saved in a file named recover3.odb.