Translating Abaqus data to MSC.ADAMS modal neutral files

The ADAMS/Flex product from MSC.Software Corporation can be used to account for flexibility in a component when performing a dynamic analysis in MSC.ADAMS. ADAMS/Flex relies on a finite element analysis code such as Abaqus to provide the component's flexibility information in a form that is usable by MSC.ADAMS. The abaqus adams translator can be used to create Abaqus models of MSC.ADAMS components and to convert the Abaqus results into an MSC.ADAMS modal neutral (.mnf) file, the format required by ADAMS/Flex.

The following topics are discussed:

Related Topics
About Execution Procedures
In Other Guides
Translating Abaqus data to modal neutral file format for analysis in MSC.ADAMS

ProductsAbaqus/Standard

Using the translator

The following procedure summarizes the typical usage of the abaqus adams translator:

  1. Create an Abaqus model for each flexible component of the MSC.ADAMS model. Each component is modeled as an Abaqus substructure.

  2. Run the Abaqus analysis. For more information, see Preparing the substructure SIM database file.

  3. Run the abaqus adams translator to read the substructure SIM database produced by the analysis and to create the modal neutral (.mnf) file for MSC.ADAMS.

  4. Read the modal neutral file into MSC.ADAMS. A separate modal neutral file must be created for each flexible part in MSC.ADAMS.

Preparing the substructure SIM database file

This section describes the preparation of a substructure SIM database that will produce the results quantities required by ADAMS/Flex.

The Abaqus substructure model

The first step in accounting for a component's flexibility in MSC.ADAMS is to model that component as an Abaqus substructure. This process involves creating an Abaqus finite element model of the component. General guidelines for building Abaqus models with substructures are described in Using substructures.

Setting up the Abaqus model to create a modal neutral file

When you create a substructure to be translated to MSC.ADAMS, the substructure generation step must include the following options: 

SUBSTRUCTURE GENERATE, MASS MATRIX=YES, RECOVERY MATRIX=YES
FLEXIBLE BODY, TYPE=ADAMS

In addition, you can add the following data to translate stress and/or strain to MSC.ADAMS: 

*ELEMENT RECOVERY MATRIX, POSITION=AVERAGED AT NODES
S,
E,

Units

The MSC.ADAMS programs require that you define the units, while Abaqus does not. Therefore, during the creation of the modal neutral file you must declare the units used in the model explicitly.

The default unit system in MSC.ADAMS is the International System of units (SI). If the Abaqus analysis uses SI units (meters, kilograms, Newtons, and seconds), you do not need to specify the units when you run the translator. If the Abaqus analysis uses American or English units (inches, pounds force, and seconds), the mass unit is slinch.

The valid options for each of the length, mass, and time options are as follows:

Length units

  • meters (default)

  • millimeters, mm

  • centimeters, cm

  • kilometers, km

  • inches, inch, in

  • feet, foot, ft

Mass units

  • kilograms, kg (default)

  • megagram, tonne

  • gram, g

  • slug

  • slinch

Time units

  • seconds, sec (default)

  • milliseconds, ms

Default values for the units options can be defined in the Abaqus environment file. The defaults for the length, mass, and time options can be defined with the adams_length_units, adams_mass_units, and adams_time_units parameters, respectively.

Translating modes with negative eigenvalues

Typically, for a non-prestressed, unrestrained substructure in three dimensions, you expect to find six rigid body modes with associated zero eigenvalues. The situation is, in general, different for prestressed substructures, which may have fewer than six modes with zero eigenvalues. Prestressing may change some expected zeroes into values that are significantly positive or negative, depending on the sign of the prestress.

By default, the translator deletes modes with negative eigenvalues and reorthogonalizes the reduced basis. If you want to retain modes with negative eigenvalues, define the environment variable MDI_MNFWRITE_OPTIONS.

  • On Linux platforms type the following command: 

    setenv MDI_MNFWRITE_OPTIONS negative_roots_OK

  • On Windows platforms type the following command: 

    set MDI_MNFWRITE_OPTIONS=negative_roots_OK

In this case the translator will treat modes with negative eigenvalues in the same manner as all other modes.

To determine if a model will have negative eigenvalues when translated by the translator, you can add an eigenfrequency extraction step with no boundary conditions to the input file.

Command summary

abaqus adamsjobjob-name substructure_simfilename units{mmksmkscgsips} lengthlength-units-name massmass-units-name timetime-units-name mnf_elsetelset-name

Command line options

job

This option specifies the input and output file names to use during results translation. The job-name value is used to construct the default substructure SIM database file name, job-name.sim. The output modal neutral file is given the name job-name.mnf.

If this option is omitted from the command line, the user will be prompted for this value.

substructure_sim

This option specifies the name of the substructure SIM database (.sim) file if it is different from job-name.sim. The file will usually be named job-name_Znn.sim.

units

This option specifies the units system for the model. The possible values are mmks, mks, cgs, or ips, which correspond to the ADAMS/View options with the same names. The default value is mks.

This option can be defined in the Abaqus environment file as follows: 

adams_unit_family=unit-family
length

This option specifies the length units for the model. If this option is specified, it overrides the length units of the specified units system.

This option can be defined in the Abaqus environment file as follows: 

adams_length_units=length-unit
mass

This option specifies the mass units for the model. If this option is specified, it overrides the mass units of the specified units system.

This option can be defined in the Abaqus environment file as follows: 

adams_mass_units=mass-unit
time

This option specifies the time units for the model. If this option is specified, it overrides the time units of the specified units system.

This option can be defined in the Abaqus environment file as follows: 

adams_time_units=time-unit
mnf_elset

This option defines a set of elements whose facets will be exported to the modal neutral file and, therefore, will be available for viewing in MSC.ADAMS. This option does not affect the mechanics of the solution.