Product: Abaqus/Standard
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 procedure summarizes the typical usage of the abaqus adams translator:
Create an Abaqus model for each flexible component of the MSC.ADAMS model. Each component is modeled as an Abaqus substructure.
Run the Abaqus analysis. For more information, see “Preparing the substructure SIM database file.”
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.
Read the modal neutral file into MSC.ADAMS. A separate modal neutral file must be created for each flexible part in MSC.ADAMS.
This section describes the preparation of a substructure SIM database that will produce the results quantities required by ADAMS/Flex.
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,” Section 10.1.1.
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=ADAMSIn 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,
The MSC.ADAMS programs require that you define the units used in the component model, while Abaqus does not. Therefore, during the creation of the modal neutral file you must declare the units used in the model explicitly. The approach to doing this in the abaqus adams execution procedure is very similar to the way it is done in the ADAMS/View Units Settings dialog box. A predefined units system can be specified by using the units option on the abaqus adams execution procedure. Alternatively, the individual length, mass, force, and time units can be specified by using the length, mass, force, and time options on the abaqus adams execution procedure. Any individual units that are specified override the corresponding units in the units system. The default units system is mks. The valid units systems for the units option are listed in Table 3.2.38–1.
Table 3.2.38–1 Valid units systems.
| Units System | Length Units | Mass Units | Force Units | Time Units |
|---|---|---|---|---|
| mks | meters | kilograms | newtons | seconds |
| mmks | millimeters | kilograms | newtons | seconds |
| cgs | centimeters | grams | dyne | seconds |
| ips | inches | pound-mass | pound-force | seconds |
The valid options for each of the length, mass, force, and time options are as follows:
Length units
Valid options for the length units are
meters
millimeters, mm
centimeters, cm
kilometers, km
inches, inch, in
feet, foot, ft
mile
Mass units
Valid options for the mass units are
kilograms, kg
megagram, tonne
gram, g
pound_mass, lbm, pound
slug
kpound_mass
ounce_mass
Force units
Valid options for the force units are
newtons, N
knewton, kN
kilogram_force, kgf
dyne
ounce_force
pound_force, lbf, pound
kpound_force
Time units
Valid options for the time units are
seconds, sec
milliseconds, ms
minutes, min
hours
Default values for the units options can be defined in the Abaqus environment file. The default for the units option can be defined with the adams_units_family parameter. The defaults for the length, mass, time, and force options can be defined with the adams_length_units, adams_mass_units, adams_time_units, and adams_force_units parameters, respectively.
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
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.
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.
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.
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
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
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
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
This option specifies the force units for the model. If this option is specified, it overrides the force units of the specified units system.
This option can be defined in the Abaqus environment file as follows:
adams_force_units=force-unit
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.