|
Using the Translator
The following procedure summarizes the typical usage of the
abaqus adams translator:
-
Create an Abaqus substructure. (General guidelines for building Abaqus models with substructures are described in Using Substructures.)
The substructure generation step must write at least the mass and stiffness matrices.
It can also write the recovery and viscous damping matrices. The FLEXIBLE BODY option must be
used. For example,
SUBSTRUCTURE GENERATE, MASS MATRIX=YES, RECOVERY MATRIX=YES, VISCOUS DAMPING MATRIX=YES
FLEXIBLE BODY, TYPE=ADAMS
-
If
TYPE=ADAMS,
a flexible body including all high-order inertia invariants is created.
-
If
TYPE=ADAMS,
FORMULATION=REDUCED,
a simplified flexible body (without high-order inertia invariants I5 and I9) is
created.
In addition, you can add the following data to translate stress and/or strain: ELEMENT RECOVERY MATRIX, POSITION=AVERAGED AT NODES
S,
E,
If the Abaqus analysis did not use SI units (meters, kilograms,
Newtons, and seconds), you must define units when you run the translator using the
length,
mass, force,
and time command line options. If the Abaqus analysis uses American or English units (inches, pounds force, and seconds), the mass
unit is slinch.
-
Run the
Abaqus
analysis.
-
Run the abaqus adams translator to read the
substructure SIM database produced by the
analysis and to create the modal neutral file.
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.
Command Summary
abaqus adams
job
job-name
substructure_sim
filename
length
length-units-name
mass
mass-units-name
time
time-units-name
force
force-units-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.
- length
-
This option specifies the length units
for the model. The valid options are as follows:
- m, meter, meters
- mm, millimeter,
millimeters
- cm, centimeter,
centimeters
- km, kilometer, kilometers
- in, inch, inches
- ft, foot, feet
- mile, miles
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. The valid options are as follows:
- kg, kilogram, kilograms
- mgg, megagram, megagrams, tonne,
tonnes
- gram, grams
- lbm, pound, pounds,
pound_mass
- uston, ustons, us_ton
- klbm, kpound_mass
- ozm, ounce, ounces,
ounce_mass
- slug
- slinch, dozen_slug
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. The valid options are as follows:
- s, sec, second, seconds
- ms, millisecond,
milliseconds
- min, minute, minutes
- h, hr, hour, hours
This option can be defined in the
Abaqus
environment file as follows:
adams_time_units=time-unit
- force
-
This option specifies the force units
for the model. The valid options are as follows:
- n, newton, newtons
- kn, knewton, knewtons, kilonewton,
kilonewtons
- mn, millinewton,
millinewtons,
- un, micronewton,
micronewtons,
- nn, nanonewton,
nanonewtons,
- kgf, kg_force,
kilogram_force
- lbf, pound, pounds,
pound_force
- ozf, ounce, ounces,
ounce_force
- dyne, dynes
- klbf, kip, kips, kilopound, kilopounds,
kpound_force
This option can be defined in the
Abaqus
environment file as follows:
adams_force_units=force-unit
|