|
Converting Nastran Bulk Data in Text Files to Abaqus Input Files
The Nastran data must be in a file with the extension
.bdf, .dat,
.nas, .nastran,
.blk, or .bulk. The Nastran data
entries that are translated are listed in the tables below. Other valid Nastran
data are skipped over and noted in the log file.
The translator is designed to translate a complete Nastran input file. If
only bulk data are present, the first two lines in the file should be the
terminators for the executive control and case control sections, namely:
CEND
BEGIN BULK
For normal termination, end the Nastran input data with the line
ENDDATA
Nastran solution sequences are translated to the
Abaqus
procedures listed in
Table 1.
The translator attempts to create a history section based on the contents of
the case control data in the Nastran file.
Converting Nastran DMIG Matrix Data in Bulk Data Text Files to an Abaqus Binary SIM File
You can specify that the translator create a
SIM file of matrix data in addition to a text
input file. The matrix data can be translated to
- a SIM file structured as if it were
created from a
MATRIX GENERATE step in an
Abaqus
input file or
- a SIM file equivalent to that resulting
from an
Abaqus
analysis with a
SUBSTRUCTURE GENERATE step.
Converting Nastran DMIG Matrix Data in Output2 Binary Files to an Abaqus Binary SIM File
The Nastran matrix data can be in one or more binary Output2 files. The
DMIG matrix data are assumed to be written to
an Output2 file using a command as follows: ASSIGN OUTPUT2='jobname_matrixdata.op2',UNIT=30
…
EXTSEOUT(STIFFNESS,
MASS,
DAMPING,
K4DAMP,
LOADS,
ASMBULK,
EXTBULK,
EXTID=10,
DMIGOP2=30)
The nodal coordinate data may be in a second Output2 file, created with a
command as follows: ASSIGN OUTPUT2='jobname.op2',UNIT=12
…
DISP(PLOT) = ALL
…
PARAM,POST,-2
These Output2 files are referenced by the
op2file1 and
op2file2 options. The use of
op2file2 is optional. Using the file names
from the example above, you specify the command line options as follows: op2file1=jobname_matrixdata.op2 op2file2=jobname.op2
The op2target option determines the
type of matrix data to create. The matrix data can be translated to
- a partial
Abaqus
input file with a
MATRIX INPUT representation of the matrix data,
- a SIM file structured as if it were
created from a
MATRIX GENERATE step in an
Abaqus
input file, or
- a SIM file equivalent to that resulting
from an
Abaqus
analysis with a
SUBSTRUCTURE GENERATE step.
Summary of Nastran Entities Translated
Table 2. Case control data.
| Nastran Command
|
Comment
|
| SPC
|
Selects
SPC sets alone or in combinations
|
| LOAD
|
Selects individual loads and load
combinations
|
| METHOD
|
Selects
EIGRL, EIGR,
or EIGB from bulk data for eigenfrequency
extraction and eigenvalue buckling prediction procedures
|
| SUBCASE
|
Delimiter for steps or load cases;
optional if there is only one step
|
| TITLE
|
Echoed as comment at top of input file
and for each step
|
| SUBTITLE
|
Echoed as comment for the step to which
it applies
|
| LABEL
|
Used as text following the
STEP option
|
| DLOAD
|
Selects dynamic loads from
bulk data
|
| LOADSET
|
| FREQUENCY
|
Selects forcing frequencies from bulk
data
|
| MPC
|
Selects
MPCADD and
MPC from bulk data if referenced in the first
SUBCASE
|
| SUPORT1
|
Selects
SUPORT1 from bulk data
|
| TSTEP
|
Selects
TSTEP from bulk data
|
| K2GG
|
Selects DMIG from
bulk data using the matrix name from the first
SUBCASE
|
| K2PP
|
| M2GG
|
| M2PP
|
| B2GG
|
| B2PP
|
| K42GG
|
| TEMPERATURE
|
Selects nodal temperatures from bulk data
|
| SET
|
Selects nodal quantities for output
|
| DISPLACEMENT
|
| VELOCITY
|
| ACCELERATION
|
| SPCFORCES
|
| PRESSURE
|
Table 3. Bulk data.
| Nastran Data Entry |
Comment |
| PARAM
|
Ignored except
for:1. WTMASS, which can
be used to modify density, mass, and rotary inertia values if the
wtmass_fixup command line
parameter is used2.
INREL, which if equal to −1 or −2
will create inertia relief loads3.
G, which is translated to GLOBAL DAMPING,
STRUCTURAL,
FIELD=MECHANICAL4.
GFL, which is translated to
GLOBAL DAMPING,
STRUCTURAL,
FIELD=ACOUSTIC
|
| CDAMP1
|
DASHPOT1/DASHPOT2
and DASHPOT
|
| CDAMP2
|
| PDAMP
|
| PDAMPT
|
| CELAS1
|
SPRING1/SPRING2
and SPRING(CELAS2
at SPOINTs are translated to MATRIX INPUT,
stiffness, and/or structural damping terms.) |
| CELAS2
|
| PELAS
|
| PELAST
|
| CMASS2
|
MATRIX INPUT
mass terms |
| CBUSH
|
CONN3D2 and CONNECTOR SECTION
|
| PBUSH
|
| PBUSHT
|
| CWELD
|
FASTENER
and FASTENER PROPERTY
|
| PWELD
|
| CONM1
|
MASS and/or
ROTARY
INERTIA
and/or UEL
|
| CONM2
|
MASS
and/or
ROTARY
INERTIA
|
| CHEXA
|
C3D8I/C3D20R/C3D6/C3D15/C3D4/C3D10
and SOLID SECTION
|
| CPENTA
|
| CTETRA
|
| PSOLID
|
| PLSOLID
|
| CQUAD4
|
S4/S3R/S8R/STRI65,
and SHELL SECTION,
SHELL GENERAL SECTION,
or MEMBRANE SECTION.
|
| CTRIA3
|
| CQUAD8
|
| CTRIA6
|
| CQUADR
|
| CTRIAR
|
| PSHELL
|
| PCOMP
|
| PCOMPG
|
| CSHEAR
|
USER ELEMENT,
LINEAR and MATRIX,
TYPE=STIFFNESS
and
TYPE=MASS,
or SHEAR4 and SHELL GENERAL SECTION |
| PSHEAR
|
| CBAR
|
B31
and BEAM SECTION
or BEAM GENERAL SECTION
|
| CBEAM
|
| PBAR
|
| PBARL
|
| PBEAM
|
| PBEAML
|
| CROD
|
T3D2 and SOLID SECTION
|
| CONROD
|
| PROD
|
| CGAP
|
GAPUNI and GAP
|
| PGAP
|
| RBAR
|
COUPLING
or MPC, type
BEAM
|
| MAT1
|
ELASTIC,
TYPE=ISO;
EXPANSION,
TYPE=ISO;
DENSITY;
and DAMPING
(G is used only for BEAM GENERAL SECTION)
|
| MAT2 |
When used alone in a PSHELL, MAT2 is translated to ELASTIC,
TYPE=LAMINA
or ELASTIC,
TYPE=ANISOTROPIC.
When used in combination with other materials, the coefficients
relating midsurface strains and curvatures to section forces and
moments are computed and entered following the SHELL GENERAL SECTION
option. |
| MAT8
|
ELASTIC,
TYPE=LAMINA;
EXPANSION,
TYPE=ORTHO;
DENSITY;
and DAMPING
|
| MAT9
|
ELASTIC,
TYPE=ANISOTROPIC
unless the data are found to be orthotropic, in which case the data
are analyzed to create ELASTIC,
TYPE=ENGINEERING
CONSTANTS.
Also DENSITY;
EXPANSION,
TYPE=ANISO
or ORTHO; and
DAMPING.
|
| MAT10
|
ACOUSTIC MEDIUM;
DENSITY
and DAMPING
|
| ACMODL
|
TIE
between a SURFACE,
TYPE=ELEMENT
defining the exterior surfaces of all acoustic solid elements and a
SURFACE,
TYPE=NODE
defined by the SET1 referenced by
the SSID. |
| NSM
|
NONSTRUCTURAL MASS
|
| NSM1
|
| NSML
|
| NSML1
|
| NSMADD
|
| GRID
|
NODE and
SYSTEM
|
| CORD1R
|
SYSTEM for
nodes; TRANSFORM
if referred to on GRID; ORIENTATION
for some elements |
| CORD1C
|
| CORD1S
|
| CORD2R
|
| CORD2C
|
| CORD2S
|
| RBE2
|
COUPLING
and KINEMATIC;
or KINEMATIC COUPLING(If
the RBE2 has only two nodes and neither node has rotational
stiffness, the RBE2 is translated to MPC, type
LINK) |
| RBE3
|
COUPLING
and DISTRIBUTING;
or DCOUP3D and DISTRIBUTING COUPLING
|
| SPCADD
|
Used to combine
SPC/SPC1/SPCD
data into a new set |
| SPC
|
BOUNDARY
|
| SPC1
|
| SPCD
|
| LOAD
|
Used to combine
FORCE,
MOMENT, etc. data into a new
set |
| FORCE
|
CLOAD
|
| FORCE1
|
| FORCE2
|
| MOMENT
|
| MOMENT1
|
| MOMENT2
|
| PLOAD
|
DLOAD
|
| PLOAD1
|
| PLOAD2
|
| PLOAD4
|
| RFORCE
|
| DLOAD
|
Dynamic loads as functions of time or
frequency |
| DAREA
|
| LSEQ
|
| RLOAD1
|
| RLOAD2
|
| TLOAD1
|
| TABLED1
|
| TABLED2
|
| TABLED4
|
| DELAY
|
| DPHASE
|
| TEMP
|
INITIAL CONDITIONS,
TYPE=TEMPERATURE
and TEMPERATURE
|
| TEMPD
|
| TSTEP
|
Time step size for dynamic and modal dynamic
procedures |
| EIGB
|
BUCKLE
|
| EIGR
|
FREQUENCY
|
| EIGRL
|
| EIGC
|
COMPLEX FREQUENCY
|
| TABDMP1
|
MODAL DAMPING
|
| FREQ
|
Forcing frequencies for
steady-state dynamic procedures |
| FREQ1
|
| FREQ2
|
| FREQ3
|
| FREQ4
|
| FREQ5
|
| MPCADD
|
EQUATION
|
| MPC
|
| SUPORT
|
INERTIA RELIEF
and BOUNDARY
|
| SUPORT1
|
| DMIG
|
MATRIX INPUT
and MATRIX ASSEMBLE
|
| GENEL
|
USER ELEMENT,
LINEAR and MATRIX,
TYPE=STIFFNESS
|
| PLOTEL
|
T3D2 (Ignored
unless the command line option
plotel=ON.)
|
Command Summary
abaqus
fromnastran
job
job-name
input
input-file
wtmass_fixup
{
OFF
ON
}
loadcases
{
OFF
ON
}
pbar_zero_reset
small-real-number
distribution
{
OFF
preservePID
ON
}
surface_based_coupling
{
OFF
ON
}
beam_offset_coupling
{
OFF
ON
}
beam_orientation_vector
{
OFF
ON
}
cbar
2-node-beam-element
cquad4
4-node-shell-element
chexa
8-node-brick-element
ctetra
10-node-tetrahedron-element
cshear
{
UEL
SHEAR4
}
plotel
{
OFF
ON
}
cdh_weld
{
OFF
RIGID
COMPLIANT
}
dmig2sim
{
GENERIC
SUBSTRUCTURE
}
op2file1
op2-filename-1
op2file2
op2-filename-2
op2target
{
INPUT
GENERIC
SUBSTRUCTURE
}
Command Line Options
- job
-
This option is used to specify the name of the
Abaqus
input file to be output by the translator. It is also the default name of the
file containing the Nastran data. Diagnostics created by the translator will be
written to a file named
job-name.log.
- input
-
This option is used to specify the name of the file containing the Nastran
data if it is different from job-name.
- wtmass_fixup
-
If
wtmass_fixup=ON,
the value on the Nastran data line PARAM, WTMASS,
value is used as a multiplier for
all density, mass, and rotary inertia values created in the
Abaqus
input file.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_wtmass_fixup={OFF | ON}
- loadcases
-
By default, each SUBCASE is translated to a
STEP option in
Abaqus.
If
loadcases=ON,
this behavior is altered for linear static analyses: each
SUBCASE is translated to a
LOAD CASE option, and all such
LOAD CASE options are grouped in a single
STEP option.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_loadcases={OFF | ON}
- pbar_zero_reset
-
Nastran allows beams to have zero values for cross-sectional area or moments
of inertia;
Abaqus
does not. Set this option equal to a small real number to reset any zero values
for A, ,
,
or J to the specified small real number. If this option is
omitted or present without a value, the default value of 1.0 × 10−20
is used in place of the zeros. To retain the zeros in the translated
Abaqus
input file, set
pbar_zero_reset=0.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_pbar_zero_reset=small-real-number
- distribution
-
This option determines how shell and membrane sections in Nastran data are
translated to
Abaqus.
If
distribution=OFF,
a separate section is created for each combination of orientation, material
offset, and/or thickness. If
distribution=preservePID
or ON, element orientations and
offsets are written using the
DISTRIBUTION option. If
distribution=preservePID,
an
Abaqus
section is created corresponding to each
PSHELL or
PCOMP property
ID. If
distribution=ON,
a single
Abaqus
section is created for all homogeneous elements referencing the same material.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_distribution={OFF | preservePID | ON}
- surface_based_coupling
-
Certain Nastran rigid elements have more than one equivalent in
Abaqus.
If
surface_based_coupling=ON,
RBE2 and RBE3
elements translate to
COUPLING with the appropriate parameters. Otherwise,
RBE2 elements translate to
KINEMATIC COUPLING and RBE3 elements
translate to
DISTRIBUTING COUPLING. This translation behavior also applies to
implied RBE2-type rigid
elements used for offsets on CBAR,
CBEAM, and
CONM2 elements.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_surface_based_coupling={OFF | ON}
- beam_offset_coupling
-
If
beam_offset_coupling=ON,
beam element offsets are translated by creating new nodes at the offset
locations, changing the beam connectivity to the new nodes, and rigidly
coupling the new and original nodes.
If
beam_offset_coupling=OFF,
beam element offsets are translated to the
CENTROID and
SHEAR CENTER options, which are suboptions of the
BEAM GENERAL SECTION option.
The setting for this parameter is ignored if the beam element references a
PBARL or
PBEAML property or if the beam offset has a
significant component in the direction of the beam axis. In these situations
the beam offsets are always translated as if
beam_offset_coupling=ON.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_beam_offset_coupling={OFF | ON}
- beam_orientation_vector
-
If
beam_orientation_vector=OFF,
beam cross-section orientations are translated by creating new nodes at the
tips of vectors defining the first principal direction of the cross-section and
changing the beam connectivity to the new nodes.
If
beam_orientation_vector=ON,
beam cross-sections are translated by defining vectors on the
BEAM SECTION and
BEAM GENERAL SECTION options.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_beam_orientation_vector={OFF | ON}
- cbar
-
This option is used to define the 2-node beam that is created from
CBAR and
CBEAM elements. The default is B31.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_cbar=2-node-beam-element
- cquad4
-
This option is used to define the 4-node shell that is created from
CQUAD4 elements. The default is S4R. If a reduced-integration element is chosen, the enhanced
hourglass formulation is applied automatically.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_cquad4=4-node-shell-element
- chexa
-
This option is used to define the 8-node brick that is created from
CHEXA elements. The default is C3D8I. If a reduced-integration element is chosen, the enhanced
hourglass formulation is applied automatically.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_chexa=8-node-brick-element
- ctetra
-
This option is used to define the 10-node tetrahedron that is created from
CTETRA elements. The default is C3D10.
This option can be defined in the
Abaqus
environment file as follows:
fromnastran_ctetra=10-node-tetrahedron-element
- cshear
-
By default, CSHEAR elements are translated to user
elements, as described in Table 3. If
cshear=SHEAR4,
CSHEAR elements are translated to
SHEAR4 elements.
- plotel
-
By default, PLOTEL elements are not
translated. If
plotel=ON,
PLOTEL elements are translated to
T3D2 truss elements in an element set named
PLOTEL_TRUSSES. The cross-sectional area of
the trusses is 1.0 × 10−20, and the material has a Young's modulus,
E, equal to 1.0.
- cdh_weld
-
By default, CHEXA elements with
RBE3 elements at all eight corner nodes are
translated to the type of 8-node element specified in the
chexa parameter. If
cdh_weld=RIGID,
CHEXA elements with
RBE3 elements at all eight corner nodes are
translated to rigid fasteners in
Abaqus.
If
cdh_weld=COMPLIANT,
CHEXA elements with
RBE3 elements at all eight corner nodes are
translated to compliant fasteners in
Abaqus.
- dmig2sim
-
This option is used to write DMIG matrix
data to a binary SIM file for further
processing by
Abaqus.
If
dmig2sim=GENERIC,
a SIM file with a generic matrix system
equivalent to that produced by a
MATRIX GENERATE step is created.
If
dmig2sim=SUBSTRUCTURE,
a SIM file with a substructure matrix system
equivalent to that produced by a
SUBSTRUCTURE GENERATE step is created.
- op2file1
- This option is used only in a workflow that reads
DMIG matrix data in an Output2 file. It
specifies the name of an Output2 file containing
DMIG matrix data. The complete file name with
the extension must be given.
- op2file2
- This option is used to give the name of a second Output2
file containing nodal coordinate data associated with
DMIG entries. If the
op2file1 option is present, specifying
op2file2 is optional. If specified, the
complete file name with the extension must be
given.
- op2target
-
This option controls the translation behavior for the
DMIG matrix data in an Output2 file.
If
op2target=INPUT,
a partial
Abaqus
input file containing a
MATRIX INPUT option is created.
If
op2target=GENERIC,
a SIM file with a generic matrix system
equivalent to that produced by a
MATRIX GENERATE step is created.
If
op2target=SUBSTRUCTURE,
a SIM file with a substructure matrix system
equivalent to that produced by a
SUBSTRUCTURE GENERATE step is created.
|