Products
Abaqus/Standard
Abaqus/Explicit
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
at SPOINTs are translated to MATRIX INPUT
viscous damping terms.) |
| 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 |
| BEAML |
| 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.
|
| MAT11 |
ELASTIC,
TYPE=ENGINEERING
CONSTANTS. Also DENSITY; EXPANSION,
TYPE=ANISO
or ORTHO; and
DAMPING. |
| ACMODL |
TIE between a
SURFACE,
TYPE=ELEMENT
defining the exterior surfaces of all acoustic solid elements and a
SURFACE
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 |
CONN3D2 and CONNECTOR SECTION
(Ignored unless the command line option
plotel=ON.)
|
| PLOTEL3
PLOTEL4 |
SFM3D3/SFM3D4
and SURFACE SECTION
(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
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
cpyram
linear-pyramid-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
-
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.
For input files created with
surface_based_coupling=ON,
the translated elements can be visualized and manipulated in Abaqus/CAE. However, large numbers of these elements may cause slower
performance.
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
-
cpyram
-
This option is used to define the 5-node pyramid that is created from
CPYRAM elements. The default is
C3D5. You can specify an
8-node brick element type, which degenerates to the appropriate pyramid
shape.
-
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,
PLOTEL3, and
PLOTEL4 elements are translated as
described above.
-
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.
|