Notation Used in the Output Variable Descriptions
The entries Field, History,
.fil, and .dat in the output variable's
description indicate the availability of the output variable. Field
refers to a field-type output selection to the output database,
History refers to a history-type output selection to the output
database, .fil refers to a results file output selection, and
.dat refers to a data file output selection. The output variable
can be written to the respective file if the word yes appears after
the category name; no means that the variable is not available to
that file.
If the word automatic appears after a category name, the variable cannot
be requested by name; it is written to the respective files according to the conditions
specified in the text.
Requesting Output of Components
Variable identifiers of the form
ABCn can be used with
(ABC1, ABC2, …), where
the highest value of n is determined by the type of
variable. Similarly, variable identifiers of the form
DEF
can be used for the ranges of i and
j indicated (DEF11,
DEF12, ).
Individual components cannot be requested in the results
(.fil) file. For postprocessing of a particular component
of a variable, request file output for all components of the variable. Output
for individual variables can be requested during postprocessing.
Direction Definitions
The direction definitions depend on the variable type.
Direction Definitions for Element Variables
For components of stress, strain, and other tensor quantities 1, 2, and 3
refer to the directions in an orthogonal coordinate system. These directions
are global directions for solid elements, surface directions for shell and
membrane elements, and axial and transverse directions for beam elements. For
finite-membrane-strain shell elements, membrane elements, and continuum
elements associated with a local orientation (see
Orientations),
the local output directions rotate with the average rotation of the element
(integral with respect to time of the spin—see
Stress rates).
Tensor components in these cases are output in the rotating local directions.
In some cases the local output directions may differ from one integration
point to the next within an element.
Abaqus/Standard
does not take this variation into account when extrapolating output variables
to the nodes, which affects output such as element quantities averaged at the
nodes or contour plots of individual tensor components. Invariant quantities at
the integration points will not be influenced by the local output directions.
You can control writing the local directions to the output database file or
to the results file (see
Specifying the Directions for Element Output
and
Output of Local Directions to the Results File).
By default, the local directions are written to the output database for all
frames that include element field output.
The directions can be printed to the data file by using user subroutine
UVARM.
Direction Definitions for Equivalent Rigid Body Variables
For all equivalent rigid body variables 1, 2, and 3 refer to global
directions.
Direction Definitions for Nodal Variables
For nodal variables 1, 2, and 3 are global directions
(1=X, 2=Y, and
3=Z; or for axisymmetric elements,
1=r and 2=z). If a local coordinate
system is defined at a node (see
Transformed Coordinate Systems),
you can specify whether output to the data or results file of vector-valued
quantities at these nodes is in the local or global system (see
Specifying the Directions for Nodal Output).
By default, nodal output is written to the data file in the local system,
whereas it is written to the results file in the global system (since this is
more convenient for postprocessing).
If nodal field output is requested for a node that has a local coordinate
system defined, a quaternion representing the rotation from the global
directions is written to the output database.
Nodal history data written to the output database are always stored in
the global directions.
Direction Definitions for Integrated Variables
For components of total force, total moment, and similar variables obtained
through integration over a surface, the directions 1, 2, and 3 refer to
directions in an orthogonal coordinate system. A fixed global coordinate system
is used if the surface is specified directly for the integrated output request.
If the surface is identified by an integrated output section definition (see
Integrated Output Section Definition)
that is associated with the integrated output request, a local coordinate
system in the initial configuration can be specified and can translate or
rotate with the deformation.
Distributed Load Output
You need to be aware of limitations that may be encountered when distributed
load output is requested.
Distributed Load Output and User Subroutines
Output can be requested for many of the distributed loads discussed in
Loads.
However, contributions to these loads defined through user subroutines (see Abaqus/Standard User Subroutines) are
not displayed, except for the variables
FILMCOEF and
SINKTEMP.
Distributed Load Output with Modal Procedures
For modal procedures only the magnitude of the load is written to the output
database.
Strain Output
The total strain E is composed of the elastic strain EE, the inelastic strain IE, and the thermal strain THE. The inelastic strain IE consists of the plastic strain PE and the creep strain CE.
For geometrically nonlinear analysis
Abaqus/Standard
makes it possible to output different strain measures as well as elastic and
various inelastic strains. The various total strain measures (integrated strain
measure E, nominal strain measure NE, and logarithmic strain measure LE) are described in
Conventions.
The default strain measure for output to the data (.dat)
and results (.fil) files is E. However, for geometrically nonlinear analysis using element
formulations that support finite strains, E is not available for output to the output database
(.odb) file, and LE is the default strain measure.
Temperature Output
In
Abaqus
temperature can either be a field variable (stress analysis, mass diffusion, …)
or a degree of freedom (heat transfer analysis, fully coupled
temperature-displacement analysis, …). For any analysis that involves
temperature, you can request the temperature either at nodes (variable NT) or in elements (variable TEMP). If element temperature output is requested at the nodes, the
integration point values are extrapolated and, if requested, averaged. These
extrapolated values are generally not as accurate as the nodal temperatures
themselves. An exception to this is adiabatic analysis, in which the element
temperatures change due to plastic heat generation but the nodal temperatures
are not updated. In that case the current nodal temperatures are obtained only
if element temperature output is requested at the nodes.
For continuum elements there is only one temperature value per node (NT11). For shells and beams more than one temperature is available
for each node (NT11, NT12, …) since a temperature gradient can exist through the
thickness of a shell or across the cross-section of a beam. In general,
variables NT12, NT13, etc. contain temperature values. However, when temperature is
defined by specifying temperature gradients, nodal temperatures for a given
section point can be obtained only by using the variable TEMP. See
Specifying Temperature and Field Variables
and
Specifying Temperature and Field Variables
for discussions on specifying temperatures in beams and shells.
Principal Value Output
Output of the principal values can be requested for stresses, strains, and
other material tensors. Either all principal values or the minimum, maximum, or
intermediate values can be obtained. All principal values of tensor
ABC are obtained with the request
ABCP. The minimum, intermediate, and maximum
principal values are obtained with the requests
ABCP1,
ABCP2, and
ABCP3.
For three-dimensional, (generalized) plane strain, and axisymmetric elements all three principal
values are obtained. For plane stress, membrane, and shell elements, the out-of-plane
principal value cannot be requested for history-type output. Principal values cannot be obtained for
truss elements or for any beam elements other than the three-dimensional beam elements with
torsional shear stresses.
If a principal value or an invariant is requested for field-type output, the
output request is replaced with an output request for the components of the
corresponding tensor.
Tensor Output
Tensor variables that are written to the output database as field-type
output are written as components in either the default directions defined by
the convention given in
Orientations
(global directions for solid elements, surface directions for shell and
membrane elements, and axial and transverse directions for beam elements), or
the user-defined local system.
For plane stress, membrane, and shell elements, only the in-plane tensor
components (11, 22, and 12 components) are stored by
Abaqus/Standard.
The out-of-plane direct component for stress (S33) is reported as zero to the output database as expected, and
the out-of-plane component of strain (E33) is reported as zero even though it is not. This is because the
thickness direction is computed based on section properties rather than at the
material level. The out-of-plane components can be requested for field-type
output and cannot be requested for history-type output. The out-of-plane stress
components are not reported to the data (.dat) file or to
the results (.fil) file.
For three-dimensional beam elements with torsional shear stresses, only the
axial and the torsional components (the 11 and 12 components) are stored by
Abaqus/Standard.
The other direct component (the 22 component) is reported as zero for
field-type output and cannot be requested for history-type output.
The components for tensor variables are written to the output database in
single precision. Therefore, a small amount of precision roundoff error may
occur when calculating the variables' principal values. Such roundoff error may
be observed, for example, when analytically zero values are calculated as
relatively small nonzero values.
|