Notation Used in the Output Variable Descriptions
The entries Field, History, and
.fil 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, and .fil
refers to a results 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.
Direction Definitions
The direction definitions depend on the variable type.
Direction Definitions for Element Variables
For components of stress, strain, and similar material variables, 1, 2, and
3 refer to the directions in an orthogonal coordinate system. These are global
directions for solid elements, surface directions for shell and membrane
elements, and axial and transverse directions for beam and pipe elements.
However, if a local orientation (Orientations)
is associated with the elements for which output is being requested, 1, 2, and
3 are local directions.
Direction Definitions for Nodal Variables
For nodal variables, 1, 2, and 3 refer to the global directions
(1=X, 2=Y, 3=Z
except for axisymmetric elements, in which case 1=R,
2=Z). Even if a local coordinate system has been defined
at a node (Transformed Coordinate Systems),
the data in the results file and the selected results file are still output in
the global directions.
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.
Abaqus/CAE
automatically uses this quaternion to transform the nodal results into the
local directions. 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 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/Explicit User Subroutines) are not
displayed.
Principal Value Output
Output of the principal values can be requested for stresses, logarithmic strains, and nominal
strains. Either all principal values or the minimum, intermediate, or maximum values can be
obtained. All principal values of tensor ABC are obtained with
the request ABCP, and the minimum, intermediate, and maximum
principal values are obtained with the requests
ABCP1,
ABCP2, and
ABCP3, respectively. For
three-dimensional, plane strain, and axisymmetric elements all three principal values are
obtained. For plane stress, membrane, and shell elements only the in-plane principal values
are obtained for history-type output, and the out-of-plane principal value cannot be
requested. For field-type output, Abaqus/CAE always assumes the out-of-plane principal value as zero, including when computing the
Max. Principal, Mid. Principal, and
Min. Principle values. Principal values cannot be obtained for
beam, pipe, and truss elements, and principal values of plastic strains cannot be requested.
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.
Abaqus/CAE
calculates all principal values and invariants from these components. If a
principal value is desired as history-type output, it must be requested
explicitly since
Abaqus/CAE
does no calculations on history data.
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 and pipe
elements), or the user-defined local system.
Abaqus/CAE
calculates all principal values and invariants from these components. See
Writing field output data, for a description of the different types of tensor
variables.
The components for tensor variables are written to the output database in single precision.
Therefore, a small amount of precision roundoff error can occur when calculating the
variables' principal values. Such roundoff error may be observed, for example, when
analytically zero values are calculated as relatively small yet nonzero values.
Requesting Output of Components
Individual components of variables can be requested as history-type output in the output database
for X–Y plotting in Abaqus/CAE. Individual component requests are not available for field-type output. If a particular
component is required for contouring in Abaqus/CAE, request field output of the generic variable (for example, S for stress). Output for
individual components of this field output can be requested within the Visualization module of Abaqus/CAE.
|