- DIRECTIONS
-
This parameter applies only to
Abaqus/Standard
analyses.
This parameter is used to obtain the directions of local element or material
coordinate systems when component output is requested. The directions are
written as a separate record for each point at which a local coordinate system
is used. See
Results file output format
for a detailed description.
Set DIRECTIONS=NO (default) if the local coordinate directions should not be
written.
Set DIRECTIONS=YES if the local coordinate directions should be written.
- ELSET
-
Set this parameter equal to the name of the element set for which this
output request is being made. If this parameter is omitted, the output will be
written for all elements in the model. In an
Abaqus/Explicit
analysis, output will also be written for all of the rebars in the model. The REBAR parameter must be included in an
Abaqus/Standard
analysis to obtain rebar output.
- FREQUENCY
-
This parameter applies only to
Abaqus/Standard
analyses.
Set this parameter equal to the output frequency, in increments. The output
will always be written to the results file at the last increment of each step
unless FREQUENCY=0. The default is FREQUENCY=1. Set FREQUENCY=0 to suppress the output.
- LAST MODE
-
This parameter applies only to
Abaqus/Standard
analyses.
This parameter is useful only during eigenvalue extraction for natural
frequencies (Natural frequency extraction)
and for eigenvalue buckling estimation (Eigenvalue buckling prediction).
Set this parameter equal to the highest mode number for which output is
required.
The default value is LAST MODE=N, where
N is the number of modes extracted. If the MODE parameter is used, the default value is LAST MODE=M, where
M is the value of the MODE parameter.
- MODE
-
This parameter applies only to
Abaqus/Standard
analyses.
This parameter is useful only during eigenvalue extraction for natural
frequencies (Natural frequency extraction)
and for eigenvalue buckling estimation (Eigenvalue buckling prediction).
Set this parameter equal to the first mode number for which output is required.
The default is MODE=1. When performing a
FREQUENCY analysis, the normalization will follow the format set by
the NORMALIZATION parameter. Otherwise, the normalization is such that the
largest displacement component in the mode has a magnitude of 1.0.
- POSITION
-
This parameter applies only to
Abaqus/Standard
analyses.
Set POSITION=AVERAGED AT NODES if the values being written are the averages of values
extrapolated to the nodes of the elements in the set. Since variables can be
discontinuous between elements with different properties,
Abaqus/Standard
breaks the output into separate tables for different element property
definitions within the element set specified.
Abaqus/Standard
will also output elements of differing types separately. Thus, averaging will
occur only over elements that contribute to a node that have the same type.
Set POSITION=CENTROIDAL if values are being written at the centroid of the element
(the centroid of the reference surface of a shell element, the midpoint between
the end nodes of a beam element).
Set POSITION=INTEGRATION POINTS (default) if values are being written at the integration
points at which the variables are actually calculated.
Set POSITION=NODES if the values being written are extrapolated to the nodes of
each element in the set but not averaged at the nodes.
- REBAR
-
This parameter applies only to
Abaqus/Standard
analyses.
This parameter can be used to obtain output only for the rebar in the
element set specified; output for the matrix material will not be given. It can
be used with or without a value. If it is used without a value, the output will
be given for all rebar in the element set. Its value can be set to the name
assigned to the rebar on the
REBAR option to specify output for that particular rebar in the
element set.
If this parameter is omitted in a model that includes rebar, the output
requests govern the output for the matrix material only (except for section
forces, when the forces in the rebar are included in the force calculation).
Rebar output can be obtained only at the integration points in continuum and
beam elements. In shell and membrane elements rebar output can be obtained at
the integration points and at the centroid of the element.