element integration points, element section points, whole elements,
and element sets;
nodes;
the whole model;
modes in mode-based dynamics procedures;
surfaces in
Abaqus/Standard;
and
sections in
Abaqus/Standard.
All of the output variables are defined in
Abaqus/Standard Output Variable Identifiers
and
Abaqus/Explicit Output Variable Identifiers.
Output quantities from the elements, nodes, and whole model can be written to
the data and results files in
Abaqus/Standard
and to the selected results file in
Abaqus/Explicit.
In
Abaqus/Standard
output quantities from eigenmodes, surfaces, and sections can also be written
to the data and results files.
For
Abaqus
models defined in terms of an assembly of part instances (see
Assembly Definition),
output in the data and results files is given in terms of node, element, set,
and surface labels generated internally by
Abaqus.
See
About Output for
details on how to relate the internally generated numbers and names to those
you specified.
The following sections discuss the input file syntax for requesting output
to the data and results files.
Abaqus/CAE
automatically requests that a data file containing the default printed output
for the current analysis procedure at the end of each step be generated; you
cannot control the contents of the data file from within
Abaqus/CAE.
An analysis from
Abaqus/CAE
does not create a results file.
Output to the Abaqus/Standard Data File
Abaqus/Standard
analysis results can be written to the data (.dat) file.
Element output, nodal output, contact surface output, energy output, modal
output, and section output are available.
Input File Usage
Use any of the following options to request output to the
Abaqus/Standard
data file:
Abaqus/Standard
analysis results can be written to the results (.fil)
file. Element output, nodal output, contact surface output, energy output,
modal output, and section output are available.
Input File Usage
Use any of the following options to request output to the
Abaqus/Standard
results file:
You can write
Abaqus/Explicit
analysis results to the selected results (.sel) file by
specifying a results file output request in conjunction with element output,
nodal output, and/or energy output requests, as explained below. A results file
output request can appear only once per step but remains in effect in
subsequent steps unless it is redefined.
You can control the frequency of all
Abaqus/Explicit
results file output for a particular step by specifying the number of intervals
during the step at which file output will be written,
n. The data are always written at the start and end
of each step in which a results file output request is active. The times at
which the results are written are referred to as time marks.
If the specified number of intervals is 10,
Abaqus/Explicit
will write results 11 times: the values at the beginning of the step and at the
end of 10 equal time intervals throughout the step. The specified number of
intervals must be a positive integer.
By default, results will be written at the increment ending immediately
after each time mark. Alternatively, you can choose to have the time increment
size adjusted so that an increment will end exactly at each of the time marks
calculated by dividing the step into n equal
intervals.
Input File Usage
Use the following option to request results at the
increments ending immediately after each time interval:
Output requests apply to the step in which they are defined and to all
subsequent steps until they are respecified.
One exception occurs when the step type changes from general to linear
perturbation (available only in
Abaqus/Standard).
Output requests defined in general steps apply only to subsequent general
steps; output requests defined in linear perturbation steps apply only to
subsequent consecutive linear perturbation steps. In other words, output
defined in a general step is independent of output defined in a linear
perturbation step. Propagation between linear perturbation steps occurs only
for consecutive linear perturbation steps. If a general analysis step occurs
between perturbation steps, output defined in the first perturbation step will
not propagate to the next perturbation step. In addition, section output
requests are not propagated among linear perturbation steps in
Abaqus/Standard.
Element Output
You can output element variables (stresses, strains, section forces, element
energies, etc.) for a particular step to the
Abaqus/Standard
data (.dat) file, the
Abaqus/Standard
results (.fil) file, or the
Abaqus/Explicit
selected results (.sel) file. The output requests can be
repeated as often as necessary within a step to define output for different
types of element variables, different element sets, etc. The same element (or
element set) can appear in several output requests.
In general, element output requests remain in effect for subsequent steps
unless they are redefined; the appearance of a single element output request in
a step removes all element output requests from a previous step. See
About Output for a
discussion of requesting output in multiple general analysis steps or linear
perturbation steps.
In
Abaqus/Explicit
the element output is written to the selected results
(.sel) file, which must be converted to the results
(.fil) file as explained above.
Input File Usage
Use the following option to output element variables to the
Abaqus/Standard
data file:
The following types of element variables are recognized for the purpose of
defining output:
“Element integration point” variables are associated with the
integration points at which the material calculations are performed (for
example, components of stress and strain). For beams and pipes defined in
Abaqus/Standard
with a general beam section, integration point variables are available only if
the output section points were specified for the section (see
Using a General Beam Section to Define the Section Behavior).
For first-order heat transfer elements the integration points are located at
the corners of the element in heat capacitance calculations.
“Element section point” variables are associated with the cross-section
of a beam, pipe, or a shell (for example, bending moments and membrane forces
on the section).
“Whole element” variables are attributes of an entire element (for
example, the total energy content of the element).
“Whole element set” variables are attributes of an entire element set
(for example, the current coordinates of the center of mass); these variables
are available only in
Abaqus/Standard.
Abaqus/Standard
allows only complete sets of basic variables (for example, all of the stress or
strain components) to be written to the results file. Individual variables
(such as a particular stress component) cannot be selected and must be obtained
by postprocessing.
Abaqus/Standard
element variables can be written to the data and results files at the
integration points, at the centroid, averaged at the nodes, or extrapolated to
the nodes.
In
Abaqus/Explicit
the complete stress or strain tensors can be written to the selected results
file, or individual scalar variables such as equivalent plastic strain can be
written.
Abaqus/Explicit
writes element variables to the results file only at the integration points
where they are calculated.
Selecting the Elements for Which Output Is Required
You can specify the element set for which output is being requested. If you
do not specify an element set, the output will be printed for all elements and,
in
Abaqus/Explicit,
for all rebars in the model. In
Abaqus/Standard
output requests for rebars are governed separately, as discussed below.
Input File Usage
Use either of the following options:
EL PRINT, ELSET=element_set_nameEL FILE, ELSET=element_set_name
Specifying the Section Point in Beams, Pipes, Shells, and Layered Solid Elements
For beams, pipes, shells, or layered solid elements in
Abaqus/Standard output
is provided at the default section points listed in
Abaqus Elements Guide.
You can specify nondefault output points.
In
Abaqus/Explicit
output is always provided at all section points for beam, pipe, and shell
element output requests.
Input File Usage
Use either of the following options in
Abaqus/Standard:
Requesting Output for Rebars in a Reinforced Model
In
Abaqus/Standard you
can request output for rebars (Defining Reinforcement).
If you do not explicitly request rebar output in an
Abaqus/Standard model
with rebars, the element output requests govern the output for the matrix
material only (except for section forces, where the forces in the rebar are
included in the force calculation). You can request output for a particular
rebar. If you do not specify the name of a rebar, output will be given for all
rebars in the specified element set (or in the whole model, if you have not
specified an element set).
In beam and continuum elements in
Abaqus/Standard
rebar output can be obtained at the integration points only. In shell,
membrane, and surface elements rebar output is available at the integration
points and at the element's centroid.
In
Abaqus/Explicit
output for the rebars in the specified element set (or the whole model, if you
have not specified an element set) is always included for element output
requests.
Input File Usage
Use either of the following options in
Abaqus/Standard:
Selecting the Position of Element Integration and Section Point Output in Abaqus/Standard
In
Abaqus/Standard
integration point variables and section variables can be written to the data
and results files in four different positions. By default, output is provided
at the integration points.
Obtaining Element Output at the Integration Points
By default, the variables are output at the integration points where they
are calculated. (You can obtain the position of the integration points by using
output variable COORD—see
Abaqus/Standard Output Variable Identifiers.)
Input File Usage
Use either of the following options:
EL PRINT, POSITION=INTEGRATION POINTSEL FILE, POSITION=INTEGRATION POINTS
Obtaining Element Output at the Centroid of Each Element
You can choose to output the variables at the centroid of each element
(the centroid of the reference surface of a shell element or the midpoint
between the end nodes of a beam or a pipe element). Centroidal values are
obtained by interpolation of the integration point values if the integration
scheme for the element does not include a centroidal integration point.
You can choose to extrapolate the variables to the nodes, then average
them over all of the elements in the set that contribute to each node. For
derived variables, such as the principal stress,
Abaqus/Standard
will first average the extrapolated tensor components over all of the elements
connected to the node to obtain unique components at each node, then calculate
the derived value based on the averaged components.
By default,
Abaqus/Standard
partitions the elements in the model into averaging regions. The partitioning
is based upon the structure of the elements: element type, number of section
points, type of material, single layer or composite, etc. Partitioning is not
based upon the values of element properties (such as thickness), material
orientations, or material constants. Averaging will occur only over elements
that contribute to a node and belong to the same averaging region.
In some situations you may want the averaging regions to take into account
the values of element properties. For example, since variables may be
discontinuous between elements with different material constants, you may not
want elements with different property definitions included in the same
averaging region. In such cases you can force
Abaqus/Standard
to take into account values of element properties by setting the
Abaqus
environment parameter average_by_section to
ON. However, in problems with many section
and/or material definitions the default value of
OFF will, in general, give much better
performance than the nondefault value of ON.
Input File Usage
Use either of the following options:
EL PRINT, POSITION=AVERAGED AT NODESEL FILE, POSITION=AVERAGED AT NODES
Obtaining Element Output Extrapolated to the Nodes
You can choose to extrapolate the element integration point variables to
the nodes of each element independently, without averaging the results from
adjoining elements.
Extrapolation and Interpolation of Element Output Variables
The shape functions of the element are used for purposes of extrapolation
and interpolation of output variables. Extrapolated values are generally not as
accurate as the values calculated at the integration points in the areas of
high stress gradients, particularly in the case of modified triangles and
tetrahedra. Therefore, adequately detailed meshing is necessary around nodes
where accurate nodal values of such element results are needed. If a
cylindrical or spherical coordinate system is defined for the element (see
Orientations),
the orientation at each integration point may be different. When the values at
the integration points are extrapolated to the nodes, the difference in the
orientation is not taken into account; therefore, if the orientation varies
significantly over the elements connected to a node, the extrapolated values
will not be very accurate. If the material orientation undergoes significant
spatial variation in a region of the model where the material behavior is truly
anisotropic, a finer mesh is required to obtain accurate results even at the
integration points. In that situation once the overall solution has converged
with respect to the mesh density, the interpolation or extrapolation away from
the integration points can also be assumed to be reasonably accurate. Element
output for second-order elements with one collapsed side in two dimensions or
one collapsed face in three dimensions should not be extrapolated to the nodes.
In a coupled temperature-displacement and a coupled
thermal-electrical-structural analysis nodal temperatures (variable NT11) are more accurate than temperatures at the integration point
(variable TEMP) extrapolated to the nodes.
For derived variables, such as the Mises equivalent stress, the components
are first extrapolated or interpolated, then the derived value is calculated
from the extrapolated or interpolated components. However, in linear mode-based
dynamic analysis procedures where values are obtained as nonlinear combinations
of modal response magnitudes (Random Response Analysis
and
Response Spectrum Analysis),
the nonlinear combinations are first calculated at the integration points.
These derived values are extrapolated to the nodes or interpolated to the
centroid.
Requesting Summaries in the Abaqus/Standard Data File
By default in
Abaqus/Standard,
summaries of element variables are printed in the data file. A summary of the
maximum and minimum values is printed at the end of each column in an output
table. The locations of the maximum and minimum values are also printed. You
can choose to suppress this summary.
Requesting Totals in the Abaqus/Standard Data File
In
Abaqus/Standard
you can print the sum (total) of each column in an output table to the data
file. Totals can be used, for example, to obtain a sum of all the energies in a
set of elements. By default, these totals are suppressed.
In
Abaqus/Standard
you can control the frequency of element output by specifying the output
frequency in increments. Unless a frequency of zero is specified to suppress
output, the variables will always be output at the last increment of the step.
In
Abaqus/Explicit
the frequency of element output is controlled as described in
Output Frequency
above.
Input File Usage
Use either of the following options in
Abaqus/Standard:
For components of stress, strain, and similar material variables, 1, 2, and
3 refer to the directions in an orthogonal coordinate system. If a local
orientation is not defined for the element, the stress/strain components are in
the default directions defined by the convention given in
Conventions:
global directions for solid elements; surface directions for shell, membrane,
and gasket elements; and axial and transverse directions for beam and pipe
elements.
If a local orientation is associated with the element, the element output
variable components are in the local directions defined by the orientation (see
Orientations).
In
Abaqus/Standard
you can request that the local directions be written to the results file if
component output is requested for any variable (see
Output of Local Directions to the Results File
below). In
Abaqus/Explicit
the local directions will always be written to the results file when tensor
output is requested for any element variable. The local directions are written
automatically to the output database file from both
Abaqus/Standard
and
Abaqus/Explicit.
In large-displacement problems the local directions defined in the reference
configuration are rotated into the current configuration by the average
material rotation. See
State storage
for details.
Controlling the Output during Eigenvalue Extraction
You can control element output during natural frequency extraction (Natural Frequency Extraction),
complex eigenvalue extraction (Complex Eigenvalue Extraction),
and eigenvalue buckling analysis (Eigenvalue Buckling Prediction)
by specifying the first and last mode numbers for which output is required. By
default, the first mode number is 1 and the last mode number is
N, where N is the number
of modes extracted. If you specify the first mode number, the default value for
the last mode number is M, where
M is the value specified for the first mode number.
In
Abaqus/Standard
the printed output of variables is arranged in tables in the data file. For
element variables, each row of a table corresponds to a particular location: an
element, a node, a section point within an element, or an integration point.
The rows that will appear in a particular table are defined by choosing an
element set and, possibly, locations within each element in the set.
Each table is defined by a data line of the element output request, which
specifies the variables to appear in that table. There is no limit to the
number of tables that can be defined. The first columns of a table define the
location—the element or node number, integration point number, etc. You choose
which data will appear in the remaining columns; up to 9 variables (columns)
can appear in a table. For example, output variables S and E cannot be requested on the same data line in a
three-dimensional analysis because that would produce 12 columns of output. If
all of the entries in a row are zero, the row is not printed.
Each table can contain only one type of output variable (whole element,
section, or integration point); one type of element; and only one type of
section definition. If an element output request to the data file includes more
than one type of output variable, element, or section definition,
Abaqus/Standard
will split the output automatically into the necessary number of individual
tables. All of the tables defined by the first data line of the output request
will be printed, then all of the tables defined by the second data line, etc.
Results File Format
An element header record (the type 1 record described in
Results File)
is created for each line of requests for each integration point and section
point in an element. In addition to the element header record, a direction
record (record type 85) can be written in
Abaqus/Standard
when complete stress or strain tensor output is requested (see below). In
Abaqus/Explicit
a direction record is always written when complete stress or strain tensor
output is requested.
For
Abaqus/Standard
file output requests with multiple variables, it is advantageous to specify as
many variables as possible on each data line of the element output request (up
to 16). By keeping the number of lines of requests to a minimum, extra type 1
and type 85 records are avoided and the size of the results file may be reduced
substantially. This is not an issue in
Abaqus/Explicit.
Element variables must be of the same “type” (element integration point
variable; element section variable; whole element variable; etc.) to be entered
on a single line—see
About Output. In
Abaqus/Standard
if all results in a file output record are zero, the record is not written to
the results file.
Output of Local Directions to the Results File
By default, in
Abaqus/Standard
the local coordinate directions are not written to the results file. If
component output is requested, you can write the local coordinate directions to
the results file. A direction record of type 85 will be written following the
type 1 record.
In
Abaqus/Explicit
the local coordinate directions are always written to the selected results file
as a direction record of type 85 when complete stress or strain tensor output
is requested.
Tensor component output is given in the local coordinate system, which may
be inherent to the element (as is the case in shells and membranes) or
user-defined (Orientations).
For shell elements a direction record is written for every material point
in the section for which component output is requested, and a separate
direction record is written for section forces and section strains. For
geometrically nonlinear analysis in
Abaqus/Standard
the record contains the current, updated directions, except for small-strain
shells and gasket elements, for which the original directions are given. For
three-dimensional beams, direction output is written only if section output has
been requested.
Direction output is not provided for trusses, two-dimensional beams,
two-dimensional gasket elements, axisymmetric shells, axisymmetric membranes,
axisymmetric gasket elements, or for values averaged at nodes. In addition, it
is not provided for GKxxN-type gasket elements, which have no membrane or transverse shear
deformation.
If you do not specify an element output request to the results file in a
step (or in any previous step of the analysis), no element output will be
written to the results file; similarly, if you do not specify an element output
request to the data file (available only in
Abaqus/Standard)
in a step (or in any previous step of the analysis), no element output will be
written to the data file.
Node Output
You can output nodal variables (displacements, reaction forces, etc.) for a
particular step to the
Abaqus/Standard
data (.dat) file, the
Abaqus/Standard
results (.fil) file, or the
Abaqus/Explicit
selected results (.sel) file. The output requests can be
repeated as often as necessary within a step to define output for different
node sets. The same node (or node set) can appear in several output requests.
In general, nodal output requests remain in effect for subsequent steps
unless they are redefined; the appearance of a single nodal output request in a
step removes all nodal output requests from a previous step. See
About Output for a
discussion of requesting output in multiple general analysis steps or linear
perturbation steps.
In
Abaqus/Explicit
the nodal output is written to the selected results (.sel)
file, which must be converted to the results (.fil) file
as explained above.
Input File Usage
Use the following option to output nodal variables to the
Abaqus/Standard
data file:
Abaqus
allows only complete sets of basic variables (for example, all of the
displacement components) to be written to the results file. Individual
variables (such as a particular displacement component) cannot be selected and
must be obtained by postprocessing.
Selecting the Nodes for Which Output Is Required
You can specify the node set for which output is being requested. If you do
not specify a node set, the output will be printed for all nodes in the model.
Requesting Summaries in the Abaqus/Standard Data File
By default in
Abaqus/Standard,
summaries of nodal variables are printed in the data file. A summary of the
maximum and minimum values is printed at the end of each column in an output
table. The locations of the maximum and minimum values are also printed. You
can choose to suppress this summary.
Requesting Totals in the Abaqus/Standard Data File
In
Abaqus/Standard
you can print the sum (total) of each column in an output table to the data
file. Totals can be used, for example, to sum reaction forces at the nodes. By
default, these totals are suppressed.
In
Abaqus/Standard
you can control the frequency of nodal output by specifying the output
frequency in increments. Unless a frequency of zero is specified to suppress
output, the variables will always be output at the last increment of the step.
In
Abaqus/Explicit
the frequency of nodal output is controlled as described in
Output Frequency
above.
Input File Usage
Use either of the following options in
Abaqus/Standard:
For nodal variables 1, 2, and 3 refer to the global directions
X, Y, and
Z, respectively. For axisymmetric elements 1 and 2
refer to the global directions r and
z.
In
Abaqus/Standard
components of nodal variables such as reaction forces are output in the global
directions unless a local coordinate system has been defined at a node (see
Transformed Coordinate Systems).
In this case you can specify whether output is desired in global or local
directions. The local directions defined by the nodal transformation cannot be
written to the results file.
The data in the
Abaqus/Explicit
selected results file are always output in the global directions, even if a
local coordinate system has been defined at a node.
Obtaining Nodal Output in the Global Directions
In
Abaqus/Standard
you can request vector-valued nodal variables in the global directions, which
is the default for nodal output requests to the results file since most
postprocessors assume that components are given in the global system.
Obtaining Nodal Output in the Local Directions Defined by Nodal Transformations
In
Abaqus/Standard
you can request vector-valued nodal variables in the local directions defined
by nodal transformations, which is the default for nodal output requests to the
data file.
Controlling the Output during Eigenvalue Extraction
You can control nodal output during natural frequency extraction, complex
eigenvalue extraction, and eigenvalue buckling analysis by specifying the first
and last mode numbers for which output is required, as described above for
element output.
In
Abaqus/Standard
the printed output of variables is arranged in tables by node set in the data
file. For nodal variables each row of a table corresponds to an individual
node.
Each table is defined by a data line of the nodal output request, which
specifies the variables to appear in that table. There is no limit to the
number of tables that can be defined. The first column of each table is the
node number. You choose the variables to appear in the remaining columns; up to
nine variables (columns) can appear in a table. If all of the entries in a row
are zero, the row is not printed. Displacement, velocity, and acceleration
components less than a relative tolerance (equal to 100 times the machine
precision times the current maximum value in the model) are treated as zero.
Results File Format
There is no header or direction record for nodes, so it makes little
difference whether items are requested on a single line or multiple lines. In
Abaqus/Standard
if all results in a record are zero, the record is not written to the results
file.
Default Nodal Output
If you do not specify a nodal output request to the results file in a step
(or in any previous step of the analysis), no nodal output will be written to
the results file; similarly if you do not specify a nodal output request to the
data file (available only in
Abaqus/Standard)
in a step (or in any previous step of the analysis), no nodal output will be
written to the data file.
Total Energy Output
You can output summaries of the energy content of the model to the
Abaqus/Standard
data (.dat) file, the
Abaqus/Standard
results (.fil) file, or the
Abaqus/Explicit
selected results (.sel) file. Energy output requests are
not available for the following procedures:
Energy output requests remain in effect for subsequent steps. Detailed
energy density output is available by using element output requests (see
Element Output).
In
Abaqus/Explicit
the energy output is written to the selected results
(.sel) file, which must be converted to the results
(.fil) file as explained above.
Input File Usage
Use the following option to output summaries of the energy
content to the
Abaqus/Standard
data file:
External Work Calculation due to Concentrated Follower Forces
Abaqus/Standard
may generate inaccurate external work (ALLWK) in the presence of a concentrated follower load that rotates
with time (see
Specifying Concentrated Follower Forces).
This problem may occur in both static and implicit dynamic analyses and may
result in an inaccurate total energy (ETOTAL) history output. Other results (displacements, stresses,
strains, etc.) are not affected. The inaccuracy is due to the fact that the
increment of work is calculated using the direction of the concentrated load at
the end of the increment instead of using an average load over the increment.
Energy Computation Accuracy
Energy terms may not be computed consistently. Some of the energy terms are integrated
using the trapezoidal rule (for example, elastic energy in Abaqus/Standard, which has second-order accuracy for smooth problems). Other terms, such as contact
frictional dissipation, are computed using the backward difference method, which is only
first-order accurate. The total energy balance may not be constant in time due to such
discrepancies, especially in the presence of discontinuities such as contact impact.
Selecting the Element Set for Which Total Energy Output Is Required
In
Abaqus/Standard
you can specify the element set for which total energy output is being
requested. In this case the energies are summed for all the elements in the
specified set. You cannot specify an element set for the following procedures:
If you do not specify an element set, the total energies for the whole model
will be output. If total energy output for both the whole model and for
different element sets is desired, the energy output requests must be repeated;
once without a specified element set to request energy output for the whole
model and once for each specified element set.
In
Abaqus/Explicit
you cannot specify selected element sets for an energy output request; the
total energies for the whole model will always be output.
Input File Usage
Use one of the following options in
Abaqus/Standard:
In
Abaqus/Standard
you can control the frequency of energy output by specifying the output
frequency in increments. Unless a frequency of zero is specified to suppress
output, the variables will always be output at the last increment of the step.
In
Abaqus/Explicit
the frequency of energy output is controlled as described in
Output Frequency
above.
Input File Usage
Use either of the following options in
Abaqus/Standard:
Energy output requests must be included for total energy output to be
written to the data and results files; no default output is provided.
Modal Output from Abaqus/Standard
You can output generalized coordinate (modal amplitude and phase) values
during modal dynamic procedures (see
About Dynamic Analysis Procedures
for an overview of the modal dynamic procedures available in
Abaqus/Standard)
to the data (.dat) file or results
(.fil) file.
You can also request that eigenvalues be written to the results file during
Eigenvalue Buckling Prediction
or
Natural Frequency Extraction.
The eigenvalues are always written to the results file when element or nodal
output to the results file is requested; however, modal output requests allow
you to write the eigenvalues to the results file without requesting any
additional output.
Input File Usage
Use the following option to output modal variables to the
Abaqus/Standard
data file:
You can control the frequency of modal output by specifying the output
frequency in increments. Unless a frequency of zero is specified to suppress
output, the variables will always be output at the last increment of the step.
Modal output requests must be included for modal results to be written to
the data and results files; no default output is provided.
Surface Output from Abaqus/Standard
In
Abaqus/Standard
you can write variables associated with surfaces in contact, coupled
temperature-displacement, coupled thermal-electrical-structural, coupled
thermal-electrical, and crack propagation problems to the data and results
files. The output requests can be repeated as often as necessary within a step
to define output for different contact pairs and different types of surface
variables.
Use element output requests (see
Element Output)
to obtain data and results file output for contact elements (such as slide line
elements; see
Slide Line Contact Elements).
Selecting the Surface Output Variables
The following types of surface variables are recognized for the purpose of
defining output:
“Secondary node” variables are associated with the integration points at which the material
calculations are performed (for example, the contact stress).
“Whole surface” variables are attributes of an entire secondary surface (for example, the total
force due to contact pressure).
Selecting the Contact Pairs for Which Output Is Required
You can select the main and secondary surfaces for which output is required, and you can specify
a subset of secondary nodes for output in addition to the main and secondary surfaces or
independently. If no surfaces or secondary nodes are specified, surface variables are
written for all the contact pairs in the model. If you specify the secondary surface but
not the main surface, output is given for all contact pairs that involve the specified
secondary surface.
By default, summaries of surface variables are printed in the data file. A
summary of the maximum and minimum values is printed at the end of each column
in an output table. The locations of the maximum and minimum values are also
printed. You can choose to suppress this summary.
You can control the frequency of surface output by specifying the output
frequency in increments. Unless a frequency of zero is specified to suppress
output, the variables will always be output at the last increment of the step.
Surface output requests must be included for surface variables associated
with contact pairs to be written to the data and results files; no default
output is provided.
If a surface output request is defined without any specified output
variables, the following variables will be written to the data and results
files by default:
For contact analysis, contact pressure (CPRESS), frictional shear stresses (CSHEAR), contact opening (COPEN), and relative tangential motions (CSLIP); see
About Contact Pairs in Abaqus/Standard.
For heat transfer analysis, heat flux per unit area (HFL), heat flux (HFLA), time integrated HFL (HTL), and time integrated HFLA (HTLA); see
Thermal Contact Properties.
For coupled thermal-electrical analysis, HFL, HFLA, HTL, HTLA, electrical current per unit area (ECD), electrical current (ECDA), time integrated ECD (ECDT), and time integrated ECDA (ECDTA); see
Electrical Contact Properties.
For coupled pore fluid-mechanical analysis, CPRESS, CSHEAR, COPEN, CSLIP, pore fluid volume flux per unit area (PFL), pore fluid volume flux (PFLA), time integrated PFL (PTL), and time integrated PFLA (PTLA); see
Pore Fluid Contact Properties.
For crack propagation analysis, there are no default output quantities;
bond failure quantities must be requested explicitly; see
Crack Propagation Analysis.
Data File Format
Printed output of variables is arranged in tables. Each table is defined by a data line of the
surface output request, which specifies the variables to appear in that table. Each table
can contain only one type of output variable (secondary node or whole surface). For
example, output variables CSTRESS and
CFN cannot be requested on the same data
line. For the secondary node type of output, each row of a table corresponds to a node on
the secondary surface. The rows that will appear in a particular table will be limited to
the node set specified in the output request. The first column of each table defines the
location (the node number). The remaining columns contain variables such as contact
pressure, frictional shear stresses, contact opening, and relative tangential (slip)
motions. For the whole surface type of output, each row of a table corresponds to an
entire secondary surface. If all of the variables in a row of a table are zero, the row is
not printed.
If a contact output request refers to more than one contact pair, a separate
table will be generated for each contact pair. All of the tables defined by the
first data line of the output request will be printed, then all of the tables
defined by the second line, etc.
Results File Format
A contact output request record (the type 1503 record described in Results File) is created for each output request. For the secondary
node type of output, this record is followed by several node header records, each of which
contains a node on the secondary surface. Each node header record is followed by records
that contain output variables. The output will be limited to the node set specified in the
output request. For the whole surface type of output, the type 1503 record is followed by
only one type 1504 node header record with a node number zero. The node header record is
followed by records containing the requested output variables.
If a contact output request refers to more than one contact pair, a separate
contact output request record is generated for each contact pair.
Section Output from Abaqus/Standard
In
Abaqus/Standard
you can output accumulated quantities associated with user-defined sections
(see
Abaqus/Standard Output Variable Identifiers)
for a particular step to the data or results file. This facility provides “free
body diagram” output, allowing analyses of force flow through a redundant
structure. The output requests can be repeated as often as necessary within a
step to define output for different sections and different section output
variables. You can assign a label to each output request that will be used to
identify the output for the section. Section output is not available for
eigenfrequency extraction, eigenvalue buckling prediction, complex
eigenfrequency extraction, or linear dynamics procedures or in procedures using
multiple load cases.
Defining the Surface Section
Section output requests are available only for sections defined using
element-based surfaces (see
Element-Based Surface Definition).
Consequently, the sections must be defined using faces of continuum elements
although other types of elements (beams, membranes, shells, springs, dashpots,
etc.) can be attached to the section.
Calculation of accumulated quantities on the section (such as the total
force) involves nodal quantities associated with elements on one side of the
section only. Therefore, the surface definition should use elements only from
one side of the section (the “base elements,” as defined in
Prescribed Assembly Loads),
thus precisely identifying the side from which accumulated quantities are
computed.
Since the section usually cuts through the mesh in a typical section output
request, automatic generation of the surface cannot be used. Specifying the
element faces gives exact control over which element faces form the surface,
which is essential when defining a cross-section through a solid body.
You must specify the name of the surface for which output is being
requested.
Surfaces that are defined in a restart analysis can be used only for section
output requests. The newly defined surface cannot be used for any other purpose
(such as a contact pair or pre-tension section definition).
For example, the following input illustrates a typical section output
request to the data file:
HEADING
Section print example
…
SURFACE, NAME=surface_nameData lines that specify the elements and their associated faces to define the
surface section
…
STEP
…
SECTION PRINT, NAME=section_name,
SURFACE=surface_name, …
…
END STEP
Alternatively, if additional section output requests are needed after the
analysis is completed, a restart analysis can be performed to request more
output as shown in the following input:
RESTART, READ, …
…
SURFACE, NAME=surface_nameData lines that specify the elements and their associated faces to define the
surface section
…
STEP
…
SECTION PRINT, NAME=section_name,
SURFACE=surface_name, …
…
END STEP
Selecting the Coordinate System in Which Output Is Desired
You can specify the choice of coordinate system in which the section output
is desired. By default, the components of vector quantities associated with the
section are obtained with respect to the global system of coordinates.
Alternatively, you can specify that output is desired in a local system as
defined below.
Input File Usage
Use either of the following options:
SECTION PRINT, NAME=section_name, SURFACE=surface_name,
AXES=GLOBAL or LOCALSECTION FILE, NAME=section_name, SURFACE=surface_name,
AXES=GLOBAL or LOCAL
Defining a Coordinate System Local to the Surface Section
You can allow
Abaqus/Standard
to define the local system, or you can specify it directly.
Default Local System
The default local system is particularly useful when the section is flat
or almost flat. While it can also be used in the case when the defined surface
is curved, the default local system may be irrelevant for such problems.
The default system is defined by a straight line in two-dimensional and
axisymmetric cases or by a plane in three-dimensional cases, fitted (in a least
square sense) through the nodes belonging to the section. The anchor point
(origin) of the local system is the centroid of the projection of the surface
on the fitted line or plane. The local directions are given by the normal
(1-direction) and the tangent direction (the 2-direction in two-dimensional and
axisymmetric cases) or the tangent directions (the 2- and 3-directions in
three-dimensional cases) to the fitted line or plane. When several straight
lines or planes can be fit equally well between the nodes defining the section
(for example, a closed circular or spherical surface), the original local
directions will be parallel to the global axes.
The positive local 1-direction is selected such that it will form an acute
angle with the average normal direction to the section, computed by averaging
the positive normals to the element faces defining the section. If the average
normal direction is zero (a closed surface), the 1-direction will form an acute
angle with the global x-axis. If in two-dimensional or
axisymmetric cases the 1-direction is within 0.1° of being normal to the global
x-axis, it will form an acute angle with the global
y-axis. In three-dimensional cases if the 1-direction is
within 0.1° of being normal to the global
X–Y plane, it will form an acute
angle with the global z-axis.
In two-dimensional and axisymmetric cases the local 2-direction is
obtained by rotating the local 1-direction counterclockwise by 90° about the
anchor point. For three-dimensional situations the tangent directions of the
surface are defined using the
Abaqus
conventions for local directions on surfaces in space (see
Conventions).
Input File Usage
Use either of the following options to use the default local
coordinate system:
A user-specified local system is defined by specifying the origin and the
directions of the axes. You can specify the origin (anchor point) by giving a
node number or by specifying the coordinates of the anchor point.
In two-dimensional and axisymmetric cases the local 2-direction is defined
by specifying either a predefined node number or the coordinates of a point
(point a) on the local 2-direction. The local 1-direction
is then obtained by rotating the local 2-axis clockwise by 90° about the anchor
point (see
Figure 1).
If node numbers are used to define the anchor point or the local directions,
they must be connected to the mesh.
Figure 1. User-defined local coordinate system.
In three-dimensional cases either two predefined nodes or the coordinates
of two points can be used to specify the local directions. A rectangular
Cartesian coordinate system is then defined by its origin (the anchor point)
and these two points. The first point (point a) must lie
on the local 2-direction, and the second (point b) must be
in the local 2–3 plane on the side of the local 3-direction. Although it is not
necessary, it is intuitive to select the second point such that it is on or
near the local 3-direction (see
Figure 1).
If you do not specify the anchor point of the local system, it is taken to
be the centroid of the projection of the surface on the fitted line or plane.
If you do not specify the directions of the axes, the local system will be
anchored at the specified anchor point and its axes will be parallel to the
default axes of the projected surface. If neither the anchor point nor the
directions are defined, the default local system will be used.
In large-deformation analyses the surface section may rotate significantly
during the deformation. By default, when output is requested in a local
coordinate system, the system rotates with the average rigid body motion of the
elements used to define the surface section (i.e., the local system and the
output are updated during the analysis). The anchor point and local directions
must then be specified relative to the undeformed configuration. You can choose
to obtain vector output in the original local coordinate system instead. This
choice is irrelevant in steps in which geometric nonlinearities are not
considered.
Input File Usage
Use either of the following options to specify the local
coordinate system directly:
SECTION PRINT, NAME=section_name, SURFACE=surface_name,
AXES=LOCAL, UPDATE=YES or NOanchor point definitionaxes definitionSECTION FILE, NAME=section_name, SURFACE=surface_name,
AXES=LOCAL, UPDATE=YES or NOanchor point definitionaxes definition
Controlling the Frequency of Output
You can control the frequency of section output by specifying the output
frequency in increments. Unless a frequency of zero is specified to suppress
output, the variables will always be output at the last increment of the step.
Printed output is arranged in tables. The first line of the table contains
the name of the requested output variable (see
Abaqus/Standard Output Variable Identifiers),
and the second line contains the corresponding value. If a section output
request is defined without any specified output variables, all appropriate
variables associated with the current analysis type are output.
If several section output requests to the data file are encountered in one
particular step, separate tables will be created for each request. Each table
has a header denoting the name of the section and the name of the surface used.
In addition, if the output is requested in a local coordinate system, the
global coordinates of the anchor point and the cosine directions of the local
axes are output.
Results File Format
Several section output records (record numbers 1580–1591 in
Results File)
are output for each section output request to the results file. The actual
collection of records to be written to the results file depends on the number
of valid output requests. If a section output request is defined without any
specified output variables, all records relevant to the current analysis type
are stored in the results file.
Vector Output in the Section
Vector output associated with section output requests consists of the total
force (SOF), the total moment (SOM), and the center of forces (SOCF). Output variable SOF is computed as a vector sum of the stress-based (internal)
nodal forces of the nodes in the surface.
Output variable SOM is computed with respect to the origin of the coordinate system
considered. Thus, if the output is requested in the global coordinate system,
the total moment is computed about the global origin; if the output is
requested in a local coordinate system, the moment is computed about the
current anchor point of the local system. The coordinates of the current anchor
point may change during the analysis if the local coordinate system is updated.
Output variables SOF and SOM are both reported in the coordinate system considered.
The center of forces SOCF is computed as the closest point to the centroid of the section
through which the total force SOF acts. SOCF is always reported in the global coordinate system. If the
total force vector is equal to zero, the centroid of the section is reported as
the center of forces SOCF.
The total moment vector, SOM, will not necessarily equal the cross product of the center of
force vector, SOCF, and total force vector, SOF. Forces acting on two different points of the section may have
components acting in opposite directions, such that these force components
generate a net moment but not a net force; therefore, the total moment may not
arise entirely from the resultant force.
Scalar Output in the Section
Scalar output associated with a section output request consists of the area
of the defined section (SOAREA), the total heat flux (SOH) in heat transfer analysis, the total current (SOE) in electrical analysis, the total mass flow (SOD) in mass diffusion analysis, and the total pore fluid volume
flux (SOP) in couple pore fluid diffusion-stress analysis. These output
variables are computed as the algebraic sum of the scalar internal nodal fluxes
(work-conjugate to the associated primary solution variables) of the nodes in
the surface. For example, in heat transfer analysis the total heat flux (SOH) is the sum of the NFLUX values at the nodes on the surfaces.
Limitations When Using Section Output Requests
Section output requests are subject to the following limitations:
Section output requests are available only for sections defined by an
element-based surface. Thus, they can be used only for sections along faces of
continuum elements.
When defining the section, elements on only one side of the section must
be used.
Abaqus/Standard
identifies all elements attached to the surface on this side and computes the
section output variables as in a free-body diagram.
The defined section must cut completely through the mesh, form a closed
surface, or be on the exterior of the body.
Figure 2
presents some typical cases of valid surfaces. If the section cuts only
partially through the mesh, a valid free-body diagram cannot be isolated (see
Figure 3)
and incorrect answers may be computed.
Abaqus/Standard
will attempt to identify the invalid cases and will issue error or warning
messages.
Elements attached to the section can be on either side of the surface
but must not cross the defined section.
Figure 3
presents a few invalid cases. In most cases
Abaqus/Standard
will successfully identify elements that cross the surface, and warning
messages will be issued. The elements will then not be considered in the
calculation of the section variables.
For section output purposes,
Abaqus/Standard
will ignore the elements attached to the section for which it cannot establish
whether they belong to one side or the other of the section (e.g., SPRING1 elements).
Section output requests cannot be specified within a substructure.
Section output requests cannot be specified in random response analyses.
The total force and the total moment in the section are computed based
only on the stresses (internal forces) in the identified elements. Thus,
inaccurate results may be obtained if distributed body loads are present in
these elements since their effect on the total force in the section is not
included. Common examples are the inertial loading in dynamic analyses, gravity
loads, distributed body forces, and centrifugal loads. In these cases the total
force in the section may depend on the choice of elements used to define the
section as illustrated in
Figure 4(a).
Assuming that gravity loading is the only active load, the element stresses
will be different in the two elements. Hence, if the same section is defined
first using element 1 and then using element 2, different answers for the total
force will be obtained. In a similar way the effects of any distributed body
fluxes (heat, electrical, etc.) prescribed in the identified elements are not
included.
Figure 4. Total force in the section.
Depending on which side of the surface is used to define the section,
different answers will be obtained in analyses similar to the case illustrated
in
Figure 4(b).
Assuming a static analysis with the concentrated loads shown in the figure
being the only active loads, a zero total force is reported if the section is
defined using element 1 and a nonzero force equal to the sum of the
concentrated loads is obtained if the section is defined using element 2.
