Abaqus
can create the following output files during an analysis:
a data file containing printed output of the model and history
definition generated by the
analysis input file processor
and, in
Abaqus/Standard,
printed output of results written during the analysis run;
an ODB output database file
containing results for postprocessing
and, in
Abaqus/Standard,
diagnostic information;
a SIM database file containing results for high-performance
postprocessing with the Physics Results Explorerapp
on the 3DEXPERIENCE platform;
a selected results file in
Abaqus/Explicit;
a results file containing results for postprocessing with external
software in
Abaqus/Standard
and
Abaqus/Explicit
(in
Abaqus/Explicit
this file is generated by converting the selected results file);
a message file containing diagnostic messages about the solution in
Abaqus/Standard
and
Abaqus/Explicit;
and
a status file containing information about the status of the analysis
and, in
Abaqus/Explicit,
diagnostic messages and information about the stable time increment.
Abaqus
can create files for restarting an analysis—see
Restarting an Analysis.
In
Abaqus/Standard
these files can also be used to extract results output not requested during an
analysis.
The data file (job-name.dat)
is a text file that contains information about the model definition (generated
by the
analysis input file processor)
and, in
Abaqus/Standard,
tabular output of results. The
analysis input file processor
information includes the model definition, the history definition, and messages
identifying any error and warning conditions that were detected while
processing the input data.
Controlling the Amount of analysis input file processor Information Written to the Data File
You can control the amount of information written to the data file by the
analysis input file processor
in
Abaqus/Standard
and
Abaqus/Explicit.
Input File Echo
By default, the input file will not be echoed to the data file. You can
choose to activate this printout. If the input file is defined in terms of an
assembly of part instances, the echo to the data file will be that of the
flattened input file (i.e., one that does not use parts and assemblies).
Input Parameter Information
For parametrized input files, information about input parameters and their
values can be printed in the data file. By default, the modified version of the
original input file showing this information will not be printed in the data
file. You can choose to activate this printout.
Parameter-Free Input File Information
For parametrized input files, a parameter-free version (after parameter
evaluation and substitution) of the original input file can be printed in the
data file. By default, this modified version of the input file will not be
printed in the data file. You can choose to activate this printout.
Model and History Definition Summaries
By default, the options defining the model and history data will not be
summarized in the data file. You can choose to activate this printout.
For an
Abaqus/Explicit
analysis the model summary data, when requested, includes the mass, center of
mass, and the rotary inertia information for the element sets in the model and
for the whole model. However, for two-dimensional models the reported rotary
inertia includes the
component corresponding to the only active rotation degree of freedom; the
remaining components are not included.
Contact Constraint Information
In
Abaqus/Standard
you can choose to activate printout of detailed information about the contact
constraints generated by the contact pair definition data.
Mass Information
In
Abaqus/Explicit
you can choose to activate printout of detailed information about the mass
property of each user-defined element set.
Requesting Printed Results
In
Abaqus/Standard
the values of output variables can be printed to the data file in tabular
format throughout the analysis. You can control the following types of printed
output during the analysis run: element output, node output, contact surface
output, energy output, fastener interaction output, modal output, section
output, and radiation output—see
Output to the Data and Results Files
and
Cavity Radiation in Abaqus/Standard.
You specify the variables to be printed in each output table and, for element
variables, the locations at which they are to be printed (at the integration
points, at the element centroid, at the nodes, or averaged at the nodes). Nodal
variables at nodes with transformations can be written in either the global or
the local coordinate system (see
Transformed Coordinate Systems).
The list of available variables is given in
Abaqus/Standard Output Variable Identifiers.
Output of results to the data file is requested as part of a step definition.
Viewing Part and Assembly Information in the Data File
An
Abaqus
model can be defined in terms of an assembly of part instances (see
Assembly Definition).
In such a model node and element numbers can be repeated within the definitions
of different parts. These local numbers are converted internally by
Abaqus
to unique global numbers, and the output written to the data file is given in
terms of those internal numbers. A map between user-defined numbers and
internal numbers is printed to the data file (after the step data) if any
output that includes node and element numbers is requested in the data file.
Set and surface names that appear in the data file are prefixed by the
assembly and part instance names, separated by underscores
(Assembly_Part1–1_setname, for example).
Local coordinate systems defined within a part or part instance are
translated and rotated according to the positioning data given in the part
instance definition.
The Output Database
The output database is a neutral binary file. Unlike the restart or binary
results files, it can be copied directly from one computing platform to another
without translation.
Format of the Output Database
The
Abaqus
output database is available in two formats,
ODB and SIM.
By default, the results output is created in
ODB format. For an
Abaqus/Standard
or
Abaqus/Explicit
analysis you have the option to write results in both formats during the same
job. Only results in SIM format can be
imported into the
3DEXPERIENCE platform
for high-performance postprocessing. For more information, see
Limitations When Writing and Postprocessing Results in SIM Format
below.
The ODB output database
(job-name.odb) is used to store
model information and analysis results in terms of an assembly of part
instances.
The SIM database file
(job-name.sim) contains model
and results information. The
Physics Results Explorerapp
on the
3DEXPERIENCE platform
uses this database for high-performance postprocessing of analysis results.
Handling of Floating Point Data
By default, floating point data are written in single precision to the
ODB output database file. You can choose to
write floating point nodal field output data to the
ODB output database file in double precision;
see
Abaqus/Standard and Abaqus/Explicit Execution
for details.
For
Abaqus/Standard
and
Abaqus/Explicit
analyses, floating point data are written to the
SIM database in single precision, with the
exception of nodal coordinates, which are written in double precision.
Choosing an Output Format
Your choice of output format depends on your level of experience with
high-performance visualization, the
Physics Results Explorerapp,
and your postprocessing needs.
If you are still learning to use high-performance visualization and
you want to compare your results with
Abaqus/Viewer,
write results in both formats.
If the model is large and you need the improved performance of the
Physics Results Explorerapp,
as well as the capabilities of
Abaqus/Viewer,
write results in both formats.
If you are confident that the high-performance visualization features
in the
Physics Results Explorerapp
provide all the capabilities you need, write results in
SIM format.
Requesting Output to the Output Database
You choose the variables to be written to the output database from the lists in Abaqus/Standard Output Variable Identifiers and Abaqus/Explicit Output Variable Identifiers. The
following types of output are available: element output, node output, contact surface
output, energy output, integrated output, time incrementation output, fastener interaction
output, modal output, and radiation output. In addition, a subset of the diagnostic
information that is written to the message file in Abaqus/Standard and Abaqus/Explicit (see The Message File in Abaqus/Standard and Abaqus/Explicit) and to the Abaqus/Explicit status file (see The Status File) is
included in the output database. See Output to the Output Database
for a detailed explanation of how to generate output database requests.
Three types of information are stored in the output database: “field” output, “history” output,
and diagnostic information. Field output is intended to be relatively infrequent output
for a large portion of the model. History output is intended to be output for a small portion of the model
requested at a fairly high frequency.
See Output to the Output Database for detailed descriptions of field and history output.
Limitations When Writing and Postprocessing Results in SIM Format
A subset of options in
Abaqus/Standard
and
Abaqus/Explicit
are not supported for analyses that produce results in
SIM format. If you include one or more of
these options or parameters in your analysis and write output in
SIM format or both formats, the analysis will
either terminate with errors or produce limited results.
The following options produce error messages in the data
(.dat) file:
The
Abaqus/Explicit
selected results file
(job-name.sel) stores
user-selected results, which are converted into the results file
(job-name.fil) for
postprocessing by other commercial postprocessing packages.
Element output, node output, and energy output can be requested (see
Output to the Data and Results Files
for details); the variables available for output are listed in
Abaqus/Explicit Output Variable Identifiers.
You can write a user-selected subset of the results for a given node set or
element set at more frequent intervals than the restart intervals. You specify
the output requests within a step definition, which allows you to be selective
about the amount of data written to the selected results file to avoid using
excessive disk storage. For example, when dealing with a very large model, you
may choose to write only the current displacements and the equivalent plastic
strain for the entire model 20 times in the step and to write the acceleration
history at one node 200 times in the step.
The Results File
The
Abaqus
results file in
Abaqus/Standard
and
Abaqus/Explicit
(job-name.fil) can be read by
external postprocessors to produce X–Y plots or
printed tabular output. Most commercial finite element results-display packages
provide translators that use the
Abaqus
results file as their input. The results file can also be used as a convenient
medium for importing analysis results into your own postprocessing program.
Accessing the Results File Information
provides details on how to read this file.
Results file output of temperature from a heat transfer, thermal-electrical,
or thermal-electrical-structural analysis can be used as input to a stress
analysis of the same mesh (see
Sequentially Coupled Thermal-Stress Analysis).
Obtaining Results File Output in Abaqus/Standard
In
Abaqus/Standard
you choose the variables to be written to the results file from the lists in
Abaqus/Standard Output Variable Identifiers
in a manner similar to that for output printed to the data file. You must
specifically request that values be written to the results file or none will be
provided. Element output, node output, contact surface output, energy output,
modal output, and radiation output are available—see
Output to the Data and Results Files
and
Cavity Radiation in Abaqus/Standard
for details.
Obtaining Results at the Beginning of a Step
You can request that the solution state at the beginning of a step (the
zero increment) be written to the
Abaqus/Standard
results file. Zero-increment file output is available only for steps in which
the concept of time governs the incrementation scheme of the selected procedure
and, hence, the following procedures are excluded:
If you request zero-increment results file output, it will be generated
for all valid procedures in a given analysis.
You must request zero-increment results file output to generate a
zero-increment results file in a data check analysis (see
Abaqus/Standard and Abaqus/Explicit Execution).
It is strongly recommended that you request zero-increment results file output
if the results file is used to drive a submodel; see
Node-Based Submodeling
for further discussion.
Obtaining Results File Output in Abaqus/Explicit
The
Abaqus/Explicit
results file is a sequential access file generated from the selected results
file (see
Abaqus/Standard and Abaqus/Explicit Execution).
The results file contains the requested results in the format described in
Results File.
Part and Assembly Information
An
Abaqus
model can be defined in terms of an assembly of part instances (see
Assembly Definition).
However, the results file does not contain part and assembly records.
In a model defined in terms of an assembly of part instances, node and
element numbers can be repeated within the definitions of different parts.
These local numbers are converted internally by
Abaqus
to unique global numbers, and the output written to the results file is given
in terms of the global (internal) numbers. A map between user-defined numbers
and internal numbers is printed to the data file if any results file output
that includes node and element numbers is requested.
Set and surface names that appear in the results file are prefixed by the
assembly and part instance names, separated by underscores
(Assembly_Part1–1_setname, for example).
Local coordinate systems defined within a part or part instance are
translated and rotated according to the positioning data given in the part
instance definition.
Format of the Results File
The
Abaqus
results file in
Abaqus/Standard
or
Abaqus/Explicit
is organized as a sequential file, in binary or in
ASCII format.
ASCII format is necessary if the file is to be
read on a computer system that is different from the one on which the file was
written. ASCII format allows the results file
to be transferred between different computer systems without having to
translate binary data. ASCII format is not
needed if the file will always be used on the same system or on systems that
use the same binary format. If the results file output will always reside on
the same computer, the default binary format is usually the most efficient way
of storing the file. For large problems a file in
ASCII format will be significantly larger than
the same file in binary format.
Controlling the Format of the Results File in Abaqus/Standard
Abaqus/Standard
can write the results file in either binary or
ASCII format. The default format is binary.
The results file output must be written in the same format for the entire
analysis. The format cannot be changed upon restarting the problem.
The format of the
Abaqus/Standard
results file can also be controlled in the
Abaqus/Standard
environment file (see
Environment File Settings).
The format specified in an analysis supersedes the value defined in the
enviroment file.
In addition, the ascfil facility in the
Abaqus
execution procedure (ASCII Translation of Results (.fil) Files)
can be used to convert a binary
Abaqus/Standard
results file (job-name.fil) to
ASCII format
(job-name.fin) after the
analysis completes.
Controlling the Format of the Results File in Abaqus/Explicit
Abaqus/Explicit
always writes the results file output in binary format during file conversion,
but the binary
Abaqus/Explicit
results file can be converted to ASCII format
using the ascfil facility (ASCII Translation of Results (.fil) Files).
ASCII Format
Results File
defines the contents of the records that are written to the results file; these
descriptions also hold if the results file is written in
ASCII format. All the data items in these
files are either integers, floating point numbers, or character strings. When
ASCII format is requested, each data item is
translated into an equivalent character string before it is written to the
file. These strings are written in 80-character logical records in the order
described in the record definitions.
Each 80-character logical record is completely filled before the next one
is started, so that any data item can be split, with some of the characters
that define the item in one logical record and the remainder in the next. Each
data item usually follows immediately behind its predecessor. The exception is
that for results file record key 2001
Abaqus
will fill out the logical record with blank characters, so that the record can
be written immediately to the physical storage medium.
Abaqus
then inserts a logical record consisting of 80 blanks, which allows the
end-of-file to be handled correctly.
The beginning of each “record” is indicated by an asterisk (*). Each
floating point number begins with the character D, followed by the number in
the format E22.15 or D22.15, depending on whether the release of
Abaqus
that wrote the results file used single precision or double precision. Each
character string begins with the character A, followed by eight characters (if
the character string has fewer than eight characters, the right part of the
string is blank; character strings longer than eight characters are written
eight characters at a time). Each integer begins with the character I, followed
by a two digit integer giving the number of decimal digits in the integer,
followed by the integer itself (written as decimal digits).
For example, record key 1900 for an S4R element with element number 5 and nodes 195, 198, 205, and 204
would be written
*I 18I 41900I 15AS4R I 3195I 3198I 3205I 3204
and record key 101 for node 135 and 6 degrees of freedom would be written
Precision of Floating Point Data in the Results File
The precision of floating point data written to the results file depends
on the precision of the executable that generates the data.
Abaqus/Standard
always uses double precision; thus, floating point data are always written to
the
Abaqus/Standard
results file in double precision.
Abaqus/Explicit
can be run in single or double precision on most machines; see
Defining an Analysis
for details on the precision level of the
Abaqus/Explicit
executable. If the double precision executable for
Abaqus/Explicit
is used, floating point data are written to the
Abaqus/Explicit
results file in double precision; likewise, if the single precision executable
for
Abaqus/Explicit
is used, floating point data are written to the
Abaqus/Explicit
results file in single precision.
Maximizing the Efficiency of the Results File
In
Abaqus/Standard
each element output request (a collection of identifying keys entered on a
single line) is preceded by an “element header” record (see
Results File).
Hence, the size of the results file can be minimized by entering all element
output variables of the same “type” (element integration point variable,
element section variable, whole element variable, etc.) on a single line. (See
Output to the Data and Results Files
for an explanation of the output variable types.) Consolidating output variable
entries is encouraged, since it will reduce the size of the results file.
Example
For example, the following output requests can be used to request output
of element variables in the results file in a stress/displacement analysis:
EL FILES, SINV, E, PE, CE, EE, ENER, TEMP, FV, COORDSF, SELOADS, ELEN, EVOLEL FILE, REBARS, SINV, E, PE, CE, EE, RBFOR, RBANGSF, SELOADS, ELEN
(The output requests for rebar quantities need not be the same as the
underlying element output requests.)
The Message File in Abaqus/Standard and Abaqus/Explicit
The message file
(job-name.msg) is a text file
that contains diagnostic messages about the progress of the solution.
The Abaqus/Standard Message File
In
Abaqus/Standard
the message file contains diagnostic or informative messages about the progress
of the solution. If any of these messages describe errors or warnings, the
number of such errors or warnings is also given at the end of the data file.
The message file is written automatically during an
Abaqus/Standard analysis.
The
Abaqus/Standard
message file contains information about the increment number, step time,
fraction of a step completed, equilibrium iterations, severe discontinuity
(contact) iterations, plasticity algorithms, adaptive mesh smoothing, the load
proportionality factor in a Riks analysis, etc.
You can control the amount of information written to the message file for
each step. This feature is sometimes helpful in difficult analyses since it
allows detailed diagnostic information to be written about certain events (such
as contact) during a nonlinear solution; this information can often be useful
in developing a strategy for the solution of highly nonlinear problems.
Controlling the Frequency of Output to the Message File
You can control the frequency at which information is printed to the
message file by specifying the desired output frequency in increments. The
default output frequency is 1 (or 10 in a direct cyclic or a low-cycle fatigue
analysis). The output will always be printed at the last increment of each step
unless you specify a frequency of zero to suppress the output.
Requesting Detailed Contact Printout
You can obtain a detailed printout of contact conditions during iteration.
This information about which points are contacting or separating in interface
and gap problems is useful in tracking the development of the solution in
difficult contact problems. The details are written for every severe
discontinuity iteration. By default, the detailed contact output is suppressed.
Requesting Detailed Model Change Printout
You can obtain a detailed printout of model change operations (removal and
reactivation) at the start of a step. This information includes the new
original coordinates and normals of elements being reactivated strain free in a
large-displacement analysis. By default, the detailed model change output is
suppressed. See
Element and Contact Pair Removal and Reactivation
for details on model change operations.
Requesting Detailed Printout of Problems with the Plasticity Algorithms
You can activate printout of element and integration point numbers for
which the plasticity algorithms have failed to converge during an iteration.
This information is useful for finding the place in the mesh and/or the
plasticity model at which
Abaqus
is encountering material model difficulties. Modeling problems and material
parameter specification problems can be identified using this detailed
printout. By default, this printout is suppressed.
Requesting Output of Equilibrium Residuals
By default, equilibrium residuals during equilibrium iterations are
output. You can choose to suppress this output entirely, but it is not
recommended; without the output of equilibrium residuals, you cannot see the
accuracy of the iteration process.
Requesting Solver Information
By default, information about the number of equations being solved and the
number of floating point operations is output for each iteration. You can
request for this output to be suppressed.
You can activate detailed printout of adaptive mesh smoothing in
Abaqus/Standard.
The output includes information about the magnitude of the maximum displacement
and the node and degree of freedom where the maximum displacement increment
occurs during each mesh sweep. It also provides the node numbers at which
geometric feature changes occur. By default, only a summary is output.
Monitoring a Degree of Freedom in the Message File
You can write the current value of a specified point and degree of freedom
to the message file. This information can be used to monitor the progress of
the solution. The information will also be written in the status file (see
below). You can control the frequency at which the value is printed in the
message file. The default frequency is 1 (or 10 in a direct cyclic analysis).
Degree of freedom monitoring does not apply to eigenvalue buckling
prediction, eigenfrequency extraction, or response spectrum procedures. For
other linear perturbation procedures output for the monitored degree of freedom
is the base state value.
The status file
(job-name.sta) is a text file
that contains information about the progress of an analysis.
The Abaqus/Standard Status File
The
Abaqus/Standard
status file contains a single 80-character record for each increment and is
updated upon completion of each increment of an analysis. This record is
written directly to secondary storage immediately at the completion of the
increment. Therefore, the status file can be examined as the analysis job is
executing, thus providing a monitor of the progress of the analysis. Other than
specifying that a degree-of-freedom variable be monitored in the status file in
Abaqus/Standard
(as described below), the information written to the
Abaqus/Standard
status file cannot be controlled.
The Abaqus/Explicit Status File
In
Abaqus/Explicit
the status file (job-name.sta)
contains, by default, mass and inertial properties for the model, initial
stable time increment information, a synopsis of the progress of the analysis
including total accumulated CPU usage and the
current time increment size, and an estimate of the memory required to process
each step. You can control additional output including the total kinetic
energy, the energy balance, the identifier of the element with the smallest
stable time increment, and the percent change in total mass of the model due to
mass scaling.
The frequency at which summary increments are written to the
Abaqus/Explicit
status file depends on the duration of the analysis in
CPU minutes and the amount of output specified
in the analysis. The following list provides general guidelines for when a
summary increment will be written to the status file.
Summary information will generally be written:
Each time restart information, field output to the output database, or
results file output is written.
Once per increment if the problem requires fewer than 20 increments.
20 times during the step for a short analysis (less than 40
CPU minutes).
Every 2 CPU minutes for an analysis
longer than 40 CPU minutes.
Errors that can be detected only while packaging the data for
Abaqus/Explicit
or during analysis are also written to the status file.
Requesting Kinetic Energy Output
By default, the kinetic energy for the model is written to the status
file. This output is written periodically throughout the step. You can choose
to include or exclude the kinetic energy output for each step.
Requesting Total Energy Output
By default, the energy balance is written periodically throughout the
step. You can choose to include or exclude the energy balance output for each
step.
Requesting Output of the Critical Element
By default, the number of the element with the current minimum stable time
increment is output to the status file. This output is written periodically
throughout the step. You can choose to include or exclude the critical element
output for each step.
Requesting Output of the Change in the Total Mass
You can write the percent change in total mass of the model due to mass
scaling to the status file for each step. This output is written periodically
throughout the step. The percent change in total mass is printed by default
only if mass scaling is present in the model.
Monitoring a Degree of Freedom in the Status File
You can write the current value of a specified point and degree of freedom
to the
Abaqus/Standard
status file. The value of the point and degree of freedom being monitored will
appear in the status file for every increment written during the analysis.
When a degree of freedom is monitored in the
Abaqus/Standard
status file, the same information is written to the message file (see above),
but the specified frequency has no effect on the output to the status file.
Degree of freedom monitoring does not apply to eigenvalue buckling
prediction, eigenfrequency extraction, or response spectrum procedures. For
other linear perturbation procedures output for the monitored degree of freedom
is the base state value.
Requesting Output in Multiple Steps
In general, output requests apply to the step in which they are given and to
all subsequent steps until they are respecified. However, output specifications
for linear perturbation steps (available only in
Abaqus/Standard;
see below and
General and Perturbation Procedures)
are treated independently of output requests for general analysis steps and
apply only to a continuous sequence of linear perturbation steps.
Database output, printed output, and results file output are independent
output modes in
Abaqus;
therefore, changing the specification for one form of output does not affect
the other forms.
General Analysis Steps
The default output requests are used in the first general analysis step of
an analysis unless you redefine them. For subsequent general analysis steps,
the definition of each form of output from the previous general step is
maintained unless you redefine it.
Linear Perturbation Steps
The default output requests are used in the first of any sequence of linear
perturbation steps unless they are redefined in that step. If a subsequent
linear perturbation step is defined without an intermediate general analysis
step, the definition of each mode of output from the previous perturbation step
is maintained unless you redefine it. If an intermediate general step is
defined, the default output requests are again used in the linear perturbation
step unless they are redefined in that step.
Element Matrix Output in Abaqus/Standard
In
Abaqus/Standard
you can write element stiffness matrices and, if available, mass matrices for
each step to a file. For heat transfer elements the operator matrices are
written if stiffness matrix output is requested.
Element matrix output is available only for elements without internal nodes
(unless those nodes have no active degrees of freedom) and with no acoustic or
internal degrees of freedom. Examples of elements for which element matrix
output is prohibited include acoustic, pipe, elbow, frame, gap, and interface
elements as well as axisymmetric elements with Fourier modes. Element matrix
output is not available for elements with coupled fields such as coupled
temperature-displacement elements and pore pressure elements. For incompatible
mode and hybrid elements, stiffness matrix output is prohibited while mass
matrix output is available. A substructure matrix output request is used to
write a substructure's reduced stiffness matrix, mass matrix, and load case
vectors to a file (see
Generating Substructures).
Element matrix output cannot be requested in a mode-based dynamic analysis
(response spectrum, steady-state dynamic, modal dynamic, or random response).
However, it can be requested in the eigenfrequency extraction analysis that
precedes the mode-based dynamic analysis to output the mass and stiffness
matrices.
The element matrices are written without the effects of nodal conditions;
therefore, boundary conditions, concentrated loads, and the effects of
multi-point constraints are not included in this output. The degrees of freedom
are always in the global directions, even if a local coordinate system (Transformed Coordinate Systems)
has been defined at nodes associated with the element.
You must select the element set for which output is requested. For models
defined in terms of an assembly of part instances (Assembly Definition),
element numbers written with element matrix output are internal numbers
generated by
Abaqus/Standard.
A map between internal numbers and the original element numbers and part
instance names is provided in the data file.
Writing the Element Matrices to the Results File
By default, element matrix output records are written to the
Abaqus/Standard
results file. The record formats for the results file are described in
Results File.
The file can be written in binary or ASCII
format based on the file format you specify (see
Controlling the Format of the Results File in Abaqus/Standard
above).
Writing the Element Matrices to a User-Defined File
You can write the element matrices to a user-defined file. The file name
should not include an extension; the extension .mtx will
be added. (See
Input Syntax Rules
for the syntax of user-specified file names.)
The format of the output file is compatible with the linear user element
(see
User-Defined Elements).
Writing the Element Matrices to the Data File
You can write the element matrix records to the
Abaqus/Standard
data file.
Including Distributed Loads
You can choose to write the load vector from distributed loads on the
elements. By default, the load vector is not written.
Controlling the Frequency of Element Matrix Output
You can control the frequency at which element matrix output will be written
by specifying an output frequency in increments. By default, the element
matrices will be output every increment (equivalent to an output frequency of
1). Specify an output frequency of 0 to suppress output of the element
matrices. Unless the output is suppressed, the matrices will always be written
at the last increment of a step.
Writing the Stiffness or Operator Matrix
You can choose to output the stiffness matrix (or operator matrix in heat
transfer elements). By default, the stiffness (operator) matrix is not output.
Writing the Mass Matrix
You can choose to output the mass matrix. By default, element mass matrices
are not output.
User-Defined Output Variables in Abaqus/Standard
In
Abaqus/Standard output
quantities can be defined as functions of any element integration point
variable listed in
Abaqus/Standard Output Variable Identifiers
by using user subroutine
UVARM. Then, output variable UVARMn can be requested for output to the data file, the results file,
or the output database.
User-Defined State Variables in Abaqus/Standard
In
Abaqus/Standard you
can allocate solution-dependent state variables and define them in user
subroutines defining material behavior, as well as user subroutines
FRIC,
UEL, and
UINTER (see
About User Subroutines and Utilities).
Output variable SDVn can be requested for output of these state variables to the
data file, the results file, or the output database. For user-defined elements
output variable SDVn cannot be requested for output to the output database.
Recovering Additional Results Output from Restart Data in Abaqus/Standard
Data needed for restart in
Abaqus/Standard are
contained in several files that are generated when you request that restart
data be written for an analysis: the restart (.res),
analysis database (.mdl and .stt),
part (.prt), and output database
(.odb) files.
Restarting an Analysis
describes the writing of restart data in more detail.
In Abaqus/Standard you can extract output from the restart data and write it to new data
(.dat), results (.fil), and output database
(.odb) files using a postprocessing analysis procedure. If the
original analysis included user subroutines, the postprocessing analysis procedure requires
the specification of the user subroutines. The data, results, and
output database file output requests are defined as described in Output to the Data and Results Files and Output to the Output Database. The output requests should be defined exactly as they would be in an analysis,
except that:
The output frequency specification has no meaning and is, therefore,
ignored (unless you are recovering additional output from a previous direct
cyclic or low-cycle fatigue analysis). Instead, you specify each increment at
which output is to be generated in the postprocessing procedure definition.
No default output is provided to the output database. Furthermore, model
information, such as boundary conditions, is not written to the output
database.
Element set energy information cannot be recovered since it is not
written to the restart file.
Output is not available for procedures that do not support restart; for
example, linear perturbation procedures.
The element sets and node sets that are defined for the analysis can be used
for defining output sets during the postprocessing procedure. Additional sets
can also be defined for the postprocessing procedure. You specify the step
number in the restart file from which output is required. You cannot obtain
results at the beginning of a step (see below).
Recovering Additional Output from a Direct Cyclic Analysis
If you use this postprocessing technique to recover additional output from a
previous direct cyclic analysis (see
Direct Cyclic Analysis),
you must specify the iteration number in the restart file from which output is
required instead of the increment. If temperatures (or predefined field
variables) are read from a results (.fil) file in the
original direct cyclic analysis, the same temperatures (or predefined field
variables) must be read into the postprocessing analysis. This specification is
needed to recover thermal strains at each time increment in the original direct
cyclic analysis since the results file is not stored in the restart analysis
database.
Recovering Additional Output from a Low-Cycle Fatigue Analysis
If you use this postprocessing technique to recover additional output from a
previous low-cycle fatigue analysis (see
Low-Cycle Fatigue Analysis Using the Direct Cyclic Approach),
you must specify the cycle number in the restart file from which output is
required instead of the increment. If temperatures (or predefined field
variables) are read from a results (.fil) file in the
original low-cycle fatigue analysis, the same temperatures (or predefined field
variables) must be read into the postprocessing analysis. This specification is
needed to recover thermal strains at each time increment in the original
low-cycle fatigue analysis since the results file is not stored in the restart
analysis database.
Example
A job can be submitted using the following input file. The analysis for
which restart data were written must be specified when you submit the job
(using the oldjob parameter of the
Abaqus
execution procedure). This example creates a new data
(.dat) file containing tabular data. The first two tables
will contain data from increments 5 and 10 of Step 1 and will give the reaction
forces of the nodes in the set CLAMP, which
was defined when the analysis was run. The next table will contain data from
increment 3 of Step 2 and will give displacements from the new node set
TIP that is defined in this postprocessing
analysis.
The following example input file recovers additional output from a previous
direct cyclic analysis and creates a new output database
(.odb) file, which contains the stress and strain for the
elements in the set ELIST from each increment
in Iteration 5 of Step 1, followed by data from each increment in Iteration 10
of Step 1:
The following example input file recovers additional output from a previous
low-cycle fatigue analysis and creates a new output database
(.odb) file, which contains the stress and strain for the
elements in the set ELIST from each increment
in Cycle 5 of Step 1, followed by data from each increment in Cycle 10 of Step
1: