An
Abaqus
input file is an ASCII data file. It can be
created by using a text editor or by using a graphical preprocessor.
The input file consists of a series of lines containing
Abaqus
options (keyword lines) and data (data lines). The input syntax for keyword and
data lines is described in
Input Syntax Rules.
Most input files have the same basic structure. The following portions of
the input file are specified to define a finite element model:
An input file often begins with the
HEADING option, which is used to define a title for the analysis.
Any number of data lines can be used to give the title; they will appear at the
beginning of the output files (About Output).
The first heading line will appear as a heading at the top of each page of the
output.
While including a title can be helpful for users examining your input
file, the
HEADING option is not required.
After the heading the input file usually contains a
model data section to define nodes, elements,
materials, initial conditions, etc. The model data section is explained below.
If the model is organized into an assembly of part instances, the model
data are further categorized and must fall within the proper level: part,
assembly, instance, or model. Models defined in terms of an assembly of part
instances are discussed in
Assembly Definition.
Finally, the input file contains history
data to define the analysis type, loading, output requests, etc. Step
definitions divide the model data from the history data in an input file:
everything appearing before the first step definition is model data, and
everything appearing within and following the first step definition is history
data. The history data section is explained below.
The input file is processed by the “analysis input file processor”
prior to executing the appropriate analysis product,
Abaqus/Standard
or
Abaqus/Explicit.
The functions of the
analysis input file processor
are to interpret the
Abaqus
options, to perform the necessary consistency checking, and to prepare the data
for the analysis products.
Most computational mechanics modeling options (element types, loading types, etc.) are available
in both Abaqus/Standard and Abaqus/Explicit, although some options are available in only one analysis product or the other. All of
the step procedure types used in an input file must be from the same analysis product;
however, it is possible to import a solution from Abaqus/Standard into Abaqus/Explicit and vice versa (see Importing and Transferring Results), which
allows each analysis product to be used at the various stages of an analysis for which it is
best suited (for example, a static preloading in Abaqus/Standard followed by a dynamic analysis in Abaqus/Explicit).
Model Data
Model data define the nodes, elements, materials, initial conditions, etc.
Required Model Data
The following model data must be included in an input file to define a
finite element model:
Geometry
The geometry of a model is described by elements and their nodes. The rules
and methods for defining nodes and elements are described in
Node Definition,
Element Definition,
and
Assembly Definition.
Cross-sections for structural elements (such as beams) must be defined. Special
features can be defined with special elements such as springs, dashpots, point
masses, etc. The element types available for modeling are described in
About the Element Library,
along with explanations of how to define the elements.
Material
definitions
A material type must be associated with most portions of the geometry. The
material library is described in
About the Material Library.
Special elements such as springs or dashpots do not have an associated
material, but their properties must be defined.
Optional Model Data
The following model data can be included as necessary:
Parts and an
assembly
The geometry of a model can be defined by organizing it into parts, which
are positioned relative to one another in an assembly (Assembly Definition).
Initial
conditions
Nonzero initial conditions such as initial stresses, temperatures, or velocities can be specified
(Initial Conditions).
Boundary
conditions
Zero-valued boundary conditions (including symmetry conditions) can be
imposed on individual solution variables such as displacements or rotations
(Boundary Conditions).
The purpose of an analysis is to predict the response of a model to some
form of external loading or to some nonequilibrium initial conditions. An
Abaqus
analysis is based on the concept of steps, which
are described in the history data portion of the input file. (For more
information on steps, see
Defining an Analysis.)
The history input data are combined within a step as needed to define the
history of the analysis.
Multiple steps can be defined in an analysis. Steps can be introduced simply
to change the output requests or to change the loads, boundary conditions,
analysis procedure, etc. There is no limit on the number of steps in an
analysis.
There are two kinds of steps in
Abaqus:
general response analysis steps, which can be linear or nonlinear; and, in
Abaqus/Standard,
linear perturbation steps (see
General and Perturbation Procedures).
A general analysis step contributes to the response history of the system; a
linear perturbation step allows the investigation of the perturbation response
of the system with respect to a base state at any stage during the response
history. The solution from the perturbation response is not carried over to
subsequent steps and, therefore, does not contribute to the response history.
The state at the end of a general step provides the initial conditions for
the next step, making it easy to simulate consecutive loadings of a model, such
as a dynamic response following a static preload or the loading of a product
during its usage following a simulation of the manufacturing process.
The optional history data described below prescribing the loading; boundary
conditions; output controls; auxiliary controls; and, in
Abaqus/Explicit,
contact conditions are continued from one general analysis step to the next
general analysis step unless modified. For example, the solution controls
prescribed in a general analysis step in
Abaqus/Standard
(see
About Convergence and Time Integration Criteria)
will remain in effect for all subsequent general analysis steps until they are
modified or reset. For linear perturbation steps only the output controls are
continued from one linear perturbation step to the next if there are no
intermediate general analysis steps and the output controls are not redefined
(see
About Output).
Input File Usage
Use the following option to begin a step definition:
The following history data must be included in an input file to define an
analysis procedure:
Response type
An option to define the analysis procedure type must appear immediately
after the beginning of the step definition.
Abaqus
can perform many types of analyses—linear or nonlinear, static or dynamic, etc.
(see
Defining an Analysis).
The type of analysis can be changed from step to step. For example, in
Abaqus/Standard a
static preload can be analyzed first, then the response type can be changed to
transient dynamic. In this way a linear or nonlinear dynamic analysis can be
performed based on the conditions at the end of the static solution.
Optional History Data
The following history data can be included as necessary:
Loading
Usually some form of external loading is defined. For example, concentrated
or distributed loads can be applied (About Loads),
temperature changes leading to thermal expansion can be prescribed (Thermal Expansion),
or contact conditions can be used to apply loads (About Contact Interactions).
The loading can be prescribed as a function of time (Amplitude Curves).
This feature can be used to prescribe loadings such as the ground motion during
a seismic event, known accelerations, or the temperature and pressure history
during a transient in an engine. If an amplitude curve is not defined,
Abaqus
assumes either that the loading varies linearly over the step or that the load
is applied instantaneously at the beginning of the step, depending on the
chosen response type (see
Defining an Analysis).
Boundary
conditions
Boundary conditions can be added, modified, or removed during an analysis
(Boundary Conditions).
Contact surfaces and contact interactions can be added, modified, or removed
as step-dependent history data during an
Abaqus/Explicit
analysis (see
About Contact Interactions).
The steps in the
Abaqus
model must be defined such that the co-simulation fits entirely within a single
Abaqus
step. Further, there can be only one co-simulation in the
Abaqus
job.
Including Model or History Data from an External File
You can specify an external file that contains a portion of the
Abaqus
input file. This file can include model and history definition data, comment
lines, and other references to external files. When a reference to an external
file is encountered,
Abaqus
will immediately process the data within the specified file. When the
end-of-file is reached,
Abaqus
will return to processing the original file.
A maximum of five levels of nested external file references can be used.
Linux
environment variables can be used to specify the file names.
You can include an encrypted file by reference in an
Abaqus
input file or in another data file. When you refer to the encrypted file, you
must also provide the file's password. If the password is correct,
Abaqus
processes the data within the specified file as it would for an unencrypted
external file. Material and connector behavior definitions within an encrypted
input file are not written to the output database. In addition, all material
and connector behavior definitions output to the data file are suppressed if an
encrypted file is used as input for any portion of the model. See
Encrypting and Decrypting Abaqus Input Data
for details about the encryption utility.
Some encrypted files are eligible for inclusion only by users with a license
for a particular
Abaqus
feature (such as
Abaqus/Explicit)
or to users at a particular site. If you attempt to include an encrypted file
for which you do not have the proper privileges,
Abaqus
issues an error message.
You cannot include encrypted input files that contain parametric input.