Products: ABAQUS/Standard ABAQUS/Explicit
A finite element analysis in ABAQUS is defined by an input file, which
contains keyword lines and data lines; and
is divided into model data and history data.
An ABAQUS input file is an ASCII data file. It can be created by using a text editor or by using a graphical preprocessor such as ABAQUS/CAE. 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,” Section 1.2.1.
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 must begin 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 (“Output,” Section 4.1.1). The first heading line will appear as a heading at the top of each page of the output.
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 “Defining an assembly,” Section 2.9.1.
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.
Most 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,” Section 7.7), 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 define the nodes, elements, materials, initial conditions, etc.
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,” Section 2.1.1; “Element definition,” Section 2.2.1; and “Defining an assembly,” Section 2.9.1. 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 Part V, “Elements,” along with explanations of how to define the elements. You can view the initial mesh or the configuration after adjustment for initial overclosure in the Visualization module of ABAQUS/CAE after a data check run (see “Execution procedure for ABAQUS/Standard and ABAQUS/Explicit,” Section 3.2.2).
Material definitions: A material type must be associated with most portions of the geometry. The material library is described in Part IV, “Materials.” Special elements such as springs or dashpots do not have an associated material, but their properties must be defined.
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 (“Defining an assembly,” Section 2.9.1).
Initial conditions: Nonzero initial conditions such as initial stresses, temperatures, or velocities can be specified (“Initial conditions,” Section 19.2.1).
Boundary conditions: Zero-valued boundary conditions (including symmetry conditions) can be imposed on individual solution variables such as displacements or rotations (“Boundary conditions,” Section 19.3.1).
Kinematic constraints: Equations involving several of the fundamental solution variables in the model (“Linear constraint equations,” Section 20.2.1) or multi-point constraints (“General multi-point constraints,” Section 20.2.2) can be defined.
Interactions: Contact and other interactions between parts can be defined (“Contact interaction analysis: overview,” Section 21.1.1).
Amplitude definitions: Amplitude curves can be defined for later use in specifying time-dependent loading or boundary conditions (“Amplitude curves,” Section 19.1.2).
Output control: You can control model definition output to the data file (“Output,” Section 4.1.1).
Environment properties: Environment properties, such as the attributes of a fluid surrounding the model, may have to be defined.
Analysis continuation: It is possible to write restart data or to use the results from a previous analysis and continue the analysis with new model or history data (“Restarting an analysis,” Section 7.1.1), with a new mesh (“Submodeling,” Section 7.3.1; “Mesh-to-mesh solution mapping,” Section 7.5.2; and “Symmetric model generation,” Section 7.8.1), or with the same or a different ABAQUS program (“Transferring results between ABAQUS analyses: overview,” Section 7.7.1).
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 “Procedures: overview,” Section 6.1.1.) 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 linear perturbation procedures,” Section 6.1.2). A general analysis step contributes to the response history of the system; a linear perturbation step allows the investigation of the linearized response of the system at any stage during 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 “Convergence and time integration criteria: overview,” Section 8.3.1) 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 “Output,” Section 4.1.1).
| Input File Usage: | Use the following option to begin a step definition: |
*STEP Use the following option to end a step definition: *END STEP |
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 “Procedures: overview,” Section 6.1.1). 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.
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 (“Applying loads: overview,” Section 19.4.1), temperature changes leading to thermal expansion can be prescribed (“Thermal expansion,” Section 12.1.2), or contact conditions can be used to apply loads (“Contact interaction analysis: overview,” Section 21.1.1).The loading can be prescribed as a function of time (“Amplitude curves,” Section 19.1.2). 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 “Procedures: overview,” Section 6.1.1).
Boundary conditions: Zero-valued or nonzero boundary conditions can be added, modified, or removed during an analysis (“Boundary conditions,” Section 19.3.1).
Output control: Quantities such as stress, strain, reaction force, temperature, and energy are available as output. The output options are described in “Output to the data and results files,” Section 4.1.2, and “Output to the output database,” Section 4.1.3; and all of the output variables are listed in “ABAQUS/Standard output variable identifiers,” Section 4.2.1, and “ABAQUS/Explicit output variable identifiers,” Section 4.2.2. The available output files are described in “Output,” Section 4.1.1.
Contact: Contact surfaces and contact interactions can be added, modified, or removed as step-dependent history data during an ABAQUS/Explicit analysis (see “Contact interaction analysis: overview,” Section 21.1.1).
Auxiliary controls: You can overwrite the solution controls that are built into ABAQUS. In some procedures these values are given in the procedure definition. More generally in ABAQUS/Standard they are given by defining solution controls (“Commonly used control parameters,” Section 8.3.2). Solution controls for contact problems (“Common difficulties associated with contact modeling in ABAQUS/Standard,” Section 21.2.9; “Common difficulties associated with contact modeling using the contact pair algorithm in ABAQUS/Explicit,” Section 21.4.6; or “Contact controls for general contact,” Section 21.3.6) can also be defined.
Element and surface removal/reactivation: In ABAQUS/Standard portions of the model can be removed or reactivated from step to step. See “Element and contact pair removal and reactivation,” Section 7.5.1.
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. UNIX environment variables can be used to specify the file names.
| Input File Usage: | *INCLUDE, INPUT=file_name |