Abaqus Model Definition | ||||||||
|
| |||||||
ProductsAbaqus/StandardAbaqus/Explicit
The input file
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.
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. 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 Abaqus/Standard and Abaqus/Explicit execution).
- 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 in Abaqus/Standard and Abaqus/Explicit).
- Kinematic constraints
-
Equations involving several of the fundamental solution variables in the model (Linear constraint equations) or multi-point constraints (General multi-point constraints) can be defined.
- Interactions
-
Contact and other interactions between parts can be defined (About contact interactions).
- Amplitude definitions
-
Amplitude curves can be defined for later use in specifying time-dependent loading or boundary conditions (Amplitude Curves).
- Output control
-
You can control model definition output to the data file (About Output).
- 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), with a new mesh (About submodeling, Mesh-to-mesh solution mapping, and Symmetric model generation), or with the same or a different Abaqus program (About transferring results between Abaqus analyses).
History data
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).
Required history data
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).
- 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 and Output to the Output Database, and all of the output variables are listed in Output Variables. The available output files are described in About Output.
- Contact
-
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).
- 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). Solution controls for contact problems (Adjusting contact controls in Abaqus/Standard, Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit, or Contact controls for general contact in Abaqus/Explicit) 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.
- Co-simulation
-
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.
Input File Usage
INCLUDE, INPUT=file_name
Including an encrypted data file
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.
Input File Usage
INCLUDE, INPUT=file_name, PASSWORD=password