2.2 Format of the input file

The ABAQUS input file is the means of communication between the preprocessor, usually ABAQUS/CAE, and the analysis product, ABAQUS/Explicit. The input file, which contains a complete description of the numerical model, is a text file with an intuitive, keyword-based format. It is easily modified using a text editor. Indeed, the input file for small analyses can be specified by typing it directly into an editor. If you are using ABAQUS/CAE, you will not need to see the input file. However, by understanding the input file, you will get a good understanding of how to use ABAQUS/Explicit.

We use the example of an overhead hoist shown in Figure 2–1 to illustrate the basic format of the ABAQUS input file. The hoist is a simple, pin-jointed framework that is constrained at the left-hand end and mounted on rollers at the right-hand end. The members can rotate freely at the joints. Since the model is two-dimensional, the frame is prevented from moving out of plane. A simulation is performed to determine the structure's deflection and the peak stress in its members when a 10 kN load is applied as shown in Figure 2–1.

Figure 2–1 Schematic of an overhead hoist.

Since this problem is very simple, the ABAQUS input file is compact and easy to understand. The complete ABAQUS input file for this example, which is shown in Figure 2–2 and also in “Overhead hoist frame,” Section A.1, is split into two distinct parts. The first section contains model data and includes all the information required to define the structure. The second section contains history data that define the model's loading history. The history can be further subdivided into a sequence of steps, each defining a separate stage of the simulation.

The input file is composed of a number of option blocks that contain data describing a part of the model. Each option block begins with a keyword line, which is usually followed by one or more data lines. These lines cannot exceed 256 characters.

Figure 2–2 Input for overhead hoist model.

2.2.1 Keyword lines

Keywords (or options) always begin with a star or asterisk (*). For example, *NODE is the keyword for specifying the nodal coordinates, and *ELEMENT is the keyword for specifying the element connectivity. Keywords are often followed by parameters, which may be required or optional. The *ELEMENT option requires the TYPE parameter because the element type must always be given when defining elements. For example,

*ELEMENT, TYPE=T2D2

indicates that we are defining T2D2 elements (two-dimensional truss elements with two nodes). Many parameters are optional and are defined only in certain circumstances. For example,

*NODE, NSET=PART1

indicates that all the nodes defined in this option block will be put into a set called PART1. It is not essential to put nodes into sets, although it is often convenient.

Keywords and parameters are case independent and must use enough characters to make them unique. Parameters are separated by commas. If a parameter has a value, use an equal sign (=) to associate the value with the parameter.

Occasionally, so many parameters are required that they will not all fit on a single 256-character line. In this case a comma is placed at the end of the line to indicate that the next line is a continuation line. For example,

*ELEMENT, TYPE = T2D2,
ELSET = FRAME

is a valid keyword line.

Details of the keywords are documented in the ABAQUS Keywords Manual.

2.2.2 Data lines

Keyword lines are usually followed by data lines, which provide data that are more easily specified as lists than as parameters on the keyword line. Examples of such data include nodal coordinates; element connectivities; or tables of material properties, such as stress-strain curves. The data required for particular option blocks are specified in the ABAQUS Keywords Manual. For example, the option block defining the nodes for the overhead hoist model is:

*NODE
101, 0., 0., 0.
102, 1., 0., 0.
103, 2., 0., 0.
104, 0.5, 0.866, 0.
105, 1.5, 0.866, 0.

The first piece of data on each data line is an integer that defines the node number. The second, third, and fourth entries are floating-point numbers that specify the

coordinates of the node.

The data can consist of a mixture of integer, floating-point, or alphanumeric values. Floating point values can be entered in a variety of ways; for example, ABAQUS interprets all of the following as the number four:

4.0	4.	4
4.0E+0	.4E+1	40.E–1

Data items are separated by commas, as in Figure 2–2, which allows fairly arbitrary spacing of the input values on the data line. If there is only one item on a data line, it must be followed by a comma.