Finite elements and nodes define the basic geometry of the physical structure being modeled in ABAQUS. Each element in the model represents a discrete portion of the physical structure, which is, in turn, represented by many interconnected elements. Elements are connected to one another by shared nodes. The coordinates of the nodes and the connectivity of the elements—that is, which nodes belong to which elements—comprise the model geometry. The collection of all the elements and nodes in a model is called the mesh. Generally, the mesh will be only an approximation of the actual geometry of the structure.

The element type, shape, and location, as well as the overall number of elements used in the mesh, affect the results obtained from a simulation. The greater the mesh density (i.e., the greater the number of elements in the mesh), the more accurate the results. As the mesh density increases, the analysis results converge to a unique solution, and the computer time required for the analysis increases. The solution obtained from the numerical model is generally an approximation to the solution of the physical problem being simulated. The extent of the approximations made in the model's geometry, material behavior, boundary conditions, and loading determines how well the numerical simulation matches the physical problem.

ABAQUS has a wide range of elements, many of which have geometry not defined completely by the coordinates of their nodes. For example, the layers of a composite shell or the dimensions of an I-beam section are not defined by the nodes of the element. Such additional geometric data are defined as physical properties of the element and are necessary to define the model geometry completely (see Chapter 3, “Finite Elements and Rigid Bodies”).

Material properties for all elements must be specified. While high-quality material data are often difficult to obtain, particularly for the more complex material models, the validity of the ABAQUS results is limited by the accuracy and extent of the material data.

Loads distort the physical structure and, thus, create stress in it. The most common forms of loading include:

Boundary conditions are used to constrain portions of the model to remain fixed (zero displacements) or to move by a prescribed amount (nonzero displacements). In a static analysis enough boundary conditions must be used to prevent the model from moving as a rigid body in any direction; otherwise, unrestrained rigid body motion causes the stiffness matrix to be singular. A solver problem will occur during the solution stage and may cause the simulation to stop prematurely.

ABAQUS will issue a warning message if it detects a solver problem during a simulation. It is important that you learn to interpret such error messages issued by ABAQUS. If you see a “numerical singularity” or “zero pivot” warning message during a static stress analysis, you should check whether all or part of your model lacks constraints against rigid body translations or rotations. In a dynamic analysis inertia forces prevent the model from undergoing infinite motion instantaneously as long as all separate parts in the model have some mass; therefore, solver problem warnings in a dynamic analysis usually indicate some other modeling problem, such as excessive plasticity.

The most common type of simulation is a static analysis, where the long-term response of the structure to the applied loads is obtained. In other cases the dynamic response of a structure to the loads may be of interest: for example, the effect of a sudden load on a component, such as occurs during an impact, or the response of a building in an earthquake.

ABAQUS can carry out many different types of simulations, but this guide only covers the two most common: static and dynamic stress analyses.

An ABAQUS simulation can generate a large amount of output. To avoid using excessive disk space, you can use options that limit the output to that required for interpreting the results.