Steps, increments, and iterations

This section introduces some new vocabulary for describing the various parts of an analysis. It is important that you clearly understand the difference between an analysis step, a load increment, and an iteration.

  • The load history for a simulation consists of one or more steps. You define the steps, which generally consist of an analysis procedure option, loading options, and output request options. Different loads, boundary conditions, analysis procedure options, and output requests can be used in each step. For example:

    • Step 1: Hold a plate between rigid jaws.

    • Step 2: Add loads to deform the plate.

    • Step 3: Find the natural frequencies of the deformed plate.

  • An increment is part of a step. In nonlinear analyses the total load applied in a step is broken into smaller increments so that the nonlinear solution path can be followed.

    In Abaqus/Standard you suggest the size of the first increment, and Abaqus/Standard automatically chooses the size of the subsequent increments. In Abaqus/Explicit the default time incrementation is fully automatic and does not require user intervention. Because the explicit method is conditionally stable, there is a stability limit for the time increment. The stable time increment is discussed in Nonlinear Explicit Dynamics.

    At the end of each increment the structure is in (approximate) equilibrium and results are available for writing to the output database, restart, data, or results files. The increments at which you select results to be written to the output database file are called frames.

    The issues associated with time incrementation in Abaqus/Standard and Abaqus/Explicit analyses are quite different, since time increments are generally much smaller in Abaqus/Explicit.

  • An iteration is an attempt at finding an equilibrium solution in an increment when solving with an implicit method. If the model is not in equilibrium at the end of the iteration, Abaqus/Standard tries another iteration. With every iteration the solution Abaqus/Standard obtains should be closer to equilibrium; sometimes Abaqus/Standard may need many iterations to obtain an equilibrium solution. When an equilibrium solution has been obtained, the increment is complete. Results can be requested only at the end of an increment.

    Abaqus/Explicit does not need to iterate to obtain the solution in an increment.