Defining Static Steps

You can define a static step to perform a stress analysis of a stable problem in which the analysis neglects inertia effects. The response can be linear or nonlinear.

You can create a static step with automatic time incrementation to have the simulation adjust the size of the time increments to solve problems effectively and efficiently. In most cases, the default automatic incrementation scheme is preferred because the solver selects increment sizes based on computational efficiency. If you have considerable experience with a particular problem, you might be able to select a more economical approach by using fixed time incrementation to manually specify the time increment.

This task shows you how to:

See Also
About Static Steps

Define Static Steps Using Automatic Time Incrementation

  1. From the Procedures section of the action bar, click Static Step .
  2. Optional: Enter a descriptive Name.
  3. In the Step Time field, enter the duration of the step.
  4. In the Maximum increments field, specify the upper limit to the number of increments in the step.

    The analysis stops if this maximum is exceeded before the Abaqus solvers arrive at the complete solution for the step.

  5. From the Time incrementation selection options, select Automatic.
  6. Adjust any of the following incrementation parameters:
    OptionDescription
    Initial time increment Length of the initial time increment. The app modifies this value as required throughout the step. If you specify a value of zero, the app assumes a default value equal to the total time period of the step.
    Minimum time incrementShortest time increment allowed for the step. The app initially displays the minimum time increment allowed. If the Abaqus solvers need a smaller time increment than this value, the simulation ends. If this value is zero, the simulation assumes a default value of the smaller of the suggested initial time increment or 10-5 times the total time period.
    Maximum time incrementLongest time increment allowed for the step. If you do not specify this value, the simulation does not impose an upper limit.
  7. Optional: Add artificial stabilization by selecting a Stabilization Type.

    For more information on adding stabilization to a step, see Adding Automatic Step Stabilization.

  8. Optional: Select Include geometric nonlinearity to indicate that geometric nonlinearity is accounted for during the step.

    Once you enable this option, it is active during all subsequent steps in the simulation.

  9. From the Matrix storage options, specify one of the following options for the matrix storage and solution scheme:
    OptionDescription
    Solver default Uses a matrix storage and solution scheme chosen by the Abaqus solvers to store the stiffness matrix.
    Symmetric Uses the symmetric matrix storage and solution scheme to store the stiffness matrix.
    Unsymmetric Uses the unsymmetric matrix storage and solution scheme to store the stiffness matrix.

    For more information about these options, see Matrix Storage and Solution Scheme in Abaqus/Standard.

  10. Click OK.

Define Static Steps Using Fixed Time Incrementation

  1. From the Procedures section of the action bar, click Static Step .
  2. Optional: Enter a descriptive Name.
  3. In the Step Time field, enter the duration of the step.
  4. In the Maximum increments field, specify the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before the Abaqus solvers arrive at the complete solution for the step.
  5. From the Time incrementation selection options, select Fixed.
  6. Enter the constant Time increment size.
  7. Optional: Add artificial stabilization by selecting a Stabilization Type.

    For more information on adding stabilization to a step, see Adding Automatic Step Stabilization.

  8. Optional: Select Include geometric nonlinearity to indicate that geometric nonlinearity is accounted for during the step.

    Once you enable this option, it is active during all subsequent steps in the simulation.

  9. From the Matrix storage options, specify one of the following options for the matrix storage and solution scheme:
    OptionDescription
    Solver default Uses a matrix storage and solution scheme chosen by the Abaqus solvers to store the stiffness matrix.
    Symmetric Uses the symmetric matrix storage and solution scheme to store the stiffness matrix.
    Unsymmetric Uses the unsymmetric matrix storage and solution scheme to store the stiffness matrix.

    For more information, see Defining an Analysis.

  10. Click OK.