Configuring a transient, static, stress/displacement analysis with time-dependent material response

• Toggle Nlgeom Off to perform a geometrically linear analysis during the current step.

• Toggle Nlgeom On to indicate that Abaqus/Standard should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.

For more information, see Linear and nonlinear procedures.

Click the arrow to the right of Automatic stabilization, and select a method for defining the damping factor:

• Select Specify dissipated energy fraction to allow Abaqus/Standard to calculate the damping factor from a dissipated energy fraction that you provide. Enter a value for the dissipated energy fraction in the adjacent field (the default is 2.0 × 10⁻⁴). For more information, see Calculating the Damping Factor Based on the Dissipated Energy Fraction.

• Select Specify damping factor to enter the damping factor directly. Enter a value for the damping factor in the adjacent field. For more information, see Directly Specifying the Damping Factor.

• Select Use damping factors from previous general step to use the damping factors at the end of the previous step as the initial factors in the current step's variable damping scheme. These factors override any initial damping factors that are calculated or specified directly in the current step. If there are no damping factors associated with the previous general step (for example, if the previous step does not use any stabilization or the current step is the first step of the analysis), Abaqus uses adaptive stabilization to determine the required damping factors.

To use adaptive stabilization, toggle on Use adaptive stabilization with max. ratio of stabilization to strain energy (if necessary), and enter a value in the adjacent field for the allowable accuracy tolerance for the ratio of energy dissipated by damping to total strain energy in each increment. The default value of 0.05 should be suitable in most cases.

(For information on displaying the Edit Step dialog box, see Creating a step, or Editing a step.)

• Choose Automatic if you want Abaqus/Standard to select time increments automatically based on the accuracy of the integration. A Creep/swelling/viscoelastic strain error tolerance parameter that you specify limits the maximum inelastic strain rate change allowed over an increment. Automatic incrementation is recommended for almost all cases.

• Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an increment size that you specify as the constant increment size throughout the step.

1. Enter values for Increment size:

   • In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.

   • In the Minimum field, enter the minimum time increment allowed. If Abaqus/Standard needs a smaller time increment than this value, it terminates the analysis.

   • In the Maximum field, enter the maximum time increment allowed.

2. In the Creep/swelling/viscoelastic strain error tolerance field, enter the maximum difference in the creep strain increment calculated from the creep strain rates at the beginning and at the end of the increment. This value controls the accuracy of the creep integration. For more information, see Automatic Incrementation.

• Choose Explicit/Implicit if you want to allow Abaqus/Standard to invoke the implicit integration scheme. For creep at very low stress levels the unconditional stability of the backward difference operator (implicit method) is desirable.

• Choose Explicit if you want to restrict Abaqus/Standard to using explicit integration. Explicit integration can be less expensive computationally and simplifies implementation of user-defined creep laws in user subroutine CREEP

For more information, see Selecting Explicit Creep Integration.

(For information on displaying the Edit Step dialog box, see Creating a step, or Editing a step.)

• Choose Direct to use the default direct sparse solver.

• Choose Iterative to use the iterative linear equation solver. The iterative solver is typically most useful for blocky structures with millions of degrees of freedom. For more information, see Iterative Linear Equation Solver.

• Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.

• Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.

• Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.

For more information on matrix storage, see Matrix Storage and Solution Scheme in Abaqus/Standard.

• Choose Full Newton to use Newton's method as a numerical technique for solving nonlinear equilibrium equations. For more information, see Nonlinear solution methods in Abaqus/Standard.

• Choose Quasi-Newton to use the quasi-Newton technique for solving nonlinear equilibrium equations. This technique can save substantial computational cost in some cases. Generally it is most successful when the system is large and the stiffness matrix is not changing much from iteration to iteration. You can use this technique only for symmetric systems of equations.

  If you choose this technique, enter a value for the Number of iterations allowed before the kernel matrix is reformed. The maximum number of iterations allowed is 25. The default number of iterations is 8.

  For more information, see Quasi-Newton solution technique.

• Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.

• Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.

• Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.

For more information on severe discontinuities, see Severe Discontinuities in Abaqus/Standard.

• Choose Instantaneous if you want loads to be applied instantaneously at the start of the step and remain constant throughout the step.

• Choose Ramp linearly over step if the load magnitude is to vary linearly over the step, from the value at the end of the previous step to the full magnitude of the load.

• Select Linear to indicate that the process is essentially monotonic and Abaqus/Standard should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.

• Select Parabolic to indicate that the process should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.

• Select None to suppress any extrapolation.

For more information, see Extrapolation of the Solution.