Configuring a dynamic, implicit procedure

1. Display the Edit Step dialog box following the procedure outlined in Creating a step (Procedure type: General; Dynamic, Implicit), or Editing a step.

2. On the Basic, Incrementation, and Other tabbed pages, configure settings such as the time period for the step, increment size, and equation solver preferences as described in the following procedures.

1. In the Edit Step dialog box, display the Basic tabbed page.

2. In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.

3. In the Time period field, enter the time period of the step.

4. Select an Nlgeom option:

   • 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.

5. Select an Application option. The application setting adjusts various numerical settings (such as damping and time incrementation) to most efficiently and accurately capture the intended behavior of your analysis.

   • Transient fidelity applications—such as an analysis of satellite systems—use small time increments to accurately resolve the vibrational response of the structure, and numerical energy dissipation is kept at a minimum.

   • Moderate dissipation applications—including various insertion, impact, and forming analyses—use some energy dissipation (via plasticity, viscous damping, or numerical effects) to reduce solution noise and improve convergence behavior without significantly degrading solution accuracy.

   • Quasi-static applications introduce inertia effects primarily to regularize unstable behavior in analyses whose main focus is a final static response. Large time increments are taken when possible to minimize computational cost, and considerable numerical dissipation may be used to obtain convergence during certain stages of the loading history.

   • The Analysis product default depends on the presence of contact in the model: analyses involving contact are treated as moderate dissipation applications; analyses without contact are treated as transient fidelity applications.

6. Toggle on Include adiabatic heating effects if you are performing an adiabatic stress analysis. This option is relevant only for isotropic metal plasticity materials with a Mises yield surface. For more information, see Adiabatic analysis.

1. In the Edit Step dialog box, display the Incrementation tabbed page.

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

2. Choose a Type option:

   • Choose Automatic to allow Abaqus/Standard to choose the size of the increments based on computational efficiency.

   • 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.

     Warning: Fixed incrementation is not generally recommended; it should be used only in special cases when you have a thorough understanding of how to interpret results obtained in this way. Impact events are particularly difficult to solve using fixed time increments.

3. In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step.

4. If you selected Automatic in Step 2, do the following:

   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.

   2. Specify the Maximum increment size:

      • Choose Specify to enter the maximum increment size directly.

      • Choose Analysis application default to set the maximum increment size automatically based on the application setting:

        • For transient fidelity applications, the default maximum increment is the time period of the step divided by 100.

        • For moderate dissipation applications, the default maximum increment is the time period of the step divided by 10.

        • For quasi-static applications, the default maximum increment is the time period of the step.

   3. The half-increment residual tolerance represents the equilibrium residual error (out-of-balance forces) halfway through a time increment. If the half-increment residual is small, it indicates that the accuracy of the solution is high and that the time step can be increased safely; conversely, if the half-increment residual is large, the time step used in the solution should be reduced. For more information, see Numerical details.

      You must specify an appropriate Half-increment Residual:

      • Toggle on Suppress calculation to reduce the solution cost by skipping half-increment residual tolerance checks.

      • Choose Analysis product default to set a half-increment residual tolerance automatically based on the application setting:

        • For transient fidelity applications involving contact, the default half-increment residual tolerance is 10,000 times the time average force and moment values.

        • For transient fidelity applications without contact, the default half-increment residual tolerance is 1000 times the time average force and moment values.

        • For moderate dissipation and quasi-static applications, the half-increment residual tolerance checks are suppressed.

      • Choose Specify scale factor to enter the half-increment residual tolerance as a scale factor applied to the time average force and moment values.

      • Choose Specify value to enter the half-increment residual tolerance value directly.

5. If you selected Fixed in Step 2, do the following:

   1. Enter a value for the constant time increment in the Increment size field.
   2. If desired, toggle on Suppress calculation to skip half-increment residual tolerance checks and reduce the solution cost.

1. In the Edit Step dialog box, display the Other tabbed page.

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

2. Choose a Matrix storage option:

   • 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.

3. Choose a Solution technique:

   • 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.

4. Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:

   • 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.

5. Choose an option for Default load variation with time:

   • 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.

6. Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:

   • Select None to suppress any extrapolation.

   • 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 displacement-based extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.

   • Select Velocity parabolic to indicate that the process should use a quadratic velocity-based extrapolation, in time, of the previous incremental solutions to begin the nonlinear equation solution for the current increment.

   • Select Analysis product default to select the extrapolation method automatically based on the application setting:

     • For transient fidelity applications, Abaqus/Standard uses the velocity-based parabolic extrapolation method.

     • For moderate dissipation and quasi-static applications, Abaqus/Standard uses the linear extrapolation method.

   For more information, see Extrapolation of the solution.

7. For transient fidelity applications, indicate Alpha, the numerical (artificial) damping control parameter in the implicit operator:

   • Choose Analysis product default to set $\alpha$= −0.05 for slight numerical damping.

   • Choose Specify to enter a nondefault value for $\alpha$. Allowable values are zero (no damping) to −0.5 ($\alpha$= −0.333 provides maximum damping).

   For moderate dissipation applications, $\alpha$ cannot be modified from the default value of −0.41421. The $\alpha$ parameter is not used in quasi-static applications.

8. Indicate how Abaqus/Standard should handle Initial acceleration calculations at beginning of step:

   • Choose Allow to calculate the actual accelerations in a model at the beginning of the dynamic step.

   • Choose Bypass to set the initial accelerations based on the following criteria:

     • If the current step is the first dynamic step, Abaqus/Standard assumes that the initial accelerations for the current step are zero.

     • If the immediately preceding step was also a dynamic step, Abaqus/Standard uses the accelerations from the end of the previous step to continue the new step.

     This approach is appropriate only if the loading does not change suddenly at the start of the new step. For more information, see Controlling calculation of accelerations at the beginning of a dynamic step.

   • Choose Analysis product default to determine the initial accelerations based on the application setting used for the step (this option is available only if the Application option on the Basic tabbed page is also set to Analysis product default):

     • For transient fidelity applications, the actual initial accelerations are calculated.

     • For moderate dissipation applications, the actual initial accelerations are set based on the criteria described above for the Bypass option.

9. If you selected Fixed time incrementation on the Incrementation tabbed page, you can toggle on Accept solution after reaching maximum number of iterations. This option directs Abaqus/Standard to accept the solution to an increment after the maximum number of iterations allowed has been completed, even if the equilibrium tolerances are not satisfied. Very small increments and a minimum of two iterations are usually necessary if you use this option.

   Warning: This approach is not recommended; you should use it only in special cases when you have a thorough understanding of how to interpret results obtained in this way.

When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.