# Configuring a direct cyclic procedure

 A direct cyclic procedure is a quasi-static analysis that uses a combination of Fourier series and time integration of the nonlinear material behavior to obtain the stabilized cyclic response of the structure iteratively. To avoid the considerable numerical expense associated with a transient analysis, a direct cyclic procedure can be used to calculate the cyclic response of a structure directly. The basis of this method is to construct a displacement function $u¯⁢(t)$ that describes the response of the structure at all times t during a load cycle with period T. For more information, see Direct cyclic analysis. This task shows you how to:

Context:

Abaqus/Standard assumes geometrically linear behavior for a direct cyclic procedure. For more information, see Linear and nonlinear procedures.

## Create or edit a direct cyclic procedure

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

2. On the Basic, Incrementation, Fatigue, and Other tabbed pages, configure settings such as the cycle time period, maximum number of increments, increment size, low-cycle fatigue options, and equation solver preferences as described in the following procedures.

## Configure settings on the Basic tabbed page

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 Cycle time period field, enter the time of a single loading cycle.

4. Toggle on Use displacement Fourier coefficients from previous direct cyclic step to indicate that the current step is a continuation of the previous direct cyclic step. See Direct cyclic analysis, for more details.

## Configure settings on the Incrementation tabbed page

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 time 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.

3. In the Maximum number of increments field, enter the upper limit to the number of increments in a single loading cycle. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step. See Controlling the incrementation during the cyclic time period, for more details.

4. If you selected Automatic in Step 2, enter values for Increment size:

1. In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
2. 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.
3. In the Maximum field, enter the maximum time increment allowed.

5. If you selected Fixed in Step 2, enter a value for the constant time increment in the Increment size field.

6. In the Maximum number of iterations field, enter an upper limit for the number of cyclic iterations. See Controlling the iterations in the modified Newton method, for more details.

7. In the Number of Fourier terms fields, enter values for the Initial and Maximum number of Fourier terms and the Increment in the number of terms. The number of Fourier terms required to obtain an accurate solution depends on the variation of the load as well as the variation of the structural response over the period. More Fourier terms usually provide a more accurate solution but at the expense of additional data storage and computational time. Each of these values must be greater than 0 and less than 100. For more information, see Controlling the Fourier representations.

8. If you selected Automatic in Step 2, choose one or both of the following options:

• Toggle on Max. allowable temperature change per increment to enter the maximum temperature change to be allowed in an increment. Abaqus/Standard will restrict the time increment to ensure that this value is not exceeded at any node during any increment of the step.

• Toggle on Creep/swelling/viscoelastic strain error tolerance to enter the maximum difference in the creep strain increment calculated from the creep strain rates based on conditions at the beginning and end of the increment, thus controlling the time integration accuracy of the creep integration.

For more details about these options, see Automatic incrementation.

9. Toggle on Evaluate structure response at time points to define specific times at which the response should be evaluated. Click the arrow to the right of this field, and select a set of time points from the list that appears. Otherwise, click to define a new set of time points. See Defining time points and Defining the time points at which the response must be evaluated, for more details.

## Configure settings on the Fatigue tabbed page

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

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

2. Toggle on Include low-cycle fatigue analysis to use the direct cyclic approach to obtain the stabilized response of a structure subjected to periodic loading. Multiple cycles can be included in a single direct cyclic analysis. The analysis models progressive damage and failure on constitutive points in the bulk materials based on a continuum damage approach. It can also be used to model delamination/debonding growth at the interfaces in laminated composites. For more details, see Low-cycle fatigue analysis using the direct cyclic approach.

3. In the Cycle increment size fields, enter values for the Minimum and Maximum increment in the number of cycles over which the damage is extrapolated forward. Each value must be greater than 0. For more details, see Damage extrapolation technique in the bulk material.

4. In the Maximum number of cycles field, choose one of the following options to specify the total number of cycles allowed in the step:

• Choose Default to use a value that is equal to one plus half of the maximum increment in number of cycles over which the damage is extrapolated.

• Choose Value, and enter a number.

See Low-cycle fatigue analysis in Abaqus/Standard, for more details.

5. In the Damage extrapolation tolerance field, enter a value or accept the default of 1.0. The maximum extrapolated damage increment will be limited by this value. See Controlling the accuracy of damage extrapolation in the bulk material when using continuum damage mechanics approach, for more details.

## Configure settings on the Other tabbed page

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 for the 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.

3. 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.