Define Static Steps Using Automatic Time Incrementation
-
From the Procedures section of the action bar, click Static Step
.
- Optional: Enter a descriptive Name.
- In the Step Time field, enter the duration of the step.
-
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.
- From the Time incrementation selection options, select Automatic.
-
Adjust any of the following incrementation parameters:
Option Description 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 increment Shortest 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 increment Longest time increment allowed for the step. If you do not specify this value, the simulation does not impose an upper limit. - Optional:
Add artificial stabilization by selecting a
Stabilization Type.
For more information on adding stabilization to a step, see Adding Automatic Step Stabilization.
- Optional:
Complete the following steps to define how continuation data is generated.
Continuation data allows you to run subsequent restart simulations from this step.
-
Specify how frequently continuation data is generated for this
step.
Option Description None Generates no continuation data. Evenly spaced intervals Specifies the number of intervals during the step at which the data is generated. Every n increments Specifies the increments at which continuation data is written. For example, specifying every 2 increments generates the data at increments 2, 4, 6, etc. -
If you chose Evenly spaced intervals,
specify how the continuation data is managed.
Option Description Exact intervals Generates the continuation data at the exact times dictated by the specified number of intervals. Next closest increment Generates the continuation data at the increment ending immediately after the time dictated by the specified number of intervals. -
Specify the Interval data to keep.
Option Description Last saved Stores only the continuation data generated at the last increment of this step. All Stores the data generated at all the specified increments of this step.
-
Specify how frequently continuation data is generated for this
step.
- 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.
-
From the Matrix storage options, specify one of the
following options for the matrix storage and solution scheme:
Option Description 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.
- Click OK.