Step Controls play an important role in static and transient dynamic analyses. Step controls are used to perform two distinct functions:
Specify the Analysis Settings for each step.
See the procedure, Specifying Analysis Settings for Multiple Steps located in the Establish Analysis Settings section.
The following items can be changed on a per step basis:
The selections available in the Details view for Step Controls group are described below.
Current Step Number: shows the step ID for which the settings in Step Controls, Nonlinear Controls, and Output Controls are applicable. The currently selected step is also highlighted in the bar at the bottom of the Graph window. You can select multiple steps by selecting rows in the data grid or the bars at the bottom of the Graph window. In this case the Current Step Number will be set to multi-step. In this case any settings modified will affect all selected steps.
Step End Time: shows the end time of the current step number. When multiple steps are selected this will indicate multi-step.
Auto Time Stepping: is discussed in detail in the Automatic Time Stepping section.
Automatic time stepping is available for static and transient analyses, and is especially useful for nonlinear solutions. Settings for controlling automatic time stepping are included in a drop down menu under Auto Time Stepping in the Details view. The following options are available:
(default setting): the Mechanical application automatically switches time stepping on and off as needed. A check is performed on non-convergent patterns. The physics of the simulation is also taken into account. The settings are presented in the following table:
|Auto Time Stepping Program Controlled Settings|
|Analysis Type||Initial Substeps||Minimum Substeps||Maximum Substeps|
|Linear Static Structural||1||1||1|
|Nonlinear Static Structural||1||1||10|
|Linear Steady-State Thermal||1||1||10|
|Nonlinear Steady-State Thermal||1||1||10|
: You control time stepping by completing the following fields that only appear if you choose this option. No checks are performed on non-convergent patterns and the physics of the simulation is not taken into account.
Initial Substeps: specifies the size of the first substep. The default is 1.
Minimum Substeps: specifies the minimum number of substeps to be taken (that is, the maximum time step size). The default is 1.
Maximum Substeps: specifies the maximum number of substeps to be taken (that is, the minimum time step size). The default is 10.
Number Of Substeps. The default is 1.: no time stepping is enabled. You are prompted to enter the
Define By allows you to set the limits on load increment in one of two ways. You can specify the Initial, Minimum and Maximum number of substeps for a step or equivalently specify the Initial, Minimum and Maximum time step size.
Carry Over Time Step is an option available when you have multiple steps. This is useful when you do not want any abrupt changes in the load increments between steps. When this is set the Initial time step size of a step will be equal to the last time step size of the previous step.
Time Integration is valid only for a Transient Structural or Transient Thermal analysis. This field indicates whether a step should include transient effects (for example, structural inertia, thermal capacitance) or whether it is a static (steady-state) step. This field can be used to set up the Initial Conditions for a transient analysis.
On: default for Transient analyses.
Off: do not include structural inertia or thermal capacitance in solving this step.
Note: With Time Integration set to Off in Transient Structural analyses, Workbench does not compute velocity results. Therefore spring damping forces, which are derived from velocity will equal zero. This is not the case for Rigid Dynamics analyses.
You can activate (include) or deactivate (delete) a load from being used in the analysis within the time span of a step. For most loads (for example, pressure or force) deleting the load is the same as setting the load value to zero. But for certain loads such as specified displacement this is not the case. Activation and deactivation of loads is not available to the Samcef or ABAQUS solver.
Note: Changing the method of how a multiple-step load value is specified (such as Tabular to Constant), the Activation/Deactivation state of all steps resets to the default, Active.
To activate or deactivate a load in a stepped analysis:
Highlight the load within a step in the Graph or a specific step in the Tabular Data window.
Click the right mouse button and choose Activate/Deactivate at this step!.
Note: For displacements and remote displacements, it is possible to deactivate only one degree of freedom within a step.
For Imported loads and Temperature, Thermal Condition, Heat Generation, Voltage, and Current loads, the following rules apply when multiple load objects of the same type exist on common geometry selections:
A load can assume any one of the following states during each load step:
Active: Load is active and data specified during the first step.
Reactivated: Load is active and data specified during the current step, but was deactivated during the previous step. A change in step status exists.
Deactivated: Load is deactivated at the current step, but was active and data applied during the previous step. A change in step status exists.
Unchanged: No change in step status exists.
During the first step, an active load will overwrite other active loads that exist higher (previously added) in the tree.
During any other subsequent step, commands are sent to the solver only if a change in step status exists for a load. Hence, any unchanged loads will get overwritten by other reactivated or deactivated loads irrespective of their location in the tree. A reactivated/deactivated load will overwrite other reactivated and deactivated loads that exist higher (previously added) in the tree.
Note: For each load step, if both Imported Loads and user-specified loads are applied on common geometry selections, the Imported Loads take precedence. See respective Imported Load for more details.
For imported loads specified as tables, with the exception of imported displacement and temperature loads, a value of zero is applied in the table where the load is deactivated, and commands are sent to the solver only at the first active load step. Hence these reactivated/deactivated imported loads with tabular loading do not overwrite other unchanged or reactivated/deactivated loads that exist higher (previously added) in the tree.
For imported loads specified as tables, the data is available outside the range of specified analysis times/frequencies. If the solve time/frequency for a step/sub-step falls outside the specified Analysis Time/Frequency, then the load value at the nearest specified analysis time is used.
Note: The tabular data view provides the equation for the calculation of values through piecewise linear interpolation at steps where data is not specified.
Some scenarios where load deactivation is useful are:
Springback of a cantilever beam after a plasticity analysis (see example below).
Bolt pretension sequence (Deactivation is possible by setting Define By to Open for the load step of interest).
Specifying different initial velocities for different parts in a transient analysis.
Example: Springback of a cantilever beam after a plasticity analysis
In this case a Y displacement of -2.00 inch is applied in the first Step. In the second step this load is deactivated (deleted). Deactivated portions of a load are shown in gray in the Graph and also have a red stop bars indicating the deactivation. The corresponding cells in the data grid are also shown in gray.
In this example the second step has a displacement value of -1.5. However since the load is deactivated this will not have any effect until the third step. In the third step a displacement of -1.5 will be step applied from the sprung-back location.