In ANSYS Mechanical Workbench, steps are changes in the load history, which are defined by the user. For example, through the use of multiple steps, a user can (a) analyze the tightening of bolts of a gasket assembly, then (b) subject that assembly, including the bolt pre-load, to external loads such as pressure and temperature loading. A third step can be introduced to unload the bolts to see the permanent deformation in the gasket. This history-dependent behavior cannot be captured if all of the loads were to be applied at the same time, so the concept of steps can play an integral part of the solution setup.This post will discuss two tips related to controlling multiple steps:
- How to change solution options for multiple steps
- How to specify different values of time
Changing Solution Options for Multiple Steps
The Analysis Settings branch (highlighted in blue above) controls the number of steps used in a solution. Each step has substep and output controls specified in the Details view, and a summary of all steps is shown when the Worksheet icon (highlighted in red) is selected. The Worksheet view is read-only, however, which may confuse users wishing to change options for multiple steps.
In the Tabular Data section, use Shift-click or Ctrl-click to select the steps that will have the same solution options. Then, right-click and choose “Select All Highlighted Steps” (highlighted in red).
The Details view will show “Current Step Number: Multi Step,” indicating that any subsequent changes to the solution options — the number of substeps, nonlinear options or frequency of saving results — will be specified for those selected steps. This is an easy way to change the solution options for multiple steps at once.
Specifying Different Values of Time
For nonlinear static analyses with rate-dependent materials, time has real significance. Although inertial effects are neglected in a static analysis, with rate-dependent materials such as creep, the time-dependent effects require that the simulation time reflect the actual time. In transient analyses, solving the real time is needed to capture acceleration and damping effects properly.
Many users are familiar with the fact that data from Excel can be copied and pasted to the Tabular Data section of a load directly. Although many loads support the use of mathematical expressions, for more complex loading, users can define the load vs. time in Excel, then paste it directly into Mechanical.
One issue arises, however, when users are trying to change the actual time values. By default, when a step is added, the “Step End Time” is incremented by one. Consequently, when adding 40 steps, the default behavior is to have an ending time of 40. However, if a user tries to copy and paste “large” time values from Excel, it may not always work, as shown below:
Time must always increase; time can never decrease. Consequently, Mechanical performs a check to ensure that an input time value is not greater than a following time entry, If this condition fails, the input time entry is ignored. When inserting a column of data, the data is pasted from the top cell to the bottom cell in that order. So if a pasted entry has a following time less than the new time, that value is not registered. This explains why time values larger than the existing time values will not be pasted correctly.
The workaround to this is quite simple — prior to defining multiple steps, specify the “Step End Time” for the first step as a very large number. Then, when additional steps are added, they will all have a large number (recall that the default behavior is to increment the last time by one, as shown below.
Now, pasting a column of time values from Excel will behave as expected since the pasted values are less than the existing time values.