To create a step, do this
Module: Step Menu: Step, Create, OK
This opens a window (see screenshots below) where you give a name, like ApplyStrain, to the step. Also, you select the Procedure type, which could be:
Is used for linear and nonlinear incremental analysis.
One step linear analysis, or two-step for buckling eigenvalue/eigenmode extraction, vibration frequencies/modes, etc. See screenshot below.
Among the General procedures you choose one of these:
This is the most common. Static analysis that can be linear or nonlinear. The nonlinear algorithm is Newton-Raphson.
Nonlinear static analysis with Riks The nonlinear algorithm is Newton-Raphson.
Among the Linear Perturbation procedures you choose one of these:
Finds buckling load-multipliers (eigenvalues) and buckling mode shapes (eigenvectors).
Finds vibration frequencies and modes of vibration.
Static linear with several load cases possible.
Once you hit Continue, you get to Edit Step where you have 3 tabs (see screnshots) below.
and
It is important to understand these concepts:
(timePeriod). In a time dependent analysis such as viscoelastic analysis, it is the time in whatever units you are using for time, say seconds. In a nonlinear analysis without real time scale, such as plasticity, it is pseudo-time (no units). The time period is divided into increments.
Inc
initialInc It is the first increment. Must satisfy initialIncmaxInc
minInc
maxInc
If a load (or specified displacement ) is defined in Module: Load, each increment increments the load by
(5.1) |
Say you apply =0.30 mm to a bar of length L=15 mm, and you want to apply it gradually, during pseudo-time 0 to 2, with increments of 0.001 mm each, then
(5.2) |
and the volume-average strain in the bar is
(5.3) |
By setting timePeriod=2, the increments correspond to strain increments, i.e.,
(5.4) |
# create a Step Step = Model.StaticStep(timePeriod=float(ModelParameters['Strain']), initialInc=0.00001, minInc=0.00000001, maxInc=0.00001, maxNumInc=100000, name='ApplyStrain', previous='Initial')